DipTrace complete help

1.1. Introducing DipTrace

DipTrace PCB Design Environment includes four integrated modules:

DipTrace provides the following features:

Easy-to-learn user interface

DipTrace features an intuitive, unified interface that requires minimal learning. Design elements can be easily selected from libraries, placed, and linked visually and logically. All modules work seamlessly within a single environment, with integrated library management, schematic-to-PCB conversion, PCB updates from schematics, back-annotation, and synchronized navigation between PCB and schematic. Customizable hotkeys, various highlighting options, and a step-by-step tutorial help users get started quickly.

Smart manual and powerful automatic routing

DipTrace offers both intelligent manual routing and advanced automatic routing. Two automatic routers are available: the Grid Router, ideal for simple projects with jumper wires, and the Shape Router, a modern shape-based router with extensive settings and features, recognized as one of the best on the market today.

Interactive manual routing tools allow designers to create and edit tracks efficiently—pushing through existing traces, navigating around obstacles, and routing at 90°, 45°, 30°, 15°, or free angles. Various routing modes and segment types, smart highlighting, panning options, and length-matching tools further streamline the process. The software supports through, blind, and buried vias, unlimited board sizes, and provides real-time DRC to detect errors before they occur.

Multi-sheet and multi-level hierarchical circuit

The Schematic module supports multi-sheet and multi-level hierarchical design, making complex projects easier to manage. Each sheet can be converted into a hierarchy block, which can be inserted into the main sheet or nested within other blocks. In PCB Layout, components can be grouped into blocks directly on the board, allowing placement and routing to be applied automatically from one block to another.

High-speed signals and Differential pairs

DipTrace provides length-matching rules and flexible meanders for high-speed nets and buses. Differential pairs can be easily created and edited for low-noise, high-speed connections, with support for single- or double-track routing, phase tuning, and advanced routing constraints.

Smart project structure

DipTrace allows creating and managing layers, net classes, via styles, class-to-class rules, templates, and design rules. This flexible setup enables efficient organization and consistent management both within a single project and across multiple projects.

Advanced verification procedures

DipTrace provides comprehensive verification tools across Schematic and PCB design modules to ensure project accuracy at every stage. In the Schematic module, ERC identifies possible pin connection errors and guides designers through step-by-step corrections, while SPICE simulation allows verification of circuit behavior and performance before routing. In the PCB Layout module, DRC checks clearances, differential pair parameters, and minimum track and drill sizes, while real-time DRC reports errors immediately during routing, moving, or editing objects. Net Connectivity Check verifies that all PCB nets are electrically connected, using traces, copper pours, and shapes to detect broken or merged nets with detailed area reports. The Compare to Schematic function ensures that the routed PCB matches the source schematic.

Import/Export features

Exchange schematics, layouts, and libraries (DXF, Altium, Eagle, EasyEDA Pro, P-CAD, PADS, Pulsonix, OrCAD, KiCAD). DipTrace supports netlists of Accel, Allegro, Mentor, PADS, P-CAD, Protel and Tango formats. Import/Export STEP/IGES, VRML and 3DS files.

Manufacturing output

DipTrace offers comprehensive control over PCB layer stacks and supports export in popular manufacturing formats, including ODB++, Gerber RS-274X/Gerber X2, and Excellon N/C Drill. Exports can include TrueType fonts, Unicode symbols, and raster images. IPC-D-356A electrical test netlists and DXF files are also supported, with DXF serving as an intermediate format for generating G-Code for CNC drilling or milling machines.

Real-time 3D PCB preview with STEP/IGES and VRML 2.0 export

The 3D preview module lets you rotate the board on three axes, zoom in and out in real time, and adjust color settings. DipTrace supports *.wrl, *.step, *.iges, and *.3ds component models, with over 7,500 3D models available for free. STEP and VRML export enable fast and reliable exchange with mechanical CAD programs.

Simulation (SPICE)

The Schematic Capture and Component Editor lets users specify SPICE settings or attach SPICE models to components. Once a circuit is complete, the schematic can also be exported as a *.cir netlist for external simulation software.

Cross-module library management

DipTrace provides two dedicated modules for managing component libraries: Component Editor and Pattern Editor. Libraries are organized into standard, custom, and auto-generated groups for efficient design. Any changes made in one module are instantly reflected across all modules, ensuring consistency throughout the project.

Component libraries

DipTrace includes comprehensive component and pattern libraries with over 170,000 parts from various manufacturers. Users can also easily search for and save components from SnapEDA.

1.2. Formats

DipTrace package has four specific file formats:

1. PCB Design (*.dip) – can be created with PCB Layout module. It contains information about patterns (footprints), nets, traces, board, layers, shapes, texts, etc.

2. Schematic (*.dch) – can be created with Schematic module and opened in the PCB Layout. It contains information about components, wires, buses, shapes and schematic sheets. PCB Layout opens schematic file as component footprints (patterns) and logic connections between the pads.

3. Pattern library (*.lib) – can be created with Pattern Editor and opened with PCB Layout to place patterns, with Component Editor and Schematic – to attach patterns to components and with Pattern Editor – to create and edit patterns.

4. Component library (*.eli) – can be created with Component Editor. These files can be opened in the Schematic and PCB Layout to place components to the design/principal circuit.

Supported file formats:

1.3. DipTrace on the Web

DipTrace official website: https://www.diptrace.com

Order DipTrace: https://diptrace.com/buy/online-store

Tutorial: https://www.diptrace.com/books/tutorial.pdf

Tech. Support email: support@diptrace.com

Sales email: sales@diptrace.com

Forum: https://www.diptrace.com/forum

Facebook Page: https://www.facebook.com/DipTrace

Youtube Channel: https://www.youtube.com/channel/UCsShjGMkGNkPBSTEVjZMn3Q

2.1.1. Main window

Schematic's main window includes: the design area, the main menu, toolbars, the properties panel, Design Manager, Place Component panel and the status bar.

On the design area you can create and edit schematic objects (components, wires, buses, shapes, tables, etc.).

Access all common functions of the program in the main menu. There are the following items: File, Edit, View, Objects, Verification, Library, Tools, Help.

Other interface elements are:

Standard toolbar – tools to work with files, cut/copy/paste objects, print, preview and configure titles, change scale and grid size.

Objects toolbar – default mode, define origin, place components, find components, create and edit wires, buses, page connectors, differential pairs, hierarchy connectors and blocks, place images, shapes, text and tables.

Place Component panel – all standard libraries, user libraries or project components. Select library from the list, find and place component. Set up the library panel, search filters, multi-part component placement tools, symbol and pattern previews.

Properties panel displays the properties of current tool or selected object.

Design Manager navigates you through the schematic (left-click highlights object/s, double click pans the circuit to show selected component or net).

Status Bar shows (left to right) the current hint, mode, snap to grid status and cursor coordinates.

2.1.2. Toolbars

DipTrace Schematic has two instrument toolbars, component placement panel (left side), and the Design Manager (on the right):

Standard Toolbar

New – create a new schematic. If previously opened project is not saved, DipTrace will offer to do that. Only one schematic can be opened in one DipTrace instance, several files – only in several DipTrace Schematics (launched separately). Copy/Paste components between them.

Open – open existing schematic (*.dch) file.

Save – save current schematic into previously selected file. If project has never been saved, the Save as dialog box will pop up.

Print – print current schematic. It is recommended to print from the Preview dialog box. Sheet settings and titles are set in the Titles and Sheet Setup dialog box.

Preview – Preview dialog box pops up.

Titles and Sheet Setup – set sheet size, orientation, border margins, titles, zones in the Titles and Sheet Setup dialog box and edit information blocks in the Title block editor.

Cut – move selected object/s to the clipboard.

Copy – copy selected objects/s to the clipboard.

Paste – paste object/s from the clipboard.

Undo – one editing step backwards.

Redo – one editing step forward. Active only after using the Undo tool. If you edit schematic after using Undo tool, the Redo tool becomes inactive.

Zoom Window – with this tool active, hold down the left mouse button and draw the box to specify where to zoom on the design area.

Zoom Extents – pan schematic to show all objects.

Undo Zoom – return to the previous scale and panning.

Scale (drop-down box) – define schematic scale (from 25% to 800% or manually type in the value). Changing scale is possible with the mouse wheel, plus sign and minus sign default hotkeys and from the main menu.

Grid Size (drop-down box) – select current grid size from the drop-down list or type a new value in the box.

Objects Toolbar

Default Mode – enable default mode. Notice that you can switch to default mode with a right-click or Esc key.

Measure –  the ruler tool for measuring any sizes/distances directly on the design area.

Define Origin – define origin with the mouse pointer.

Place Component – Place Component dialog box.

Find Component – Search Component in all DipTrace libraries.

Place Wire – Place Wire tool.

Place Bus – Place Bus tool.

Place Bus Connector – place bus connectors to connect schematic sheets with a bus. To connect two or more bus connectors together, give them the same name.

Edit Mode – edit existing wires and buses. It is activated automatically when you try to edit wire or bus in the Default mode.

Define Differential Pair – create differential pair tool (define positive and negative nets of a pair, change color, net class and review pair properties).

Place Hierarchy Connector – this connector means pin (in/out) of the hierarchical block on a regular sheet.

Place Hierarchy Block – place hierarchical block on the sheet.

Place Table – place table to the schematic sheet.

Place Shape, Text, Picture – these tools allow the user to place the following objects: Line, Arc, Rectangle, Filled Rectangle, Obround, Filled Obround, Polyline, Filled Polygon, Text, Image.

2.1.3. Place Component panel

2.1.4. Design Manager

Design Manager panel is on the right side of the screen. Select "View \ Toolbars \ Design Manager" from the main menu or press default Ctrl+2 hotkeys to display/hide the panel. Design Manager consists of the Properties panel and the Design Manager itself to navigate through the schematic.

The Properties panel shows the properties of selected object or active tool and allows the designer to change them.

Right below is the Design Manager, it is the list of all project components (press the button) or nets (press ). Select component or net in the list, and all pins of selected object will appear in the list right below. Left-click in the list to highlight an object, or double click it in the list to pan the design area to selected object.

To adjust the width of the Design Manager panel, hover the mouse pointer over its edge, then drag and drop it.

2.1.5. Status Bar

Status bar is located in the bottommost part of the Schematic window.

It shows the following information:

Hint - standard hint containing information about the selected object on the design area.

Mode - shows the current mode (Default, Place Wire, Place Bus, etc.).

Grid Snap - the current Snap to Grid status.

X, Y - coordinates of the current position of the cursor or selected element.

2.1.6.1. File

New – create a new schematic. If previously opened project is not saved, DipTrace will offer to do that. Only one schematic can be open in one DipTrace instance, several files – only in several DipTrace Schematics (launched separately). Copy and paste components between them.

Open – open existing schematic (*.dch) file.

Open Recent – open last five schematic projects.

Save – save current schematic into previously selected file. If project has never been saved, the Save as dialog box will pop up. This tool is active only if current schematic has unsaved changes.

Save as – specify the filename and location where schematic file will be saved.

Save Selected As – save selected objects into a separate (*.dch) file.

Import – import schematic from DipTrace ASCII, DipTrace XML, Altium ASCII, P-CAD ASCII, P-CAD PDIF, PADS SCH ASCII 2005, OrCAD EDIF, Eagle XML and KiCAD Schematic formats.

Export – export schematic to DipTrace ASCII, DipTrace XML, P-CAD ASCII, DXF, Eagle XML; DipTrace creates netlists of various formats, Spice netlist for external simulation and Bill of Materials.

Titles and Sheet Setup – open Titles and Sheet Setup dialog box to set sheet size and orientation, border margins, titles etc. Launch the Title Block Editor from this menu item to create custom title blocks.

Preview – open the Preview dialog box before printing.

Print – print current schematic as it is. We recommend to print from the Preview dialog box. Sheet settings and titles are customized in the Titles and Sheet Setup dialog box.

Schematic Information – general information about current circuit (number of pins, parts, components, nets, sheets).

Convert to PCB – open current schematic in the PCB Layout.

Back Annotate – update RefDes, Value, component names, net names, and net classes from the PCB file.

Recover Schematic – recover the latest project. The function is useful if DipTrace closed incorrectly or if the project was not properly saved. DipTrace automatically saves every 10 editing steps.

Recovery Options – configure recovery options: turn ON/OFF recovery and change the number of steps remembered.

Exit – close the Schematic. If current project was not saved, the software will offer to save it.

2.1.6.2. Edit

Undo – one editing step backward.

Redo – one editing step forward. It is active only after using the Undo tool. If you edit schematic after using the Undo, Redo tool becomes inactive.

Undo/ Redo Zoom – select if to consider Zoom a separate editing step or not.

Cut – move selected object/s to the clipboard.

Copy – copy selected object/s to the clipboard.

Paste – paste object/s from the clipboard.

Delete – delete selected object/s.

Select All – select all objects of the schematic.

Edit Selection – selecting objects by type and properties. Different selection modes available: new selection, add to selection, remove from selection, keep selected.

Cross Selection - enable cross selection between Schematic Capture and PCB Layout, choose objects and actions to be included in this function.

Find in Schematic – find specific component or net on the schematic. Search by name, RefDes, value, pattern, etc.

Add Sheet – add new blank sheet to the schematic.

Sheet Type – select whether current sheet is normal or hierarchical.

Copy Matrix – create a copy matrix, based on selected objects. It is possible to specify the number of rows, columns and row/column spacings.

Rotate – rotate selected object/s 90 degrees counter-clockwise. If objects form a group, they have a common center of rotation, otherwise, each has its own center of rotation.

Rotate Group – rotate selected objects around one common center point.

Flip Group – flip selected objects vertically and horizontally.

Align Objects – align selected objects horizontally or vertically and distribute them equally.

Group – unite all selected objects into a group. This tool is active only if several objects are selected.

Ungroup – ungroup selected objects. This tool is active only if one or more groups are selected.

Lock Selected – lock moving and editing of all selected objects.

Unlock Selected – unlock moving and editing of all selected objects, if they were previously locked.

Properties – open the Properties dialog box for selected object.

2.1.6.3. View

Toolbars – show/hide the toolbars.

Display Hint – display hint for the objects on the design area. Hint is duplicated in the bottom-left corner of the screen on the status bar.

Part Preview – preview component before placing it on the schematic.

Group Similar Parts – similar parts of multi-part component are shown with a single item in the part selection list on the Place Component panel. If this option is active, one of similar parts is selected automatically, based on existing parts of the schematic.

Part Markings – default Part Marking options.

Pin Numbers – show/hide the pin numbers and select their font size.

Move Part Text – use this tool to move component markings.

Connection to Bus – set up the markings of wire-to-bus connections. There are two modes: Net Name – net name is shown, Net Number in Bus – net number in the bus is shown (each bus has its own net numeration). Marking text position and font can be changed.

Net Names – set Vector or TrueType font and choose the desired size. This selection will apply to all net names, except those with custom settings.

Hide Power and Gnd – show/hide Power or Ground parts and nets.

Display Titles – show/hide titles. Sheet settings and titles are set in the Titles and Sheet Setup dialog box.

Display Sheet – show/hide the sheet. Sheet size is set in the Titles and Sheet Setup dialog box.

Scale – define schematic scale (from 25% to 800% or type in a new value). Changing the scale is also possible with the mouse wheel or the Plus sign (+) and Minus sign (-) default hotkeys.

Line Width – change the line width of the wires, buses, tables, titles and set diameter of wire nodes.

Colors – change the color template of the design area and its elements.

Graphics Mode – change the graphics mode of the design area.

Units – change units of measurement (mm, mil, or inches).

Precision – adjust precision rate for project values and the grid.

Display Origin – show/hide the origin.

Define Origin – define origin with the mouse pointer or by coordinates (incremental to existing origin).

Grid – show/hide the grid.

Snap to Grid – enable/ disable snap to grid, when the grid is on.

Grid Size – grid size submenu. Select from different standard and custom sizes.

Customize Grid – add/edit standard grid sizes.

2.1.6.4. Objects

Place Component – Place Component dialog box.

Find Component – Search Filters dialog box.

Search Parts at SnapEDA – search SnapEDA libraries directly from within DipTrace.

New Part Request – place an order to get the required part designed within 24 hours.

Circuit – place wire, bus, bus connector to the schematic or enable the Edit mode for existing wires and buses.

High Speed – define differential pair tool and Differential Pair Manager.

Hierarchy – place hierarchical connectors and blocks.

Net Classes – add/edit/delete net classes to the project. More settings available only in the PCB Layout.

Load Classes – load net classes from previously saved rule file (*.rul) or directly from any layout file (*.dip). 

Connection Manager – Connection Manager dialog box.

Place Table – place table to the schematic.

Place Shape – place a shape (line, arc, rectangle, filled rectangle, obround, filled obround, polyline, filled polygon).

Place Text – add a text object to the schematic.

Place Picture – add an image to the schematic.

Drawing properties – change default color and line width for shapes and select default font for text objects. Shapes, pictures and text objects in general are considered as shapes.

Measure – the ruler tool for measuring any sizes/distances directly on the design area.

2.1.6.5. Verification

Electrical Rule Check (ERC) – verifies electrical rules for current schematic and shows errors if there are some.

Electrical Rule Setup – change electrical rules in the dialog box.

Check Hierarchy – hierarchy verification, displays errors in the hierarchy tree structure (closed loops).

2.1.6.6. Library

Library Setup – library setup dialog box allows for complete setup of component placement panel: add/delete component library groups, sort them, and add/delete certain libraries and folders to/from the library groups.

Copy <Library name> Library to another group – copy selected library (selected in the list on the Place Component panel) to another library group.

Open <Library name> Library in Component Editor – open current library (selected in the list on the Place Component panel) in the Component Editor

Add Library to <Library group> – add selected library to current library group.

Move <Library name> Library to Another group – move selected library to another library group.

Remove <Library name> Library from <Library group> – remove selected library from current library group.

Add project libraries from another project – add all libraries from another DipTrace file.

Save Design Cache as library – save auto-generated (virtual) Design Cache library as a regular library.

Clear Design Cache – remove all components from the Design Cache library (does not change the project itself).

Remove <Component name> from the Design Cache – remove selected component from the Design Cache library.

2.1.6.7. Tools

SPICE simulator – launch built-in NGSPICE simulator to check the integrity of your circuit and its behaviour.

RefDes Renumbering – arrange reference designators automatically from the top-left to the bottom-right by rows or by columns.

Component Suppliers – launch Suppliers and Prices from Octopart dialog to check prices and availability of parts for your design from different suppliers.

Plugins - extend the software functionality by running plugins. Comprehensive documentation and plugin examples with source codes are provided.

HotKey Settings – check and customize hotkeys for various tools, actions, and dialog boxes in the Schematic.

Environment Variables  – define and manage environment variables.

PCB Layout – launch PCB Layout module.

Component Editor – launch Component Editor module.

Pattern Editor – launch Pattern Editor module. 

2.1.6.8. Help

Schematic Help – Schematic Help file.

DipTrace Tutorial – DipTrace PDF step-by-step tutorial, learn how to work in DipTrace on the example circuit.

Getting Started – getting started dialog box with useful software links.

Register – enter the User Name and Registration Key to register your DipTrace edition.

Request Support – DipTrace support portal.

PCB Design Service – request affordable PCB design service from our experienced engineers (online request form).

DipTrace Home Page – DipTrace official website.

About – general information (current version, edition, and software build).

2.1.7.1. Component

Right-click on a component to open this submenu:

Component RefDes – change RefDes of the component. Current RefDes is an item caption.

Optimize RefDes – renumber RefDes of the components to optimize numbers (if some components were previously deleted or renamed).

RefDes Renumbering – arrange reference designators from the top-left to the bottom-right by rows or by columns.

Links – display all links from component's additional fields.

Block Subcircuit – open hierarchy block circuit. Item is visible only for hierarchical blocks.

Lock Selected – lock moving and editing of all selected objects.

Unlock Selected – unlock moving and editing of all selected objects, if they were previously locked.

Disconnect Wires – disconnect all component pins from the wires.

Connect Wires – connect component pins to the wire ends located in the same grid point on the design area.

Attached Pattern – attach pattern to the component. You can attach pattern by selecting it from the pattern library and changing pin numbers.

Pad Signal Delay – define any additional distance that a signal propagates within a component. This value is considered for phase and length tuning.

SPICE Model – open SPICE Model dialog to set up or edit the model of the current component or all the components of the schematic that will be used for simulation.

SPICE: Show Current  – open NGSPICE Simulator window with the signal trace displayed on the graph (based on the results of a previously-run simulation).

Replace Part – replace current part with another part from component library.

Save to library – save component into a library file or active library.

Price and Availability – check component price and availability from a featured supplier or all the suppliers from Octopart catalog.

Update from library – update selected parts, components or component type from the library.

Pin Numbers – show/hide pin numbers for selected parts.

Part Origin – show/hide the origin of selected component.

Rotate – rotate selected objects 90 degrees counter-clockwise. If objects form a group, they have a common center of rotation, otherwise, each has its own center of rotation.

Flip – flip component horizontally or vertically.

Change Sheet – move part to selected sheet (if circuit has more than one sheet).

Align Objects – align selected objects horizontally or vertically and distribute them equally.

Snap to Grid – snap selected component to the grid, when the grid is on, but Snap to Grid option is disabled for the overall project.

Cut – move selected object to the clipboard.

Copy – copy selected objects to the clipboard.

Delete – delete selected objects.

Group – unite all selected objects into a group. Tool is active only if several objects are selected.

Ungroup – ungroup selected objects. This tool is active only if one or more groups are selected.

Properties – component properties dialog box.

2.1.7.2. Pin

Right-click on the pin to open this submenu.

Pin Name – change pin name. To start/finish inversion, use the tilde sign key.

Net Name – change net name dialog box. Item is visible if this pin belongs to some net.

Not connected – put "not connected" declaration on the pin. Not connected pin is not considered as an error by ERC if Not Connected option is turned ON.

Delete from Net – delete current pin from the net.

Display Wire – display wire connected to the pin. Item is visible only if wire was hidden.

Add to Net – add current pin to net from the list.

Connection Manager – Connection Manager for the circuit.

Signal Delay –  set pin signal delay.

Net Properties – net properties dialog box for the net connected to selected pin.

Pin Properties – pin properties dialog box to change all pin properties and font of pin name.

2.1.7.3. Net

Right-click on a wire to open this submenu:

Net Name – change name of the net. Current name is an item caption.

Display Name – show net name in the design area (separate text object).

Direction Arrows – display direction arrows for selected wires.

Wire Color – change color of the net wire.

Lock Selected – lock moving and editing of all selected objects.

Unlock Selected – unlock moving and editing of all selected objects if they were previously locked.

Add Node – add node to the wire segment.

Hide Wire – hide current wire. All pins that belong to this wire will be connected without wires.

Bus Connection – re-connect wire to the bus. The item is available only for wires connected to buses.

Number in Bus – change net number in the bus. Item is visible if "View \ Connection to Bus \ Net Number in Bus" main menu option is checked.

Connection Manager – launch the Connection Manager.

SPICE: Show Voltage –  open NGSPICE Simulator window with the signal trace displayed on the graph (based on the results of a previously-run simulation).

Delete Line – delete wire segment.

Delete Wire – delete wire. Net structure is changed.

Change Sheet – move net to selected sheet (if the circuit has more than one sheet). Net can not be moved if it is connected to non-moving objects.

Snap to Grid – snap the selected net of the pair to the grid, when the grid is on, but Snap to Grid option is disabled for the overall project.

Snap to Grid – snap the selected net to the grid, when the grid is on, but Snap to Grid option is disabled for the overall project.

Cut – move selected object to the clipboard.

Copy – copy selected objects to the clipboard.

Delete – delete selected objects.

Group – unite all the selected objects to a group. This tool is active only if several objects are selected.

Ungroup – ungroup the selected objects. This tool is active only if one or more groups are selected.

Properties – Net Properties dialog box.

2.1.7.4. Differential pair

Right-click on a differential pair wire to open this submenu:

Diff Pair Name – change differential pair name. Current name is an item caption.

Display Name – show differential pair name on the design area (separate text object).

Direction Arrows – display signal direction arrow for selected wire.

Diff Pair Color – change color of the differential pair.

Lock Selected – lock moving and editing of all selected objects.

Unlock Selected – unlock moving and editing of all selected objects if they were previously locked.

Add Node – add node to wire segment.

Hide Wire – hide current wire. All pins belonging to this wire will be connected without wires.

Bus Connection – re-connect wire to the bus. The item is available only for wires connected to buses.

Number in Bus – change net number in the bus. Item is visible if "View \ Connection to Bus \ Net Number in Bus" main menu option is checked.

Connection Manager – launch the Connection Manager.

Delete Line – delete wire segment.

Delete Wire – delete wire. Net structure is changed.

Remove Diff Pair – remove differential pair declaration from the nets of the pair. The nets remain.

Change Sheet – move selected net of the pair to another sheet (if circuit has more than one sheet). Net can not be moved if it is connected to non-moving objects.

Cut – move selected object to the clipboard.

Copy – copy selected objects to the clipboard.

Delete – delete selected objects.

Group – unite all selected objects to a group. This tool is active only if several objects are selected.

Ungroup – ungroup selected objects. This tool is active only if one or more groups are selected.

Properties – Differential Pair Properties dialog box.

2.1.7.5. Bus

Right-click on a bus to open this submenu.

Bus Name – change the name of the bus. Current name is an item caption.

Display Name – show bus name on the design area (separate text object).

Lock Selected – lock moving and editing of all selected objects.

Unlock Selected – unlock moving and editing of all selected objects, if they were previously locked.

Add Node – add node to the bus segment.

Delete Line – delete bus segment.

Delete Wire – delete bus line. Bus structure is changed if necessary.

Change Sheet – change current sheet of selected bus.

Snap to Grid – snap the selected bus to grid, when the grid is on, but Snap to Grid option is disabled for the overall project.

Cut – move selected object to the clipboard.

Copy – copy selected object/s to the clipboard.

Delete – delete selected objects.

Group – unite all selected objects to a group. This tool is active only if several objects are selected.

Ungroup – ungroup selected objects. This tool is active only if one or more groups are selected.

Bus Nets – list of the bus nets. Here you can delete nets from the bus if necessary.

2.1.7.6. Bus connector

Right-click on a bus connector to open this submenu.

Bus Connector Name – change the name of the bus connector. Current name is an item caption. Busses connected to connectors with similar names are automatically merged.

Lock Selected – lock moving and editing of all selected objects.

Unlock Selected – unlock moving and editing of all selected objects, if they were previously locked.

Change Sheet – change current bus connector sheet.

Align Objects – align selected objects horizontally or vertically and distribute them equally.

Snap to Grid – snap selected bus connector to the grid, when the grid is on, but Snap to Grid option is disabled for the overall project.

Cut – move selected object/s to the clipboard.

Copy – copy selected object/s to the clipboard.

Delete – delete selected object/s.

Group – unite all selected objects into a group. This tool is active only if several objects are selected.

Ungroup – ungroup selected objects. This tool is active only if one or more groups are selected.

2.1.7.7. Shape

Right-click on a shape, text, or picture to open this submenu:

Shape Name – change the shape name or the text.

Edit Text  – change the text. Object size is changed automatically.

Font Type – choose font type of a text object (Vector, TrueType). Unicode characters are supported in TrueType mode only.

Font – change font settings (size, text width, line width) of a text object.

Lock Selected – lock moving and editing of selected objects.

Unlock Selected – unlock moving and editing of selected objects, if they were previously locked.

Insert Point – insert point to the polyline or polygon.

Delete Point – delete point from the polyline or polygon.

Rotate – rotate selected objects 90 degrees counter-clockwise. If objects form a group, they have a common center of rotation, otherwise, each has its own.

Change Sheet – change current sheet (move shape to another schematic sheet).

Align Objects – align selected objects horizontally or vertically and distribute them equally.

Snap to Grid – snap the selected shape to grid, when the grid is on, but Snap to Grid option is disabled for the overall project.

Cut – move selected object/s to the clipboard.

Copy – copy selected object/s.

Delete – delete selected object/s.

Group – unite all selected objects to a group. This tool is active only if several objects are selected.

Ungroup – ungroup selected objects. This tool is active only if one or more groups are selected.

Font Type – choose the font type for the text object (Vector, TrueType). Unicode is supported only in the TrueType mode.

Font – change text font. It is active only for the text objects.

Properties – change Shape Properties.

2.1.7.8. Table

Right-click on the table to open this submenu.

Name – change table name. Current name is the item caption.

Current Cell – change properties of current table cell (size, text, align, font).

Lock Selected – lock moving and editing of selected objects.

Unlock Selected – unlock moving and editing of selected objects, if they were previously locked.

Column Width – change column width.

Row Height – change row height.

Add Column – add new column to the table.

Add Row – add new row to the table.

Insert Column – insert new column.

Insert Row – inserts new row.

Delete Column – delete current column from the table.

Delete Row – delete current row from the table.

Save to File – save table content to Excel CSV or Text file.

Rotate – rotate selected objects 90 degrees counter-clockwise. If objects form a group, they have a common center of rotation, otherwise each has its own center of rotation.

Change Sheet – move table to another sheet.

Align Objects – align selected objects horizontally or vertically and distribute them equally.

Snap to Grid – snap the selected table to grid, when the grid is on, but Snap to Grid option is disabled for the overall project.

Cut – move selected object/s to the clipboard.

Copy – copy selected object/s.

Delete – delete selected object/s.

Group – unite all selected objects into a group. This tool is active only if several objects are selected.

Ungroup – ungroup selected objects. This tool is active only if one or more groups are selected.

Properties – change table properties.

2.1.8. Modes of operation

There are several modes of operation in the DipTrace Schematic:

Default mode – set by default. It becomes active as soon as you launch the Schematic. To activate this mode from any other mode, you need to right-click on empty space on the design area (maybe several times). Esc key or button on the Objects toolbar can be used as well. This mode allows the user to select and move objects as well as place wires, edit existing wires, and change size of shapes, texts, and pictures by automatically switching to necessary operational mode after clicking on the object.

Measure mode. Select measuring tool from the main menu ("Objects/ Measure") or press on the Objects toolbar. Left-click in the starting point and move the mouse pointer to the end point keeping left button pressed. The length will be displayed in the bottom-left corner, in the hint area.

Define Origin mode. Select Define Origin tool from the main menu  (View/ Define Origin/ By Mouse Pointer)  or press on the Objects toolbar. Left-click in the design area to establish a new Origin point.

Place Component – select component in the component list on the Place Component panel or press Place button in the Place Component dialog box to enable this mode.

Place Table – select "Objects \ Place Table" from the main menu or press button on the Objects toolbar.

Place Wire – select "Objects \ Circuit \ Place Wire" from the main menu, press button on the Objects toolbar, or simply left-click on the pin to enable this mode. Select the first pin or wire segment, then draw it to the final pin or wire segment, and left-click it. It is possible to place wire automatically or segment by segment.

Place Bus – select "Objects \ Circuit \ Place Bus" from the main menu or press button on the Objects toolbar. To place bus, select the start point, bus segment, or bus connector, and specify the key points of the bus all the way to the final bus segment or bus connector with the left mouse clicks. Right-click, and choose Enter from the submenu to apply.

Place Bus Connector – select "Objects \ Circuit \ Place Bus Connector" from the main menu or press button on the Objects toolbar. To place bus connector, just left-click on the design area. Give similar names to several bus connectors to connect them. All buses will be united automatically.

Edit Wires and Buses – select "Objects \ Circuit \ Edit Mode" from the main menu, press button on the Objects toolbar or simply drag and drop. This mode allows the designer to move wire segments and bus segments orthogonally.

Place Shape – select shape or text placement tool from the main menu ("Objects") or button on the Objects toolbar.

Place Text mode. Select text placement tool from the main menu (Objects/ Place Text) or press  button. Left-click on the design area and type a text. DipTrace supports multi-line text placement. Select Edit Text item from the right-click submenu to change the text, line spacing and alignment. Use Text Properties dialogue, launched by selecting Properties item from the right-click submenu, to adjust other text properties: font, layer, text angle, anchor point location, etc. 

Move Part Markings – select "View \Move Part Texts" from the main menu or press F10 default hotkey. Press R or Space to rotate texts while moving, just like regular objects.

2.1.9. Hotkeys

DipTrace features customizable hotkeys in all software modules. To open the Hotkey Settings dialog box, proceed to "Tools/ Hotkey Settings" from the main menu in any of the DipTrace modules: Schematic, PCB Layout, Component and Pattern Editors. The designer can view or assign hotkeys to various tools, actions and dialog boxes by left clicking in a corresponding field and pressing a keyboard combination.

If a combination is already in use, a warning message comes out. Notice that certain shortcuts are reserved by the program and are not customizable. Press OK to apply changes. To restore default configuration, press Set Default Hotkey Configuration button on the panel.

Hotkeys reserved by the system:

Please notice that most items in the main menu and various drop-down lists have shortcut combinations right next to them. In this help document we always refer to default shortcuts.

2.1.10. Environment Variables

According to DipTrace License Policy, the software can be used by one license holder on several devices. To ensure smooth portability of your projects, DipTrace features an Environment Variables tool that allows setting variables for the paths to directories containing libraries, 3D models, images, etc. on different machines.

Go to Tools/ Environment Variables to open the Environment Variables dialog.

In the Common Variables section you can see the paths used by the software during installation and the corresponding variables for those paths.

In the User Variables part you can establish new variables for the paths to the directories, where your libraries or 3D models are stored. Type the variable in the Variable cell and set the path in the Folder line or press button and select Browse for Folder to select the directory. Use the same variable on another PC to associate it with the path to the required folder on that machine. In this way when switching between machines the software will look for the files using the path corresponding to the established variable on the given PC.

You can check the Auto Replace option for the software to substitute the path with the variable in any items with such path as soon as they appear in the project or press button and select “Replace folder with  %variable name%” to apply this command to all currently existing items in the project. To reverse the command select “Replace %variable name% with Folder” from the menu.

Remember to use the same variables to set the paths to the corresponding folders on another machine. If your component or 3D model libraries have been changed, make sure to update them in the source folder on your device.  

To delete a variable press and select Delete <Variable Name>.

Environment Variables feature also allows creating a portable version of the program by establishing a variable for the launch directory, which can be stored, for instance, on a portable drive.

2.2.1. Create project

If you launch DipTrace (no command prompt), a new project will be created automatically. To create a new project, select "File \ New" from the main menu or press the corresponding button on the Standard toolbar. If current project is not saved, the program will offer to do this.

2.2.2. Open project

Select "File \ Open" from the main menu or press the corresponding button on the Standard toolbar to open schematic file and choose the file you need (*.dch).

The last five files are saved in the "File \ Open Recent" submenu for quick access.

2.2.3. Save project

It is possible to save the project by choosing "File \ Save" or "File \ Save as" from the main menu. For the first item there is a tool on the Standard toolbar.

To save project, select "File \ Save" from the main menu or press the corresponding button on the Standard toolbar. If schematic has never been saved, the Save As dialog box will pop up automatically. The user should select the location and file name for the schematic, all further changes will be automatically rewritten into this file.

If you need to save only a part of your schematic, select it, and go to "File \ Save Selected As" from the main menu.

2.2.4. Schematic to PCB

To convert existing schematic to PCB Layout, select "File \ Convert to PCB" from the main menu. You can also save your schematic and open a *.dch file directly in the PCB Layout.

When you open schematic in the PCB Layout, DipTrace suggests to use schematic rules or load rules from another layout project (layers, DRC, net classes, via styles etc.). You can also arrange components for easier placement. Choose "Placement \ Arrange Components" from the main menu in the PCB Layout.

2.2.5. Back Annotate

Back annotate feature allows the user to automatically apply changes made in the PCB Layout directly on the principal circuit in the Schematic.

This feature has limited functionality (only updates the reference designators, values and types of components, net names, and net classes) and is not capable to add new components or create new nets on the principal circuit.

We always recommend that any changes should be made in the schematic first. Back Annotation does not work if schematic or PCB layout has been created in different PCB CAD software.

To launch the back annotation for existing schematic, select "File \ Back Annotate" from the main menu, then select the PCB layout file (*.dip).

Back annotation of the names does not work for multiple hierarchical blocks (if any hierarchical sheet was placed more than once). In this case names on the PCB and Schematic will be different (R1 in Schematic will be R1_1, R1_2, etc. in the PCB Layout, due to hierarchy block index in the component RefDes on the board).

2.2.6.1. DipTrace ASCII

DipTrace allows the user to save/open data in the textual ASCII format. This format has been developed to allow for data transferring from/to other EDA packages and for forward compatibility.

To import schematic file from DipTrace ASCII format, select "File \ Import \ DipTrace ASCII", choose a file, and click Import.

2.2.6.2. DipTace XML

DipTrace Schematic Capture allows saving/ opening data in the textual DipTrace XML format. This format can be used for data transferring from/to other EDA packages and for forward compatibility between the DipTrace versions.

To import a library file in DipTrace XML format, select "Library/ Import/ DipXML" then select file, and click OK.

2.2.6.3. Altium ASCII

DipTrace imports schematics from the Altium ASCII (*.schdoc) format.

Notice that your schematic should be in the ASCII format, not binary (save schematic as an ASCII file in the Altium software).

In the DipTrace select "File \ Import \ Altium ASCII" from the main menu and open Altium ASCII schematic file. The following dialog pops up:

Schematics include only pattern names, you need to specify where to get the pattern libraries to proceed. Use Add and Delete buttons to add pattern libraries to the list. With Shift or Ctrl keys several libraries can be added at a time.

We recommend importing your Altium ASCII pattern libraries (*.lia) in the Pattern Editor prior to importing schematic or PCB files from Altium, but you can also find patterns in the DipTrace libraries. Use Pattern Names Help to quickly find acceptable component footprints in DipTrace standard libraries because pattern names may be different.

Press Assign all Patterns by names – patterns will be found and attached automatically. Check all patterns yourself, use File Components list and the preview field below.

File Components list

RefDes – Altium component reference designator;

Name – Altium component name;

Pattern Name – Altium pattern name;

Pattern – related DipTrace pattern.

Select component in the list, then select pattern from the library, and press Attach to Component button to attach patterns to components according to component RefDes, name or pattern name.

The star symbol (*) after the pattern name in the list means that this pattern had been connected manually.

You can also import Altium schematic without patterns.

2.2.6.4. Eagle Schematic

DipTrace imports schematics from the EAGLE format (*.sch).

Select "File \ Import \ EAGLE Schematic" from the main menu in the DipTrace Schematic, and select an EAGLE schematic file (*.sch).

Components and patterns are included into EAGLE schematic and PCB files, you don't have to connect patterns when importing from EAGLE. All components of an imported project are available in the auto-generated Design Cache library in the Project Libraries library group on the Place Component panel. You can save Design Cache as a regular library directly on the Place Component panel or import component and pattern libraries from EAGLE in DipTrace Component Editor and DipTrace Pattern Editor.

2.2.6.5. EasyEDA Pro

DipTrace supports import of schematics from EasyEDA Pro format (*.epro).

Choose "File \ Import \  EasyEDA Pro" from the main menu in the DipTrace Schematic, and select  EasyEDA Pro Project file (*.epro).

2.2.6.6. P-CAD ASCII

DipTrace imports schematics from the P-CAD ASCII (*.sch) format.

Notice that your schematic should be in the ASCII format, not binary (both have the same extension in P-CAD).

Select "File \ Import \ P-CAD ASCII" from the main menu and open schematic file. The following dialog pops up:

Schematics include only pattern names, you need to specify where to get the pattern libraries to proceed. Use Add and Delete buttons to add pattern libraries to the list. With Shift or Ctrl keys several libraries can be added at a time.

We recommend importing your P-CAD ASCII pattern libraries (*.lia) in the Pattern Editor prior to importing schematic or PCB files from P-CAD, but you can also find patterns in the DipTrace libraries. Use Pattern Names Help to quickly find acceptable component footprints in DipTrace standard libraries because pattern names may be different.

Press Assign all Patterns by names – patterns will be found and attached automatically. Check all patterns yourself, use File Components list and the preview field below.

File Components list

RefDes – P-CAD component reference designator;

Name – P-CAD component name;

Pattern Name – P-CAD pattern name;

Pattern – related DipTrace pattern.

Select component in the list, then select pattern from the library, and press Attach to Component button to attach patterns to components according to component RefDes, name or pattern name.

The star symbol (*) after the pattern name in the list means that this pattern had been connected manually.

You can also import P-CAD schematic without patterns.

2.2.6.7. P-CAD PDIF

DipTrace Schematic module allows the user to import P-CAD PDIF files.

Select "File \ Import \ P-CAD PDIF" from the main menu, then select *.pdf or *.cfg file of a P-CAD Schematic. *.cfg files are used for multi-sheet schematics.

Notice that P-CAD has separate *.pdf file for each sheet and *.cfg file to unite all schematic sheets together. DipTrace has a single *.dsc file for single or multi-sheet schematics.

You can import schematic without patterns.

Notice that importing P-CAD PDIF schematic does not differ from importing other formats. See P-CAD ASCII import page for basic instructions.

Use Pattern Names Help to quickly find acceptable component footprints in DipTrace standard libraries.

2.2.6.8. PADS ASCII 2005

DipTrace imports schematics from the PADS Schematic ASCII 2005 (*.txt) format. Select "File \ Import \ PADS SCH ASCII 2005" from the main menu and open a schematic file. The following window pops up:

PADS schematics include only pattern names, you need to specify where to get the pattern libraries to proceed. Use Add and Delete buttons to add pattern libraries to the list. With Shift or Ctrl keys several libraries can be added at a time.

We recommend importing your PADS ASCII pattern libraries (files with *.d and *.c extensions) in the Pattern Editor prior to importing schematic or PCB files from PADS, but you can also find patterns in the DipTrace libraries. Use Pattern Names Help to quickly find acceptable component footprints in DipTrace standard libraries because pattern names may be different.

Press Assign all Patterns by names – patterns will be found and attached automatically. Check all patterns yourself, use File Components list and the preview field below.

File Components list

RefDes – PADS component reference designator;

Name – PADS component name;

Pattern Name – PADS pattern name;

Pattern – related DipTrace pattern.

Select component in the list, then select pattern from the library, and press Attach to Component button to attach patterns to components according to component RefDes, name or pattern name.

The star symbol (*) after the pattern name in the list means that this pattern had been connected manually.

You can also import PADS schematic without patterns.

2.2.6.9. OrCAD EDIF

DipTrace imports schematics from the OrCAD EDIF format.

Select "File \ Import \ OrCAD EDIF Schematic" from the main menu and open schematic file (file with *.edf extension). The following window pops up:

OrCAD schematics include only pattern names, you need to specify where to get the pattern libraries to proceed. Use Add and Delete buttons to add pattern libraries to the list. With Shift or Ctrl keys several libraries can be added at a time. Use Pattern Names Help to quickly find acceptable component footprints in DipTrace standard libraries because pattern names may be different.

Press Assign all Patterns by names – patterns will be found and attached automatically. Check all patterns yourself, use File Components list and the preview field below.

File Components list

RefDes – OrCAD component reference designator;

Name – OrCAD component name;

Pattern Name – OrCAD pattern name;

Pattern – related DipTrace pattern.

Select component in the list, then select pattern from the library, and press Attach to Component button to attach patterns to components according to component RefDes, name or pattern name.

The star symbol (*) after the pattern name in the list means that this pattern had been connected manually.

You can also import OrCAD schematic without patterns.

2.2.6.10. KiCAD Schematic

DipTrace imports schematics from the KiCAD Schematic format.

Select "File \ Import \ KiCAD Schematic" from the main menu and open schematic file (file with *.pro extension). The following window pops up:

KiCAD schematics include only pattern names and you need to specify where to get the pattern libraries to proceed. Use Add and Delete buttons to add pattern libraries to the list. With Shift or Ctrl keys several libraries can be added at a time. Use Pattern Names Help to quickly find acceptable component footprints in DipTrace standard libraries because pattern names may be different.

Press Assign all Patterns by names – patterns will be found and attached automatically. Check all patterns yourself, use File Components list and the preview field below.

File Components list

RefDes – KiCAD component reference designator;

Name – KiCAD component name;

Pattern Name – KiCAD pattern name;

Pattern – related DipTrace pattern.

Select component in the list, then select pattern from the library, and press Attach to Component button to attach patterns to components according to component RefDes, name or pattern name.

The star symbol (*) after the pattern name in the list means that this pattern had been connected manually.

You can also import KiCAD schematic without patterns.

2.2.6.11. Pulsonix

DipTrace supports import of schematics from Pulsonix format (*.psa).

Choose "File \ Import \ Pulsonix" from the main menu in the DipTrace Schematic, and select Pulsonix schematics file (*.psa).

2.2.7.1. DipTrace ASCII

DipTrace allows you to save/open data in textual ASCII format. This format has been developed to allow for data transferring from/to other EDA packages and for forward compatibility.

To export schematic file into DipTrace ASCII format, select "File \ Export \ DipTrace ASCII", define the filename, and press OK.

2.2.7.2. DipTace XML

DipTrace Schematic Capture allows saving/ opening data in the textual DipTrace XML format. This format can be used for data transferring from/to other EDA packages and for forward compatibility between the DipTrace versions.

To export a schematic file in DipTrace XML format, select "Library/ Export/ DipXML" then define filename, and click OK.

2.2.7.3. DXF

DipTrace allows for exporting schematic to DXF format accepted by almost all PCB CAD programs. Select "File \ Export \ DXF" from the main menu. The following window pops up automatically:

Select schematic sheet for exporting and enable/disable text, tables, and titles in the DXF file. Other objects will be exported as they are. Change coordinate offset or use the design origin. Press Export and define the filename to complete the export process or press Cancel to reject it.

2.2.7.4. P-CAD ASCII

DipTrace allows the user to export Schematics to P-CAD ASCII format (files with *.sch extension).

To export existing schematic to P-CAD, select "File \ Export \ P-CAD ASCII" from the main menu, define the filename and save it.

2.2.7.5. Netlist

DipTrace allows the designer to export schematic's netlist in the most popular netlist formats. Netlists allow for transferring the source data to various board design applications. DipTrace exports netlists of these formats: Accel, Allegro, KiCAD, Mentor, OrCAD, PADS, P-CAD, Protel 2.0, Tango.

To export a netlist, select "File \ Export \ Netlist" and choose appropriate netlist format. In the pop-up dialog box, define the filename for the netlist, and press OK.

2.2.7.6. Eagle Schematic

DipTrace allows the user to export Schematics to Eagle Schematic format (files with *.sch).

Please note that in DipTrace, both Pin Name and Pin Number can be assigned to a pin, while in Eagle a pin is denominated only with a Pin Name. When exporting DipTrace Schematic to Eagle format, Pin Name, if assigned in the source file, is carried over to Eagle. However, if no Pin Name is assigned in the original project, Pin Number is carried over to Eagle as a Pin Name.

Pin Number display is configured for all pins of all components via View/ Pin Numbers item (in Eagle: Pin Settings - Visible/ Pad).

To export existing schematic to Eagle, select "File \ Export \ Eagle Schematic" from the main menu, define the filename and save it.

2.2.7.7. SPICE netlist

You can run SPICE simulation directly in DipTrace or export SPICE netlist (*.cir) for external simulation.

We can recommend freeware LT Spice software from the Linear Technologies to simulate schematics made in DipTrace.

To export SPICE netlist from DipTrace Schematic, select "File \ Export \ Spice Netlist" from the main menu.

In the pop-up dialog box specify GND net (zero signal), SPICE commands, and press OK to export the netlist.

SPICE models for all components should be defined before export.

Simulation command for LT Spice looks like this: ".TRAN 0s 10s 0.1s", where 0s – start time, 10s – end time, 0.1s – step of simulation.

However, correct start/end time and step can be changed directly in the LT Spice. Please refer to the corresponding SPICE language documentation.

2.2.7.8. Bill of Materials

To create a bill of materials for the schematic, select "File/ Export/ Bill of Materials" from the main menu. The following dialog box will pop up:

The rows of the BOM table can be grouped by components, parts, component name, name and value/ pattern. Select the appropriate option from the Group Rows by drop-down list.

Reference designators for multiple hierarchical blocks may correspond to schematic (R1, R2, etc.) or PCB (R1_1, R1_2, etc., R2_1, R2_2, etc.). Quantity is always counted by the number of physical components (by PCB). To show RefDes by opened hierarchy, check RefDes by Open Hierarchy option.

To show column headers, check Add Header item.

Check Add Row Number to add the first column with row numbers  ("1", "2", "3", etc.)

Check Add Total Quantity to add the last row with total quantity of components, parts, pins (depending on the row).

You can define the columns of the BOM table.

To add a column, select component property from the Show drop-down list, set the column width, alignment, and press Add button. Remember to add Supplier and Price columns, if you want this information to be included into the BOM table.

You can press the Suppliers and Prices button in the bottom-left corner to open Suppliers and Prices from Octopart dialog and assign suppliers or check the current prices.

To change parameters of the existing column, select it from the Columns list, and change the corresponding fields.

To insert a new column, select position in the Columns list, and press Insert button.

To delete a column, select it from the Columns list, and press Delete button.

There are four ways to create a BOM table:

1. Current Sheet. Only one table with all components. To place it, select Current Sheet from the Create On drop-down list, press Place Table, and left-click the top left corner of the table on the schematic sheet.

2. Each Sheet. Each sheet of schematic has its own bill of materials. To create BOM tables, select Each Sheet from the Create On list, press Place Table, and left-click the top-left corners of the BOM tables on every schematic sheet. The tables are created on all schematic sheets. You can move the BOM tables directly on the sheets, like regular table objects.

3. New Sheet(s). DipTrace creates a new sheet and places the BOM table there. You can select the sheet template from the template list and adjust table by sheet border width. Press Place Table, the BOM table will appear according to the sheet size and titles. If there is no space to place all components on a single sheet, the software will add more sheets automatically.

4. Export to File. The BOM files are available in 2 formats: Excel CSV and files with *.bom extension. When exporting to file, DipTrace will ask you to set a Column Divider and decide whether to use Quotation Marks for values or not. 

Please notice that you can add custom rows and columns to the BOM file in any spreadsheet editor.

2.2.8. Schematic information

With Schematic Information dialog box you can check the number of components, pins, nets, etc.

To show this dialog box, select "File/ Schematic Information" from the main menu.

2.3.1. Review

In DipTrace a typical electronic component consists of schematic symbol, PCB footprint (pattern), and possibly a 3D model. All these entities represent a single component on various design stages. The Schematic module works with schematic symbols, which represent real electronic components on the principal circuit.

Refer to the Component Editor Help and Pattern Editor Help for more details about designing components and libraries.

Place Component panel is on the left side of the screen. It has all necessary tools for placing single- and multi-part components and managing libraries and library groups in all DipTrace modules.

Libraries are organized to library groups for convenience.

There are three library groups available by default: 

1) Components (all standard libraries, user can not edit this library group); 

2) User Components (designer adds/deletes libraries to/from this group); 

3) Project Libraries (auto-generated library with all components from currently opened circuit).

Library Setup dialog box allows the user to add libraries from separate files into the DipTrace system, create new and edit existing library groups. Changes in the library structure made in the Schematic immediately affect the libraries in the PCB Layout and other software modules. Pattern library groups are not visible on the panel in the Schematic.

It is possible to search components in any library or all of them by applying search filters. Select "Objects/ Find Component" from the main menu or press button on the Place Component panel to set up and apply the filters. You can stop the filter at any moment of the search process.  

2.3.2. Library groups

Library groups are very easy means of organizing libraries. There are three default library groups: Components, User Components, and Project Libraries (auto-generated library group for storing all components of active principal circuit in the Design Cache library).

Press to change active library group or open the Library Setup dialog box to create and edit library groups and connect separate libraries from the files.

Press to change move/copy/delete component libraries between the library groups.

2.3.3. Library setup

Place Component panel allows the user to find and place components. Select the library group, then select library from the list, and select the component from the list right below to place it on the design area.

Library Setup

Go to "Library \ Library Setup" from the main menu or press  and select Library Setup from the submenu. In the pop-up dialog box the user can create library groups and add/delete libraries to/from the groups. The Library Setup panel is the same as in the PCB Layout and allows the user to edit not only the component library groups, but the pattern library groups as well.

Press Add to create new library group, type in its name into the field below, and select the group type, depending on what libraries you are going to store in the group: 

Components Only type allows for adding only component libraries (files with *.eli extension) to the group; 

Patterns Only type allows for adding only pattern libraries (files with *.lib extension); 
Components and Patterns type allows for adding both library files into current library group.

Select library group from the list, and press Add Library or Add Folder buttons to add libraries from the files to the library group.

The user can not edit the standard library groups: Components and Patterns.

2.3.4. Search filters

Search filters help to find components by various parameters. Select "Objects \ Find Component" from the main menu or press button on the Place Component panel. Select the search area (where to search for components), type in the name, and press Apply Filter. Press + or - buttons to add/delete new filters, which allow for finding components by RefDes, Value, Manufacturer, Pattern, Datasheet or Additional Fields.

Press Search at SnapEDA button to open SnapEDA dialog and look up the components based on the entered parameters in SNapEDA libraries directly from within DipTrace. 

Press New Part Request to be directed to the 24-Hour Component Design Service, where you can place an order for the required component design.  

2.3.5. Search at SnapEDA

To look for the required components in SnapEDA libraries, go to "Objects \ Search Parts at SnapEDA". In the pop-up, register or log-in, if necessary, then enter data in the Search field and press button.

Select a component from the search results, its symbol and pattern will appear in the preview field, if available.

Press Place Component button to place the pattern directly on the design area.

Save to Library button allows adding the component to the existing user library or a newly-created one.

Download 3D Model button gets active, if a 3D model is available for the selected component. Press it to download the .step file to your computer. The model will be automatically attached to the respective pattern.

Press Check Price and Availability button and choose the option that suits you best. If <Featured Supplier> is selected - you will be directed to its official website.

With Check All Suppliers option selected, you’ll be able to check prices and availability of the selected component from different suppliers listed in Octopart catalog.

Note that Digi-Key is a featured supplier by default, you can change it as well as your preferred currency by pressing the Featured Supplier and Currency button at the bottom of the Suppliers and Prices from Octopart dialog.

2.3.6. Save components as a library

DipTrace Schematic module allows the designer to save components of the current principal circuit as a new library or add them to the existing one. Select components on the design area, right-click on one of them, and choose Save To Library from the submenu.

Design Cache (auto-generated library with all components of the design) can be saved as well – select Design Cache library, press , then select Save Design Cache as Library from the submenu.

2.4.1. Toolbars

DipTrace Schematic has two toolbars, Design Manager, and Place Component panel.

To show/hide the toolbars and panels, select "View \ Toolbars" from the main menu (or use Ctrl+1 – Ctrl+4 default hotkeys). The user can increase the size of the design area by hiding unused toolbars or panels. DipTrace remembers the configuration of the toolbars.

2.4.2. Group similar parts

Multi-part components typically consist of several identical parts and a power part. DipTrace allows the designer to group similar parts of the multi-part component for convenience.

If "View \ Group Similar Parts" main menu item is checked, all similar parts are shown by a single item in the list of component parts on the Place Component panel.

The part for placement is selected from a group automatically depending on existing parts on the schematic.

If "View \ Group Similar Parts" is unchecked you can select any of similar parts manually.

Notice that this feature works only for similar parts. If some multi-part component has different parts (even if they are visually identical) Grouping Similar Parts does not work.

2.4.3. Part Markings

To define default Part Markings settings for the current project, select "View/ Part Markings" from the main menu. Mark the parameter/s you would like to be shown: RefDes, Name, Values, Manufacturer, Datasheet or any additional field of the component.

If you are dealing with a multi-part component, you can also choose to show individual parameters of the parts.

Component markings can be aligned by center, top, bottom, left, right, top-right corner of the part or automatically (i.e. the software will select the best way to position the markings).

In this dialogue, you can also change font type (Vector or TrueType). We strongly recommend using Vector font and switch to the TrueType if you need Unicode characters.

Press Font Settings button to adjust markings font size, line and text width and text color.

To move component markings, select "View/ Move Part Texts" from the main menu or press F10 hotkey (by default).

To rotate markings, press R or Space while moving them.

To see how to set up display of markings for individual components, check Component Properties section of this Help manual.

2.4.4. Pin numbers

Configure pin number display options for all schematic parts or for each component individually. Custom settings have priority over the default (common) settings.

To show/hide pin numbers for all components, select "View \ Pin Numbers" from the main menu. You can change the font type and size here too.

For individual settings select the component/s, right-click on one of them, and choose Pin Numbers. It is possible to use default settings for schematic or show/hide pin numbers for particular components.

2.4.5. Connection to Bus

When a wire is connected to the bus, the connection point is marked with the net name or net number (in the bus). The marking can be above the wires or below them.

To configure what to display and where to display it, select "View \ Connection to Bus" from the main menu.

Here you can also define the font type and the size for bus markings.

DipTrace automatically assigns the net numbers in the bus (you can rearrange them). Right-click on the wire near the bus connection, and select Number in Bus from the submenu. This item is visible only if "View \ Connection to Bus \ Net Number in Bus" main menu item is checked.

2.4.6. Net Names

Use the Net Names option under the View menu to configure a common font type and size for the names of all schematic nets.

To display a net name, right-click on a net and select Display Name.

For individual net name settings, right-click on the net name box and choose one of the following options:

Edit Text: Modify the text, line spacing, angle, and anchor point.

Type: Set the font to either Vector or TrueType.

Font: Adjust the size, line width, text width, and color.

Keep in mind that custom settings for individual nets take precedence over the common settings.

2.4.7. Power and GND

It is possible to hide Power and Ground parts and nets. Choose "View \ Hide Power and Gnd" item from the main menu.

Use Net Properties dialog box to change net settings.

2.4.8. Titles

To show/hide titles and sheet, select "View \ Display Titles" and "View \ Display Sheet" from the main menu.

Sheet size and orientation, border margins, zones, and title blocks are specified in the Sheet and Titles Setup dialog box. Select "View \ Sheet and Titles Setup" from the main menu or press button on the Standard toolbar. To create custom title blocks, press the Title Block Editor button in the Sheet and Titles Setup dialog box.

To change text, font, and alignment of title block field, move the cursor to the corresponding field, and left-click it.

To show/hide the borders of the sheet on the design area, select "View \ Display Sheet" from the main menu.

2.4.9. Scaling/Panning

There are several ways to change the scale of the design area:

1. The mouse wheel – you can decrease or increase scale in very wide limits.

2. Drop-down list on the Standard toolbar (from 25% to 800%).

3. "View \ Scale" from the main menu. It is possible to select from 25% to 800%, zoom in, zoom out or specify custom scale.

4. Plus sign (+) and minus sign (–) default hotkeys to zoom IN/OUT.

5. "Zoom window" or "Zoom Extents" tools on the Standard toolbar for mouse-defined zone zoom.

Current scale is always displayed in the drop-down list on the Standard toolbar.

Panning the design area is possible with the right mouse button (hold down and move) or by arrow keys when you create wire, shape or another object.

2.4.10. Line width

DipTrace Schematic allows the user to change basic visual parameters of the principal circuit being designed. Select "View \ Line Width" from the main menu and change node diameter (the point where two wires connect), line width (wire), buses, tables, and titles.

2.4.11. Colors

DipTrace allows the user to edit design area color template as well as all elements and print colors. Go to "View \ Colors" from the main menu.

Three color templates are available: White Background, Black Background and User Defined. White background is a default template. Black background is more eye-friendly and very popular with engineers. To select color template, use the Template drop-down list.

To define color of specific element, left-click on the corresponding color rectangle, and select a new color in the pop-up dialog box. Standard templates doesn't allow for user customizations, therefore User Defined template is activated automatically.

Select the Print Colors tab to adjust colors when printing the schematic.

Schematic module and Component Editor share same color template. This means that if you need to change colors in the Component Editor, you have to change them in the Schematic. The same rule applies to PCB Layout and Pattern Editor.

2.4.12. Graphics mode

DipTrace Schematics and PCB Layout programs work in Direct3D, OpenGL and Windows GDI modes. You can select the graphics mode from the main menu "View \ Graphics Mode".

1. Direct3D is the fastest mode for regular Windows PC without high-end OpenGL hardware. This mode depends on hardware/drivers/versions, some machines still experience problems due to outdated OS/drivers.

2. OpenGL is a bit slower than Direct3D, but less dependent on hardware/drivers. OpenGL mode is the best choice for high-end engineering stations with professional OpenGL graphic adapters.

Try which one works better for you.

3. Windows GDI is an alternate mode if both Direct3D and OpenGL modes do not work correctly with your machine. It is much slower, but less dependent on drivers/hardware/OS. This mode is enough for comfortable work on small and medium projects.

2.4.13. Units

It is possible to work with the following measurement units: millimeters, mils and inches.

To change the current units, select "View/ Units" from the main menu or use Shift + U default keyboard shortcut.

2.4.14. Precision

Precision

DipTrace allows adjusting the precision rate for project values and the grid.

Select View/ Precision… to open the following dialogue-box:

Configure the precision level by defining the number of decimal places (up to ten) for all the values used in the project by units.

You can also set the minimum grid size and grid precision for the current units. Those values are converted, when measurement units are changed.  

Please note that high precision rates are used only at designing stage. When the project is saved into a file, precision up to 0.001 mil is applied.

2.4.15. Origin

Design origin is customizable, you can change its position at any time while creating or editing the schematic.

To display the origin, select "View \ Display Origin" from the main menu or press F1 hotkey (by default).

Origin can be defined with the mouse pointer or by coordinates (incrementally from current point). To define origin with the mouse, select "View \ Define Origin \ By Mouse Pointer" from the main menu or press button on the Elements toolbar, then define a new center point on the design area with a left-click (the design origin can be aligned with key points of some objects). To change origin by coordinates, select "View \ Define Origin \ By Coordinates" from the main menu.

To return origin to default position (center of the sheet), select "View \ Define Origin \ Default Position" from the main menu.

2.4.16. Grid

The user can create and edit objects on the design area freely or by the grid. If the grid is visible and Snap to Grid option is enabled, the components align by the first pin, while wires, buses, ports and shapes align by their key points.

To show/hide the grid, select "View \ Grid" from the main menu or press F11 default hotkey.

Select "View \ Snap to Grid" from the main menu, or press Alt+F11 hotkey (by default) to activate/deactivate snap to grid, when the grid is on.

If Snap to Grid option is disabled, the objects of the schematic are no longer snapped to the grid, but you can leave the grid visible.

When Snap to Grid option is disabled for the entire project, you can choose to snap to grid individual elements of your schematic (symbol, shape, text, image, etc.) by selecting Snap to Grid item from the right-click submenu of those elements, when the grid is on.

To open the grid size submenu, select "View \ Grid Size" from the main menu. Here you can select the grid size from the list or specify a custom size.

You can select it from the drop-down list on the Standard toolbar or with Ctrl + Plus sign (+), Ctrl + Minus sign (-) hotkeys.

Select "View \ Customize Grid" from the main menu to change the list of available grid steps.

2.5.1.1. Review

Regular component in DipTrace includes one or several schematic symbols (parts) and attached pattern (possibly with a 3D model). Schematic symbol consists of pins, shapes and text (marking) elements.

Change pin type and other pin properties in the Pin Properties dialog box. To start/finish inversion in the pin name use the Tilde Sign (~) hotkey.

In the Schematic it is possible to place component parts from the Place Component panel or from the Place Component dialog box.

For multi-part components, you can select part or a group of similar parts. Assign RefDes, Value, Name, Part, Manufacturer, Datasheet or Additional fields as part markings of the component on the design area. When component is on the design area, the user can move, rotate, flip, replace, update or change current schematic sheet for the component, etc.

2.5.1.2. Multi-part components

DipTrace allows the designer to create and use multi-part components in the program. Components of this kind have special reference designators consisting of component RefDes and part RefDes after the point (for example parts of "D1" component are marked "D1.1", "D1.2", etc). Certain parameters of multi-part components can be changed directly in the Component Properties dialog box in the DipTrace Schematic, for example, RefDes and the name of exact part.

When multi-part component is selected in the component list on the Place Component panel, press All Parts button, and select current part which you want to place.

The number of parts is displayed in the upper-right corner of the symbol's preview. It is also possible to select part in the Place Component dialog box.

Multi-part component may include similar or different parts. If "View \ Group Similar Parts" item is checked, similar parts are shown by a single item in the parts list and current part for placement is selected automatically.

Notice that Group Similar Parts works only for similar parts, not for multi-part components with different parts (even if they are visually identical).

The parts of a multi-part component are generally interchangeable. In DipTrace you can easily substitute one with the other - right-click on a part, select Swap Parts and choose the part for which you want to substitute the selected one.  This option works with both types of identical parts of a multi-part component. 

2.5.1.3. Net port

Net Ports are components that do not have attached patterns. These components exist only as a means of connecting pins without wires and do not have physical packages. You can create new net ports in the Component Editor or find them in the standard DipTrace libraries, select Net Ports library from the Components library group. This library hosts all the most popular net ports (incl. GND, PWR).

Place two or more net ports with the same name on one or several schematic sheets and connect wires to their pins to create a single net connected with net ports.

Notice that nets connected to the net ports are not automatically renamed to match the name of the net port.

You can use net ports with several pins to connect several wires at a time. Wires connected to the corresponding pins of connected net ports will be connected automatically. If pin numbers are different, the wires will not connect.

Reconnecting is possible simply by changing the net port name (right-click on the net port and select the first item from the submenu). However, we do not recommend renaming pins. Net ports can be used in hierarchical schematics (DipTrace will create global nets automatically).

A wire can show the direction of the signal for convenience. Right-click on a wire, and select Direction Arrows from the submenu, then select either Forward or Backward.

To remove the arrow, right-click on the wire, and select Direction Arrows from the submenu, then select None.

2.5.1.4. Place component

Place components directly from the Place Component panel or with Place Component dialog box. Select "Objects \ Place Component" from the main menu or press button on the Objects toolbar.

Select library group in the drop-down list, select library, and select component. Press Place button. Use Filter ON/OFF button to adjust filters or turn them ON/OFF. Press Library Setup to edit library groups, press Display Pattern to preview component pattern.

Press Price and Availability button to consult price and availability of the selected component from a featured supplier or all the suppliers from Octopart catalog.

Use R or Space bar to rotate component before placement. You can drag and drop the component to change its location; guidelines will appear while moving it to help you align it with other components.

2.5.1.5. Attached pattern

DipTrace allows the user to change attached pattern and pin numbers for existing component/s or attach new pattern/s directly in the Schematic.

To change attached pattern, right-click on the component, and select Attached Pattern from the submenu or press Attached Pattern button in the Component Properties dialog box.

Select component from the list on the left side, then choose the library group from the Pattern Libraries drop-down list, select library, and select appropriate pattern from the list below (you can apply filters to find the pattern). Assign Pin to Pad connections in the corresponding table or visually in the component and pattern previews. Note that pads with the same numbers are automatically connected to one net. Use @ sign after the identical pad numbers to avoid errors.

You can also create connections between pads manually: left-click on a pad and then click on another one, with which you want to create a connection - a menu will pop up; confirm or cancel pad connection by selecting the respective option.

Press Apply to Other Components to apply selected pattern to similar components with the same name regardless of the pattern, or to components with the same pattern regardless of their name.

Designer can Undo to the previous pattern.

The Side drop-down list is good for SMD patterns with pads on both sides of the board (for example, EDGE connectors).

If it is a multi-part component, each part can be selected separately in order to define pin numbers, use the Part drop-down list under the schematic symbol preview field.

Attach Pattern dialog box is the same as in the Component Editor, but instead of all components of active library you see all components of current schematic.

2.5.1.6. SPICE Model

To define/change SPICE settings of a component, right-click it and select SPICE Model from the submenu. The following dialog box will pop up:

All the parts of the current schematic are displayed on the left. Left-click to select the required component from the list or use the search field to find it.

Pin-to-signal connections can be established using the table in the central part of the dialog box. The list of available signals with comments is located right below.

The dialog allows selecting the model type, defining parameters, model and signals for the components. Resistor, Capacitor, Inductor, Sources, Mutual Inductance and Transmission Line types do not require models and you can define their parameters manually. SubSkt type is often used to define logics, chips, etc., however, it can be used for almost any purpose.

Notice that models can be loaded from external ASCII files (usually available at manufacturers' websites or other locations on the Internet), just select the Model tab and press Load.

A SPICE model can also be loaded from the existing DipTrace library (press Get SPICE Model from Library button and select the respective Library group, Library and Component).

Once defined, component SPICE settings can be applied to Similar parts of the Component or All Similar Parts of the Schematic - press Apply to Other Parts button and select the required option.

Template line shows how the component will be displayed in the Spice netlist. Notice that you can scroll it to the right if necessary, because templates may be quite long.

If you are not familiar with SPICE language, we recommend using SPICE Language Documentation available on the Internet to discover more details.

After defining SPICE models for the schematic components you can run a built-in NGSPICE Simulator.

2.5.1.7. Properties

Right-click on a component, and select Properties from the submenu to open the Component Properties dialog box.

Here you can adjust component position by setting X and Y coordinates.

Component can be updated from the selected library. Press button to browse for the required library file. Press Update Component button to apply changes.

A typical component has the following parameters: RefDes, Value, Name, Manufacturer, Datasheet, Additional fields, Part RefDes and Part Name (for multi-part components). RefDes is a unique component identifier.

Press Configure Additional Fields button to add more descriptive fields.

New fields can be added to the Current Component, Selected Components, Similar Name Components, components with Similar Set of Fields or All Components.

Enable Parts checkbox allows the designer to change internal RefDes and name of each part of multi-part component.

In the Markings Tab of the Component Properties dialog, you can choose to show/hide certain marking/-s (RefDes, Value, Name, etc.) or apply Common (default) settings to a given component. If you are dealing with a multi-part component, you can also select whether to show/hide or apply common settings to the markings of individual parts.

To define marking alignment settings, select the necessary option from the drop-down in Align column. The markings can be adjusted by the top, bottom, left, right, the center or corner of the component. You can also apply Common or Auto settings. In the first case, the software will use default parameters set for the entire project (View/ Part Markings). If Auto mode is selected, DipTrace will automatically select the best location for the markings.   There is one more Aligning option - Position. Use it for precise Markings placement. Once selected, an active line appears in Position column. Press button to select the location of Markings anchor point, set its coordinates and rotation angle.

To change shift and spacing for the component text markings, select "View/ Move Part Texts" from the main menu or press F10 hotkey (by default). To rotate component markings while moving, press R or Space hotkeys.

2.5.1.8. Signal delay

Bond wires inside electronic component's package connect pads to the die. These wires introduce a signal delay, which should be accounted for in high-speed designs. Manufacturers report this in-device pad signal delay in picosecond time or as a length in the datasheets. 

Pad signal delay value is considered for phase and length tuning and is added to the total length of the tracks when on the circuit board. We recommend setting up signal delays when designing a component in the DipTrace Component Editor, but you can also set it directly on the schematic (delay value is valid only for this schematic and PCB, this change does not affect the component in the library).

To set pad signal delay in the Schematic, right-click on the component and select Pad Signal Delay from the submenu or right-click on the pin and select Signal Delay.

Select pad from the list (if not selected already), and enter a signal delay in mils right below. Press OK to apply changes. 

You can also assign pad signal delays directly in the PCB Layout and Component Editor (recommended).

2.5.1.9. RefDes renumbering

Reference designators can be renumbered from the top-left to the bottom-right corner of the schematic sheet by rows or columns for convenience of exploring the schematic. Select "Tools \ RefDes Renumbering" from the main menu or right-click on any component, and select RefDes Renumbering from the submenu:

Renumbering can be applied to all reference designators of schematic or only to current RefDes (option is available only if you called RefDes Renumbering dialog box from the component submenu). Component position in the renumbering array can be determined by its top-left corner or by its origin.

Page Step value means page start increment index in the RefDes naming procedure (i.e. if the Page Step is 100, reference designators on the second page will be R101, R102, IC101, etc.).

Renumbering is possible by rows and by columns:

2.5.1.10. Pin properties

DipTrace Schematic allows the designer to change pin properties. Right-click on the pin, and select Pin Properties from the submenu. The following dialog box will appear:

Here you can change the graphical pin type, electric type for ERC verification, pin name, and pin number. Pin number is usually a pad number of related pattern.

There are 15 types of pins:

Press Font of Name button to adjust pin name font size, line and text width.

To start/finish inversion in the pin name use the Tilde Sign (~).

Properties and font of pin names can be applied to: single pin, selected parts and to all parts of current schematic.

2.5.1.11. Assign Supplier

In DipTrace you can consult prices and availability of the components used in your design in Octopart’s supplier database. The best supplier can be assigned to each component. This information can subsequently be included into the bill of materials.

To select suppliers, go to Tools/ Assign Suppliers. The following dialog will pop-up:

To assign a supplier to a component:

1. Select a component in the Layout Components section on the left. Using the drop-down menu you can filter the list to display Assigned, Not Assigned or All Components.

2. Review the component specifications in the central part of the dialog and select the appropriate one. To filter the search results by Manufacturer or Package, use the respective drop-downs on the right. You can Search Octopart Database directly from DipTrace to look for specific parts or to narrow down the suggested options.

3.Consult prices and availability of the selected component from different suppliers. Note that Digi-Key is the featured supplier by default, meaning that it’s automatically selected as the provider. You can easily re-assign the supplier for a certain part by pressing the Select button. To change your preferred supplier and currency, press the Featured Supplier and Currency button.

When done, press the Assign to Component button and proceed with the next component.

2.5.2.1. Review

Nets in DipTrace Schematic consist of wires connecting component pins, buses, and ports for nets and buses. Net connections can be visual and logic (by name, without wires, with net ports). See Connecting for more information. All wire-to-bus connections are marked with net name or net number in the bus.

There are two modes of creating wires: automatic and manual (use M hotkey to switch between the modes while drawing the wire). Automatic mode draws the wire from the start point to the end point automatically, DipTrace avoids overlaying parts or wire segments with parts and wires of the same orientation if there is enough free space on the sheet. Manual mode allows the user to place wire segments step-by-step, use S or Space hotkeys to switch between the segments.

Nets can be renamed, wires can be hidden or moved to another sheet, net color can be changed, etc.

2.5.2.2. Net classes

Net classes organize nets and allow the user to automatically apply predefined parameters to newly created nets. To add/edit net classes or move nets from one net class to another, select "Objects \ Net Classes" from the main menu. The following dialog box will appear:

The user can add/delete net classes and edit their properties. Enter the name of the net class, select type (normal or differential pair) and enter values to set up the trace width, clearance, differential pair length and phase tolerances (if it is differential pair net class). These settings will be transferred to the PCB Layout, where more routing parameters will be available for customization.

DipTrace does not allow for nets outside any net class, hence all nets are automatically assigned to Default net class. The user can edit this class, but can not delete it.

Only blank net classes (no nets belong to the net class) can be deleted. Net should be moved to another net class before deleting. To move nets between the classes, use lists on the right side of the dialog box and Up and Down buttons.

Net classes can be loaded from the PCB Layout, select "Objects \ Load Classes" from the main menu and select the layout file to extract the net classes or use the Back Annotate feature ("File \ Back Annotate" from the main menu).

2.5.2.3. Placing wires

There are several ways to create wires in the Schematic:

1. Default (Visual). Place wire with the mouse in the default mode (or in the Place Wire mode), left-click on the start point of the future wire (pin or wire segment), and then left-click on the end point (pin, wire segment or bus).

The software draws wires and creates corners automatically – the wire never overlays any components or wire segments with the same orientation (depends on the free space on the sheet). Press M hotkey to place wire segments step-by-step and create corners manually (use S or Space hotkeys to switch between 0>90 and 90>0 segments, U hotkey removes the last placed segment).

Right-click, and select Enter from the submenu to finish/cancel wire placement, or use Enter or Esc hotkeys.

2. From the submenu. Right-click on the pin, and select Add to Net from the submenu, choose net in the drop-down list, and press OK. It is possible to connect pins to existing nets without wires, check Connect without Wire box in the Add to Net dialog box.

3. Connection Manager. To create wires with the Connection Manager, select "Objects \ Connection Manager" from the main menu or right-click on any net, and choose Connection Manager. It is possible to edit net list by adding/deleting pins to/from existing nets and to add new nets to the schematic.

See connecting for more details about using buses, net ports and connection without wires.

2.5.2.4. Editing wires

The user can move wires orthogonally. To enable wire editing mode, select "Objects \ Circuit \ Edit Mode" from the main menu or press button on the Objects toolbar. This mode is activated automatically, when you try to drag existing wire segment with the mouse.

To add nodes to the wire segment, right-click it, and select Add Node from the submenu.

To change net for the wire connected to the bus, right-click on the wire, select Bus Connection from the submenu, and select a new net from the pop-up dialog box. To create a new net, enter its name in the Bus Connection dialog box, and press OK.

To delete wire segment, right-click it, and select Delete Line or Delete Wire from the submenu. The first option deletes a single straight line, the second – all segments of the wire between two connection points. Net structure can be changed.

The user can move a wire or entire net to another schematic sheet (if it is multi-sheet schematic). Select Change sheet from the right-click submenu.

Notice that you can not move wire to another sheet if it is connected to non-moving objects (components etc.). Therefore, if you want to move some wire to another sheet, select it together with connected components and move altogether to another sheet.

2.5.2.5. Connecting wires

DipTrace Schematic allows the user to connect pins with wires, net ports, buses and bus connectors, as well as connecting pins without wires.

1. Bus and Bus Connectors. To connect pins or wires with a bus, you should place a bus first, then connect wires or pins to the bus. The bus is a good choice when you need to connect many points in different parts of the schematic (in this case one bus replaces tens or even hundreds of wires with a single thick blue line). See Bus Review topic. Use bus connectors to connect buses on different schematic sheets (pages).

2. Connection without wire. To connect pin to any net without wire, right-click on the pin, select Add To Net from the submenu (item is visible if at least one net exists on the schematic), then select net from the drop-down list, and check Connect without Wires checkbox. Press OK. Please see the picture below: U2: Pin 4 (inverted MCLR) is connected without a wire.

3. Connect Nets by Name. To connect wires (nets) by name, right-click on any wire, and select the first item with the net name from the submenu. Now type in the name of existing net, which you want to connect with this wire, and press OK. The program may warn you that such net already exists and whether you want to connect wires by name (the warning message pops up only if Connect Nets By Name checkbox is unchecked for one or both nets).

Nets connected by name does not have any special marks, but when hovering over the wire with the mouse, you see two visually unconnected wires highlighted.

If you check Connect Related Wires Only checkbox in the Net Properties or Rename Net dialog box, DipTrace will connect only the wires which are visually connected. Therefore, you can easily move groups of wires between the nets by simply renaming them without deleting existing nets, which are logically connected with the wires being renamed. Two connected wires can not belong to different nets.

Notice that only global nets allow for connecting pins on different hierarchical levels.

4. Net Ports. Place two or more net ports with the same name on one or several schematic sheets and connect wires to their pins. Please see the picture below: U2: Pin 5 VSS is connected to the GND net with the net port.

Notice that nets connected to the net ports are not automatically renamed to match the name of the net port.

You can use net ports with several pins to connect several wires at a time. Wires connected to the corresponding pins of connected net ports will be connected automatically. If pin numbers are different, the wires will not connect.

Reconnecting is possible simply by changing the net port name (right-click on the net port and select the first item from the submenu). However, we do not recommend renaming pins. Net ports can be used in hierarchical schematics (DipTrace will create global nets automatically).

The picture below shows all aforementioned ways of connection:

Here you can see "Net 59 – Net 7" connected to the bus, U2:VSS and C13:1 connected together via the GND net ports, U2:MCLR(inv.) and U2:RA4 connected to RESET and P8 nets without wires.

2.5.2.6. Properties

Right-click on the net, and select Properties from the submenu. The following dialog pops up:

The Name section allows the user to rename entire net or rename only related wires (Rename Related Wires Only checkbox). If renaming only related  wires, a group of visually connected wires will be disconnected from existing net and logically connected to a new net (by name). If you would like to connect wires by renaming them, enable Connect Nets by Name checkbox.

Connect Net to Pins by Name – connect all component pins with a net, if they have similar names.

Global Net for Hierarchy checkbox allows the designer to use a single net on different hierarchical sheets (different hierarchical levels). The net will not be separated by the blocks, i.e. all pins connected to the global net in hierarchy will be connected together in the layout, even if they are located in different hierarchy blocks. Global net is created automatically if some wire is connected to net port inside the hierarchical sheet.

Net Class – here you can change the net class of the net and preview its properties (type, trace width, clearance, etc.).

If Hide Power or Ground main menu item is enabled, the wire(s) will become hidden when you hide power objects.

2.5.2.7. Connection Manager

Connection Manager is another tool to work with net structure. It is very convenient, especially for complex schematics. Select "Objects/ Connection Manager" from the main menu or right-click on any net, and select Connection Manager from the submenu.

Here you can select net from the drop-down list. All pins of the net appear in the Net Pins table.

You can rename the net with the button or delete it with the button. Press to add new net.

To delete pin from the net, select it in the table, and press Delete button.

To add new pin to the net, select component/part and a pin of this part, then press Add button.

2.5.3.1. Review

Differential pair signaling is a method of transmitting high-frequency low-voltage signals using two tightly coupled conductors (tracks on the circuit board). One track carries a signal and the other one carries an equal, but opposite image of the signal. Differential pairs are EMI immune, they generate less noise than single-track connections and, basically, are the only acceptable way to transmit high-frequency pulses on a circuit board.

DipTrace provides tools to create and edit differential pairs on the schematic and directly in the PCB Layout. Differential pair declaration can be put on the nets that already exist on the design area. Create a special type Differential Pair net class prior to defining a differential pair. Net classes manage all differential pair properties and routing constraints. Differential pairs are not allowed to have parameters outside a differential pair net class. DipTrace does not impose any restrictions on how many classes can be created.

The software controls various aspects of differential pair routing in the net class parameters (also available in the Schematic): trace width, gap, clearance to other objects, maximum total uncoupled length for two tracks of the pair, tolerance for length difference, dynamic phase tolerance, and phase error length for a differential pair net class.

Diff pair parameters are verified as DRC constraints in the PCB Layout.

2.5.3.2. Create differential pair

In order to create a differential pair in DipTrace, proceed to the Net Classes dialog box ("Objects \ Net Classes" from the main menu) and create a new net class. Press Add button, and select Differential Pair Type.

Class properties allow the user to change trace width, primary gap between the traces, clearances to other objects, differential pair length and dynamic phase settings. These parameters will be automatically transferred to the PCB Layout. Press OK to close the Net Classes dialog.

Now go to "Objects \ High Speed \ Define Differential Pair" from the main menu. In the pop-up dialog change pair name, color, and define positive and negative nets of the pair with the corresponding drop-downs or by pin pointing nets directly on the design area (just press or buttons and click on the pad of the net to put a differential pair declaration).

Notice that the previous net name will be disregarded in favor of the new one, typically it consists of a diff pair name + positive or negative net index.

Press Edit Net Classes button to open the Net Classes dialog box if you need to.

Select differential pair net class from the drop-down list, and apply changes by pressing OK button. Differential pair nets are marked with a special symbol directly on the design area. Custom diff pair color also applies.

Notice that differential pair can not exist outside differential pair net class.

2.5.3.3. Edit differential pair

Editing differential pair wires does not differ from editing any regular nets and wires. However, with some special features available in the right-click submenu. If you are new to the software, please review Editing Regular Wires topic first.

When you hover over one of the differential pair nets with the mouse cursor, current wire and a differential pair symbol of the other wire are highlighted.

2.5.3.4. Diff pair properties

Right-click on any wire that belongs to a differential pair, and select Properties from the submenu.

This dialog box allows the designer to change differential pair name, wire color, define other nets to the differential pair, change current net class, and review differential pair routing parameters. Net class defines all differential pair routing parameters. If you need to change them, you need to change current net class. Press Edit Net Classes to manage and edit Net Classes.

Notice that differential pair can not exist outside differential pair net class.

2.5.3.5. Differential Pair Manager

Differential Pair Manager is the most convenient way to create/edit/delete differential pairs in complex projects. Go to "Objects \ High Speed \ Differential Pair Manager" from the main menu. The following dialog box will pop up:

Sort differential pairs by net classes with the Net Class drop-down list.

Select differential pair from the list and review or change all differential pair parameters. Press Edit Net Classes to open the Net Classes dialog box for adding/deleting/editing net classes. In order to add or delete differential pair use Add or Delete buttons. Press OK to apply changes.

2.5.4.1. Review

Bus allows for visually grouping and compacting various nets (replacing tens or hundreds of wires with a single thick blue line). Buses also allow the designer to visually connect nets on different schematic sheets/pages. All wire-to-bus connections are marked with the net name or net number in the bus.

Each bus has its own list of bus nets. While connecting wire to the bus, you can connect it to the net which is already inside the bus or add new net. If you need to change nets in the bus, right-click on the wire segment connected to bus, and select Bus Connection from the submenu.

Bus connectors allows the designer to connect buses on the same or different schematic sheets. If two or more bus connectors have the same name, all  buses connected to them will automatically merge into a single bus.

2.5.4.2. Placing a bus

To create a bus, select "Objects \ Circuit \ Place Bus" from the main menu or press button on the Objects toolbar and draw the bus line segment-by-segment. You can terminate bus on the other bus line, bus connector or on empty spot. To terminate or cancel bus placement, right-click while drawing the bus, and select corresponding item from the submenu, or use Enter and Esc hotkeys respectively.

S or Space hotkeys allow the user to switch between 0>90 and 90>0 segments. U hotkey undoes the last segment.

Bus lines connected to bus connectors with the same name are united automatically. Schematic bus structure can be changed by changing the names of bus connectors. Be careful while renaming bus connectors if their buses already have connected nets.

2.5.4.3. Editing a bus

You can move bus segments in the edit mode or default mode (in this case the edit mode is activated automatically). To activate the edit mode manually (for example, if you want to edit the bus, which lies under some component), select "Objects \ Circuit \ Edit Mode" from the main menu or press button on the Objects toolbar. Now left-click on the bus segment and drag it:

To add node to the bus segment, right-click it, and select Add Node from the submenu.

Single bus can be located on different schematic sheets (not hierarchy blocks).

To connect bus lines on different schematic sheets:

– Place bus connectors on both sheets,

– Define the same names to the bus connectors,

– Connect bus lines to the connectors.

You can move bus to another schematic sheet. In this case, the bus will disappear from the current sheet, but all wires will be still connected to this bus. Bus connectors and connected bus should be moved together, just like a regular net.  

To delete bus segment, right-click it, and select Delete Line from the submenu. Select Delete Wire from the right-click submenu to delete the wire. Select Delete from the right-click submenu to delete entire bus.

2.5.4.4. Bus nets

To open the list of bus nets, right-click on the bus, and select Bus Nets from the submenu. The following dialog box will appear:

Here you can choose a bus and delete nets. After deleting, the structure may be changed, so please be careful.

2.5.5.1. Review

Shapes allow the designer to make any custom drawings directly on the schematic sheet.

The following shape types are available: Line, Arc, Rectangle, Filled Rectangle, Obround, Filled Obround, Polyline, Polygon, Text, and Picture.

2.5.5.2. Create

To place a shape, press button on the Objects toolbar and select the corresponding shape, or go to "Objects \ Place Shape" from the main menu. Then draw a shape on the design area.

To place a Line, press button on the Objects Toolbar. Left-click to anchor the starting point and the end point. When drawing the line, it’s dimensions will be displayed by DipTrace.

To place an Arc, press button on the Objects Toolbar. There are three modes for Arc placement in DipTrace. Left-click to anchor the starting point, then right-click to select placement mode:

Choose Clockwise or Counter-Clockwise from the right-click submenu to define the concavity direction of the curve.  

Select Cancel from the right-click submenu to cancel the arc placement.

When drawing an arc, it’s key parameters (radius, deg.) will be displayed by DipTrace.  

To place a Rectangle/ Filled Rectangle, press or button respectively on the Objects Toolbar. Left-click to anchor the starting point, draw the shape and left-click in the end point. When drawing the shape, it’s dimensions will be displayed by DipTrace.  

To place a Obround/ Filled Obround shape, press or button respectively on the Objects Toolbar. Left-click to anchor the starting point, draw the shape and left-click in the end point. When drawing the shape, it’s dimensions will be displayed by DipTrace.

To place a Polyline/ Polygon, press or button respectively on the Objects Toolbar. Left-click to anchor the starting point, draw the shape, left-click to anchor points, right-click in the end point and select Enter form the submenu. When drawing the shape, it’s dimensions will be displayed by DipTrace.

To define shape color and line width before placement, select "Objects \ Drawing Properties" from the main menu. However, it is possible to change these properties for objects already on the design area via Properties submenu.

2.5.5.3. Edit

To change shape size, select a shape, and drag its key points with the left mouse button.

Right-click on the shape object and move it to another sheet, if necessary (Change Sheet item).

For precise shape editing, use the Shape Properties dialog box.

2.5.5.4.1. Line

Right-click on a line, and select Properties from the submenu to open Shape Properties dialog box:

You can use pre-defined line width (Objects/ Drawing Properties/ Line Width) or set a new value for the given shape.

To change shape color, click on the colored rectangle and select a new one.

Start and End Points can be adjusted by changing  X and Y coordinates or by using button to set them by Mouse Pointer.

Finally, you can edit Line Dimensions, just type-in new values for Horizontal (dX) and Vertical (dY)  tangent.

2.5.5.4.2. Arc

Right-click on an Arc, and select Properties from the submenu to open Shape Properties dialog box:

You can use pre-defined line width (Objects/ Drawing Properties/ Line Width) or set a new value for the given shape.

To change shape color, click on the colored rectangle and select a new one.

Select an Arc Edit mode: Center+Start/End Angle+Radius or Start/ End Point+Radius or angle. Type-in all the required values. Note that points can be defined by X and Y coordinates or set by Mouse Pointer upon pressing .

Finally, you can change arc Radius and Angle.

2.5.5.4.3. Rectangle/ Filled Rectangle

Right-click on a Rectangle/ Filled Rectangle, and select Properties from the submenu to open Shape Properties dialog box:

You can use pre-defined line width (Objects/ Drawing Properties/ Line Width) or set a new value for the Rectangle.

To change shape color, click on the colored rectangle and select a new one.

Next, you can change the position of an anchor point and type-in its coordinates for precise shape positioning.

Finally, you can edit shape dimensions.

2.5.5.4.4. Obround/ Filled Obround

Right-click on an Obround/ Filled Obround shape, and select Properties from the submenu to open Shape Properties dialog box:

You can use pre-defined line width (Objects/ Drawing Properties/ Line Width) or set a new value for the Obround shape.

To change shape color, click on the colored rectangle and select a new one.

Next, you can change the position of an anchor point and type-in its coordinates for precise shape positioning.

Finally, you can edit shape dimensions.

2.5.5.4.5. Polyline/ Polygon

Right-click on a Polyline/ Polygon shape, and select Properties from the submenu to open Shape Properties dialog box:

You can use pre-defined line width (Objects/ Drawing Properties/ Line Width) or set a new value for the Polyline shape.

To change shape color, click on the colored rectangle and select a new one.

Next, you can change the position of an anchor point and type-in its coordinates.

Finally, you can edit shape dimensions by clicking on Polyline Points/ Polygon Points button.

2.5.6.1. Create

A multiline text can be placed in DipTrace. Go to Objects/ Place Text or press button on Objects toolbar.

Left-click on the design area and type the text.

Use Enter key to move to the next line.

Right-click on a free spot of the design area to return to default mode. You can drag and drop the text to change its location; guidelines will appear while moving the text to help you align it with other text objects.

To define text font type and size, width and color before placement, select Objects/ Drawing Properties from the main menu. However, it is possible to change these properties for objects already placed on the design area.

Note that tilde (~) before and after text is reserved by the software for placing a line over the pin name, which implies inversion; if you want a tilde symbol to appear as it is, you should place it twice:

~text~/~~text

2.5.6.2. Edit

To edit, double click on the text object or right-click on it and select Edit Text. The following dialog will appear:

Here you can change the text, line spacing and alignment. Press Show All Text Properties button to access Text Properties dialog that allows for adjusting more text object parameters.

Right-click on a text object and select Font Type from the submenu. Vector and TrueType fonts are available. Vector font is recommended, if you use Latin characters. Unicode characters are supported only by the TrueType fonts.

To change text object size, select it and drag its key points with the left mouse button, the font size will change automatically.

Select Rotate from the text right-click submenu to rotate it at 90-degree step counter-clockwise. You can use R or Space hotkeys for the same purpose.

Right-click on the text object and move it to another sheet, if necessary (Change Sheet item).

2.5.6.3. Properties

To open Text Properties dialog, right-click on the text object and select Properties from the submenu.

In the pop-up dialogue you can set line spacing and text alignment.

Choose an angle from the Text Angle drop-down or just type-in the required value to rotate the text.

The location of the Anchor Point of the text box is set by ticking the respective circle. Anchor Point is displayed as a cross. You can also set the coordinates of the Anchor point for precise text positioning.

Select Font Type: Vector font is recommended, if you use Latin characters; unicode characters are supported only by the TrueType fonts.

Press Font Settings button to open Font dialog (it can also be accessed by selecting Font in the text right-click submenu):

Here you can set the font size, select the Line Width from Thin, Normal, Bold or Customize it, and also define the Text Width and color.

Mark Monospaced Font to distribute character spacing evenly across the text, applicable to vector font only.

2.5.7.1. Review

Table has a certain number of columns and rows.

Table field can contain any text aligned by left, center or right (Vector or TrueType fonts for Unicode characters).

To change column width or row height, use the Table Properties dialog box or select the corresponding item from the table submenu.

To change text and cell alignment, left-click on the table cell, and specify new text and alignment.

2.5.7.2. Create

To place a table, select "Objects \ Place Table" from the main menu or press button on the Objects toolbar. Then left-click on the design area, where the table should be created and you will see this dialog box:

Specify a table name, number of columns and rows, column width and row height, alignment, line spacing and font type.

To define other parameters of the text placed in the table fields, press Font button.  Click the Place button to create the table.

All table properties can be changed in the Table Properties dialog box.

2.5.7.3. Edit

To define text and alignment of the table field, left-click on the field and make all changes in the pop-up dialog box.

To change column width or row height, hover over the cell which belongs to the column or the row of the table, right-click to open the submenu, then select Column Width or Row Height, enter new values, and press OK. To change size of all columns and rows of the table, use the Table Properties dialog box.

To add columns and rows to the table, move the mouse cursor to the table border, right-click it and select the corresponding item from the submenu.

To insert columns or rows to the table, move the mouse cursor to the table field, right-click it and select the corresponding item from the submenu. Empty columns or rows will be inserted before selected cell.

To delete columns or rows from the table, move the mouse cursor to the cell, which belongs to the column or row, right-click it, and select Delete Column or Delete Row from the submenu.

To move table to another sheet, right-click it or right-click on any table field, and select Change Sheet from the submenu.

2.5.7.4. Properties

To change table properties, right-click on a table, and select Properties from the submenu. The following dialog box pops up:

Here you can change the table name, column width, row height, alignment, and font by default.

Changes can be applied to:

– all table cells;

– cells with default settings;

– as default settings for new cells (not for existing cells).

2.5.7.5. Saving to file

Schematic table can be saved into Excel CSV file or into formatted text files.

To save table to a file, right-click on a table, and select Save to File from the submenu and decide on the file format (Excel CSV or Text File). CSV file is perfectly supported by popular spreadsheet programs (MS Excel, OpenOffice, etc.). When exporting to CSV file, DipTrace will ask you to set a Column Divider and decide whether to use Quotation Marks for values or not. 

2.5.8. Bus connector

Bus Connectors allows the designer to connect buses on different parts of the schematic (including different schematic sheets).

All buses connected to the bus connectors which have the same name, are united into a single bus automatically.

Correctly connected bus connector has a green connection point. Blue connection point means that the bus line and the bus connector are not connected, even if visually everything is OK.

Notice that boxes around the names of the bus ports show that these bus ports are connected. Underlined means unconnected.

To connect bus lines on different schematic sheets:

– Place bus connectors on both sheets,

– Define the same names to the bus connectors,

– Connect bus lines to the connectors.

Net ports basically serve the same purpose as bus connectors, but net ports only connect one or several nets. See Connecting for details. User can easily change current sheet for selected bus connector, like for any other object. If bus connector is connected to a bus, select both and move them to another sheet.

2.5.9. Hierarchy

DipTrace supports hierarchical schematics based on the multi-sheet structure. This structure allows for vast block routing capabilities. There are two basic objects that are used in the hierarchy: hierarchy connectors and hierarchy blocks.

To create a hierarchical schematic, you should add new sheet to the schematic ("Edit \ Add Sheet" from the main menu), then go to "Edit \ Sheet Type \ Hierarchy Block" from the main menu to change sheet type. You can change sheet type for the second and all further sheets. The first sheet is always on top level of hierarchy, it is a main circuit, you can not delete it.

The next step is adding hierarchical connectors to the sheet. They are associated with block pins (IN/OUT). Select "Objects \ Hierarchy \ Place Connector" from the main menu or press button on the Objects toolbar, then place connectors on the design area. The location of hierarchy connectors defines the location of the block pins on the main sheet.

Now design the subcircuit and connect its inputs and outputs to hierarchical connectors inside the block. You can use global nets to connect pins on different hierarchy levels. Net is always global if it is connected to net ports inside a hierarchical block (Net 15, connected to the GND pin on the picture below).

To place hierarchical block into the upper-level hierarchical block or to the main sheet, select "Objects \ Hierarchy \ Place Block" from the main menu or press on the Objects toolbar. Select hierarchical sheet from the list and place it on the design area. You can place unlimited number of blocks. If there are several hierarchy blocks with the same content – the software will assign special indexes to reference designators and net names: <RefDes>_<Block Number> or <Net Name>_<Block Number>.

Notice that DipTrace supports multi-level hierarchy, but you should be very careful while designing schematic with hierarchy, because probability of making an error sufficiently increases.

2.5.10. Search objects

To find component or net on the schematic, select "Edit \ Find in Schematic" from the main menu or press Ctrl+F hotkeys (by default).

In the pop-up dialog box, select the object type (Component or Net) and the search criterion (All, RefDes, Value or Name). Then enter the full or partial search term and press Enter or click Search.

In the Results list, double-click an object or click Locate to highlight and center it in the design area.

To select objects, choose one or more entries in the Result list and click Select.

For direct editing, click Properties to open the object’s Properties dialog.

The Search dialog does not need to be closed while working with the schematic. It can be minimized by clicking the arrow in the upper-left corner.

2.6.1. Select objects

DipTrace has several ways to select objects or edit existing selection:

1. The mouse. Click on the object with a mouse button. Use left mouse button to select an object, and right mouse button – to open object's submenu. Notice that you can select overlaying objects by clicking the same button again and again, depending on the number of overlaying objects.

2. Default mode. In the Default mode hold down the left mouse button on empty area, and move the mouse pointer to draw the selection box. All objects surrounded by this box will be selected when you release the mouse button.

Use Ctrl or Shift hotkeys to add objects to the selection.

If you try to select one object from a group, the entire group will be selected.

To select all objects of the design, go to "Edit \ Select All" from the main menu or press Ctrl+A hotkeys.

3. Edit Selection. Go to "Edit \ Edit Selection" from the main menu. Edit Selection dialog box allows the user to select objects by type.

In the pop-up dialog box select the objects and one of the selection modes:

1. New Selection – deselect all previously selected objects and create a new selection based on your choice;

2. Add to Selection – add specified objects to existing selection;

3. Remove from Selection – remove specified objects from existing selection;

4. Keep Selected – deselect all selected objects, which do not correspond to the specified parameters. This mode allows the designer to select objects by type and area. Use box selection and Ctrl hotkey to define an area, then select Keep Selected mode which will deselect unspecified objects.

2.6.2. Cross Selection

DipTrace features Cross Selection and Cross Highlight between the Schematic and PCB, meaning that when objects (components, nets and pins) are selected or highlighted in the Schematic Capture, they are simultaneously selected/ highlighted in the PCB and vice versa.

To enable this feature, go to Edit/ Cross Selection in the main menu and mark Enable Cross Selection in the pop-up dialog.

You can choose which objects will be selected or highlighted, and which actions will be synchronized between both modules when using this function.

To use this feature, make sure related schematic is assigned to the PCB (in the PCB Layout module got to File/ Layout Information from the main menu and in the Related Schematic section of the dialog press button to browse for and select the related schematic file).

2.6.3. General functions

There are following general editing functions: Delete, Cut, Copy and Paste.

Select objects before applying these functions.

To apply one of these functions to the objects, select a corresponding sub-item from the main menu ("Edit"). It is possible to use default hotkeys: Cut (Ctrl+X), Copy (Ctrl+C), Paste (Ctrl+V), and Delete (Del). Copying is also possible between the program instances.

To create the matrix based on selected objects, select "Edit \ Copy Matrix", define the number of columns and rows, spacings, and press OK.

2.6.4. Undo/Redo function

To cancel the last editing step and return to the previous state, select "Edit \ Undo" from the main menu or press the corresponding button on the Standard toolbar.

It is also possible to recover canceled steps. Choose "Edit \ Redo" from the main menu or press the corresponding button on the Standard toolbar. If you edit symbol after using the Undo tool, Redo tool becomes inactive.

You can select whether to consider Zoom a separate editing step or not, using Undo/ Redo Zoom item of Edit menu.

2.6.5. Undo/Redo Zoom

You can select whether to consider Zoom a separate editing step or not, by choosing from the following options:

Change if action not visible. If the editing step being canceled does not belong to the currently visible area of the design field, the first Undo command will return the view to the previous scale to make the location visible again; the second Undo command will cancel the action. If the location is visible on the design area, the first Undo command will cancel the action.

Change Always. The change of the scale is always considered as a separate editing step. Undo command returns the view to the previous scale.

Do Not Change. Undo command cancels the last editing without changing the scale.

2.6.6. Move/Rotate objects

To change location of some objects select them, and drag to a new location. If you move components, all wires connected to them will also change.

You can use the arrow keys to move selected objects. Hold down the Shift key for orthogonal moving.

To rotate object counter-clockwise, select it, and press R hotkey or select "Edit \ Rotate" from the main menu.

2.6.7. Align Objects

Select objects on the design area, then go to "Edit \ Align Objects" from the main menu, or right-click on one of the objects and select Align Objects from the submenu.

Select the alignment direction, then select how to align objects in the row or column (left, center or right) and set distribution settings by objects' boundaries or equally with a custom spacing.

You can group multiple objects into one so they will stay together if they are aligned or distributed.

At least two objects (or groups of objects) have to be selected for the Align tool to become available because the alignment is relative.

2.6.8. Group

Group is an abstract object which unites several design objects. Group defines some similar editing properties: fixed position relatively to each other, rotation according to the center of the group, all objects of the group will be selected when one of them is selected.

Borders and center point of a group are clearly marked. When any object of the group is highlighted – the group is highlighted.

To create a group, select objects, and go to "Edit \ Group" from the main menu. To ungroup objects, select any object of existing group, and go to "Edit \ Ungroup" from the main menu or use the right-click submenu. Visibility of menu items depends on the state of selection.

2.6.9. Lock/Unlock objects

To lock selected objects (prevent moving, editing, etc.) select objects first, then right-click on one of them, and choose Lock Selected from the submenu, "Edit \ Lock Selected" item from the main menu or press Ctrl+L default hotkeys. To unlock selected objects, go to "Edit \ Unlock Selected" from the main menu or Unlock Selected from the right-click submenu. Locked objects highlight in lower contrast when selected.

2.6.10. Working with sheets

Schematic may contain several sheets. To connect signals on different sheets, use bus connectors, net ports, connecting without wires, and connection by name. To add new sheet to schematic, select "Edit \ Add Sheet" from the main menu.

All sheets of the schematic are listed as tabs in the bottom-left corner of the design area:

To change current sheet, left-click it or right-click to open the sheet submenu. You can insert, delete, rename, move sheets left or right, and change sheet type. Hierarchy blocks are created based on the sheets, they are displayed together with regular sheets on this bar. To change sheet type, select "Edit \ Sheet Type" from the main menu (available for 2nd+ sheets), or right-click on the sheet tab, and select "Sheet Type \ Hierarchy" from the submenu. See Hierarchy for details.

You can move objects between schematic sheets, just right-click on an object, and select Change Sheet from the submenu.

A wire can show the direction of the signal for convenience. Right-click on a wire, and select Direction Arrows from the submenu, then select either Forward or Backward.

To remove the arrow, right-click on the wire, and select Direction Arrows from the submenu, then select None.

2.7.1. Electrical rule check

ERC feature allows the designer to check electrical rules for the schematic. To set up ERC, select "Verification \ Electrical Rule Setup" from main menu.

Check the Pin Type checkbox to verify the compatibility of connected pins according to the colored grid. Left-click in the corresponding grid cells (where the  pin types cross) to set up errors and warnings. Errors are red, warnings – yellow, green means that pins of selected types are compatible.

Check Not Connected checkbox and DipTrace will consider all not connected pins as errors.

Check Pin Superimposing checkbox – DipTrace will consider all superimposed pins as errors.

Check Only One Pin in Net – DipTrace will consider all nets with only one pin as errors.

Short Circuit – DipTrace verifies if pins with Power and Ground type are somewhere connected together causing the short circuit. Power and Ground pins have the same electrical type, therefore ERC uses the pin name masks to recognize these pins (use Power Pins for SC section below to set up the nets).

Press Run ERC to launch verification, or go to "Verification \ Electrical Rule Check" from the main menu. The error list or "No Errors" message will pop up. To localize an error, double click it in the list of errors. Launch the ERC again after fixing the errors to ensure that schematic is correct.

2.7.2. Hierarchy check

Hierarchy should always have strict tree structure without "closed" loops. Hierarchy verification allows the user to find these loops and reports them as errors.

A typical closed loop situation: Block_1 includes Block_2 inside it, Block_2 includes Block_3, and Block_3 includes Block_1.

To run this verification select "Verification \ Check Hierarchy" from the main menu.

2.7.3. NGSPICE Simulator

DipTrace features a built-in mixed-level/mixed-signal electronic circuit simulator. To launch it, go to 'Tools/ SPICE Simulator' from the main menu.

In the pop-up window you can select and set up the parameters for the Small-Signal AC, DC Transfer Function, Transient and Noise simulation - just select the respective tab and enter the required values. To check SPICE value Prefixes, press button.

If you are designing a digital circuit, use Digital tab to run the simulation.

As soon as the simulation parameters are set, select ground net from the GND Net drop-down and press Run Simulation button.

Remember to define SPICE models for all the components of the circuit before running the simulation.

Double-click on the item in the All Signals list or use and buttons to add a signal to or remove it from the simulation chart. Press button to select a component or net directly on the schematic.

Right above the simulation Chart you can see a panel with a set of tools that facilitate its management:

- select an area on the graph you want to zoom in; you can also use the mouse wheel to zoom the chart in and out;

- return to the original zoom extents;

- return to the previous scale.

You can also select Black or White background from the drop-down.

Mark the Crosshair Cursor check-box to change the shape of the cursor.

Press Export CSV to save a file with the simulation values.

To save the chart as an image in the PNG, JPEG or BMP format, press the Save Picture button.

Use check boxes next to the signals in the list on the right of the graph to display or hide the signal trace.

To highlight the trace that represents a signal, hover over the colored line next to it.

To change the color of the line that represents a signal, left-click on it in the list of signals and select a new color.

2.8. Plugins

DipTrace supports plugins, allowing the software's functionality to be extended and customized according to users' needs. This means that users can enhance their design process by adding specific features or automations that are not available in the default software.

Plugins can be created using any programming environment, offering flexibility to developers with different coding preferences and expertise. Whether you are proficient in C++, Python, or another programming language, you can develop plugins to integrate seamlessly with DipTrace.

To help users get started, DipTrace provides sample plugins along with their source codes. These examples serve as a valuable resource for learning how to develop and implement plugins.

In the Schematic Capture Convert Shapes to Dash/Dot Lines plugin is available. It allows users to convert selected shapes in their design into dashed or dot-dashed lines. It offers customization options for units, line types, and sizes of dashes and dots.

2.8.1. Convert selected shapes to Dash/ Dot

To convert a shape to a dash line, place and/ or select it in your schematic. To run the plugin go to Tools/ Plugins in the main menu and select Convert selected shapes to Dash/ Dot.

If you don't have .NET 8.0 installed, you will be prompted to install it.

In the pop-up dialogue set the Parameters as required:

Units: mm, mil, inch

Line Type: Dashed or Dot-Dashed

Dash and Dot Size and the Space between the elements.

Mark Dot Size as Line Width to automatically adjust the dot size to match the Line width.

Mark Adjust Dash Size to allow the software to determine the dash size.

Click OK to apply the changes.

Click Cancel to discard changes.

2.9.1. Print

Use the Preview dialog box before printing the schematic (we recommend printing directly from the Preview dialog box).

To print design without previewing it (which we do not recommend), select "File \ Print" from the main menu or press button on the Standard toolbar. Schematic on the paper is what you actually see on the design area. It is also possible to show the page borders and titles on the design area.

To change title properties, use Titles and Sheet Setup dialog box.

You can use title templates or create your own title blocks with the Title Block Editor.

2.9.2. Preview

To open the Preview dialog box select "File \ Preview" from the main menu or press button on the Standard toolbar.

Schematic sheet is automatically scaled to fit the preview area. To change the scale of the sheet from 10% to 600%, use the Scale drop-down list.

Drag and drop to move sheet around a preview area.

Use button to move schematic inside the sheet and the Print Scale drop-down list to change the circuit's size relatively to the sheet. Zoom In and Zoom Out easily.

Scale to Page checkbox scales the schematic and the sheet titles to fit the page.

If the Scale Tables item is checked, all tables on the schematic will be scaled when Print Scale value changes.

Press the Print All button to print all sheets and the Print Current Sheet button to print only the current sheet. Use Current Sheet drop-down list to change the current schematic sheet.

You can save your schematic as a PDF file or an image by pressing Export PDF or Save Picture buttons correspondingly.

To use custom colors for printing, press button.

2.9.3. Titles and sheet setup

To set up the sheet size, edges, titles and create custom title blocks, select "File \ Titles and Sheet Setup" from the main menu or press button on the Standard toolbar.

In this dialog box you can set sheet size, border margins, zones and title blocks.

The user can place up to four title blocks inside the sheet border (at four corners of the sheet) and two title blocks outside the sheet border (in the top-left and bottom-left corners). Zones are marked with numbers on top and bottom sides and with characters on left and right sides. It is possible to set two-zone marking templates: ANSI or ISO with Sheet Template drop-down list. Save titles and sheet sizes as the sheet template, just press .

Check Display Zone Border checkbox to show the outside zone border. Set zone width by X and Y axes.

Use the Title Block Editor to create your own or edit existing title blocks. Press Title Block Editor button to launch the editor.

To change print settings and select printer, press Print Settings button.

Sheet size and orientation depend on the printer settings. To change sheet parameters manually, press Sheet Size button.

It is possible to apply changes only to current sheet or to all sheets of the schematic.

2.9.4. Title block editor

To open the Title Block Editor, select "File/ Title and Sheet Setup" from the main menu and then press the Title Block Editor button in the pop-up dialog box.

To create a new title block, press Add button or press Duplicate to get a copy of selected title block template. Then select a title block template from the list, and press Create Title Block button. In the pop-up dialog box enter the width and height of the title block, number of columns/rows, and press OK.

DipTrace will create a new block with columns and rows of equal size, depending on the total width/height of the block. Width and height of each column/row can be changed in the block editing field, just drag and drop size field borders (cells on the top and left sides of the Block editing field) or click them and enter exact values.

To create a text field, select one or several cells in the Block editing field, and press Create Text Field button. In the pop-up dialog box enter the text, select font, font parameters, alignment, and press OK or leave it blank to add text directly on the sheet. Field borders will be highlighted in red, they are invisible on the sheet. To draw or erase field border lines on the invisible cell borders, select required cell/s and press the corresponding button to add or delete the border lines.

Cells without a field are shown with gray color, regular fields (blank text fields) – with white color, fields with predefined text – aqua color, selected cells – dark blue color.

Press OK to save a title block and close the dialog box. All changes and custom fields are saved automatically and can be reapplied to other projects.

Notice that if you've made changes in active title block, you need to select it again in the Title Blocks tab in order to update the titles on the design area.

3.1.1. Main window

DipTrace PCB Layout main window includes the design area, main menu, toolbars, the Component Placement panel, Design Manager with layers/objects/properties panel, and the status bar at the bottom (hint area and cursor coordinates).

You can place and edit different objects (components, ratlines, traces, copper pours, shapes, tables, etc.) on the design area.

The main menu provides access to all common program features. Main menu: File, Edit, View, Objects, Placement, Route, High Speed, Verification, Library, Tools, Help.

Other interface elements:

Standard Toolbar – tools to work with files, cut/copy/paste objects, print, preview and configure titles, launch 3D Preview, change scale and grid size.

Elements Toolbar – tools to switch to the default mode, the ruler tool, change origin, apply search filters, select component placement side of the board, create ratlines, pads, vias, mounting holes, copper pours, board outline, dimensions, and tables.

Route Toolbar – tools to create and edit traces, run and set up the autorouters, check design rules, select current signal layer.

Drawing Toolbar – tools to draw shapes and polygons, place texts and images.

Placement Toolbar – arrange components and auto-placement tools.

High Speed Toolbar – define and edit differential pairs, add meanders, and phase tune tool.

Place Component (Library Manager) – work with libraries and components. Library groups, library tools, search filters, pattern preview. Search and place components on the design area.

Layers/Objects/Properties panel – (active tab depends on selected object/tool/mode).

Layers tab – work with layers (show/hide, add/delete/edit, change stack position and color) and change layer display mode;

Objects tab – show/hide different objects on the design area and block certain objects from being selected;

Properties tab – edit properties of selected tool/object.

Design Manager – navigates the user around the layout. Left-click in the list of components or nets to highlights object on the design area, double click to pan to selected component/net.

Status Bar shows (left to right) the current hint, mode, view, snap to grid status and cursor coordinates.

3.1.2. Toolbars

DipTrace PCB Layout has six toolbars, the Place Component panel, and Design Manager:

Standard toolbar

New – create a new layout. If current project has unsaved changes, DipTrace will offer to save it. PCB Layout can open one project at a time. If you would like to open several layouts, for example, to copy objects between them, just run several instances of DipTrace PCB Layout.

Open – open existing layout (*.dip) or schematic (*.dch) file.

Save – save current layout. If current project has unsaved changes, DipTrace will offer to save it. The program saves changes into the previously selected file. This tool is active only if there is unsaved activity.

Print – print the current layout. We recommend printing from the Preview panel. Sheet settings and titles are set in the Titles and Sheet Setup dialog box.

Preview – print preview dialog box.

Titles and Sheet Setup – open Titles and Sheet Setup dialog box to select sheet size and orientation, border margins, titles, zones, open the Title Block Editor, etc.

3D Preview – preview the circuit board in three dimensions (3D component models for patterns should be downloaded and connected to the patterns). Configure the folders with 3D models using the "Tools \ 3D Preview \ Patterns and Models Search..." main menu item. 

Panelizing – open Panelizing dialog box to configure panelization of the current layout with V-scoring or Tab Routing options.

Cut – move selected object/s to the clipboard.

Copy – copy selected object/s.

Paste – paste object/s from the clipboard.

Undo – one editing step backward.

Redo – one editing step forward. This tool is active only after using the Undo tool. If you edit a layout after using the Undo tool, the Redo tool becomes inactive.

Zoom Window – set current scale and pan layout to defined area.

Zoom Extents – set current scale and pan layout to show all objects.

Undo Zoom – return to the previous scale and panning.

Scale – define the layout scale (from 25% to 800% or type in a new value). Changing the scale is possible with the mouse wheel, Plus sign (+) and Minus sign (-) hotkeys or from the main menu.

Grid Size – select current grid size from the drop-down list or type in a new value.

Route toolbar

Route Manual – draw traces manually.

Edit Traces – edit existing traces with respect to 90- and 45-degree angles. It is activated automatically when you try to edit traces in the Default mode.

Free Edit Traces – edit existing traces by moving nodes and lines anywhere, no restrictions.

Routing Setup – set the trace width and clearance of Default net class, default via style dimensions and copper to board clearance. Set up manual routing settings in the corresponding tab.

Run Autorouter – launch autorouter.

Autorouter Setup – set up current autorouter.

Check Design – verify a current design, verification reports various types of errors (crossed traces, small clearances, size, and differential pair routing violations, etc.). Errors are shown with red or magenta circles and red arrows directly on the design area and in the error list. The list of errors appears in the upper-right, you can navigate the layout and fix errors step-by-step. It also shows where to setup design constraints.

Design Rules – set up the design rules. Launch and set up the real-time DRC in this dialog box (the same rules as for regular DRC apply).

Current Signal/Plane Layer – drop-down list to select current signal/plane layer.

Elements toolbar

Default Mode – enable the default mode (activated with Esc key or right-click on the blank spot on the design area).

Measure (Ruler) – measure spacings and sizes while designing a PCB. Click on the start point and move the mouse cursor to the end point. The length is shown in the lower-left corner of the screen, in the hint area.

Define Origin – define the design origin visually with the mouse pointer.

Place Component – component placement dialog box.

Component Placement Side (drop-down menu) – select a side of the circuit board where to place components.

Find Component – search filters dialog box.

Place Ratline – create a logical connection (ratline) between two pads by left clicking them.

Place Pad – place a separate pad on the design area.

Place Static Via – place static via. Select current via style on the Properties tab.

Place Mounting Hole – place a mounting hole on the design area. Default hole dimensions are set in the Properties tab on the Design Manager when Place Mounting Hole tool is active.

Pads and Mounting Holes can be parts of patterns as well as separate objects.

Place Fiducial – place a fiducial on the design area.

Place Copper Pour – draw the copper pour polygon on the current signal/plane layer.

Place Board Outline – place the board outline polygon.

Place Dimension – place horizontal, vertical, free, radial dimensions and pointers from the pop-up submenu.

Place Table – place table on the layout. Table are usually in assembly or silk layers.

Placement Toolbar

Arrange Components – place all components next to the board outline (inside or outside it). It's not a component placement. This feature is used after converting from Schematic to arrange chaotic location of components, just to make layout easy to navigate.

Run Auto-placement – place all unlocked components with optimization by connection length. DipTrace tries to find the best places for each component in order to make routing as easy as possible.

Auto-Place Selected – auto-place selected components only.

Placement Setup – the placement setup dialog box. Change auto-placement accuracy, spacings and other parameters.

Drawing Toolbar

Place Shape – Line, Arc, Rectangle, Filled Rectangle, Ellipse, Filled Ellipse, Polyline, Filled Polygon.

Place Text – place custom text directly on the design area.

Place Image – place an image from the file directly on the design area.

Place QR Code – generate and place a QR code containing a URL or text information.

Layer drop-down list – select the circuit board layer where new shapes and objects will be placed. You can also change the layer of existing objects later using the right-click context menu.

High Speed Toolbar

Define Differential Pair – create a differential pair (define positive and negative nets of the pair, change color, net class, and review a pair properties).

Edit Single Track of a Pair – move/edit only a single track of a differential pair with respect to 45- and 90-degree angles. The second track does not move, like if it was edited with the regular trace edit tool.

Free edit single track of a Pair – move/edit only a single track of a differential pair without any constraints. The second track does not move like if it was edited with regular free edit tool.

Add Meander – apply meanders to copper traces on the design area for length matching.

Phase Tune – calculate phase shift between the tracks of a differential pair and apply custom and auto-sized meanders to compensate it.

3.1.3. Place Component panel

Price and Availability - check the selected component’s price and availability on the Mouser website or across our supplier database.

3.1.4. Design Manager

This panel is on the right side of the screen. To display/hide the Design Manager, select "View \ Toolbars \ Design Manager" from the main menu or press Ctrl+2 hotkeys by default.

There are three tabs in the upper part of the Design Manager.

Layers tab – change and manage board layers (add/move/delete/hide layers, change settings and layer display mode). Blue check marks – show/hide the layer, color rectangle – change the layer color. Double-click on the layer name to make this layer active.

Objects tab – show/hide different objects on the design area and block certain objects from being selected.

Properties tab – editable properties of selected tool/object.

Right below is the Design Manager, it allows the designer to navigate through the layout. Press button to see the list of components, and press button to see the list of nets. Select component or net in the list, and all pins of selected object will appear in the list right below. Left-click in that list to highlight an object, or double-click it in the list to pan the design area to selected object. You can right-click on any component, net or pint in the list to open its submenu.

To adjust the width of the Design Manager panel, hover the mouse pointer over its edge,  then drag and drop it.

3.1.5. Status Bar

Status bar is located in the bottommost part of the PCB Layout window.

It shows the following information:

Hint - depending on the selected option, displays standard or detailed pop-up hint (containing pad/via/hole dimensions, trace length) for the objects on the design area.

Mode - shows the current mode (Default, Route Manual, Edit Traces, etc.).

View - the current view (Normal, Mirror).

Grid Snap - the current Snap to Grid (link PCB Layout > View functions > Grid) status.

X, Y - coordinates of the current position of the cursor or selected element.

3.1.6.1. File

New – create a new layout. If current project has unsaved changes, DipTrace will offer to save it. PCB Layout can open one project at a time. If you would like to open several layouts, for example, to copy objects between them, just run several instances of DipTrace PCB Layout.

Open – open existing layout (*.dip, *.dipxml) or schematic (*.dch, *.dchxml) file.

Open Recent – open 5 last layout projects.

Save – save current layout. If the project has never been saved, specify the file name in the pop-up dialog box, otherwise the project is automatically saved into the file. This tool is active only if a current layout has unsaved changes.

Save as – save layout into selected file.

Save Selected As – save selected objects into the file.

Import – import layout or its part from DipTrace ASCII, DipTrace XML, DXF, Gerber, N/C Drill, ODB++, Altium, Eagle XML, KiCAD, P-CAD ASCII, P-CAD PDIF, PADS ASCII, OrCAD Min,  Sprint-Layout, Interchange, Autorouter SES as well as netlists from Accel, Allegro, Mentor, OrCAD, PADS, PCAD, KiCAD, Protel 2.0 and Tango formats.

Export – export layout to DipTrace ASCII, DipTrace XML, DXF, PDF, Gerber, Gerber X2, N/C Drill, ODB++, IPC-2581, IPC-D-356A, Bill of Materials, Pick and Place, G-Code for Solder Paste Dispensing, Mach 2/3 Drill, OrCAD TAP Drill, P-CAD ASCII, PADS PCB ASCII, OrCAD Min Interchange, Eagle XML and Autorouter DSN formats.

Order PCB – order PCB manufacturing with Bay Area Circuits (California), PCBWay (China) or Aisler (Netherlands).

Titles and Sheet Setup – Titles and Sheet Setup dialog box to set sheet size and orientation, border margins, titles, zones, and open the Title Block Editor.

Preview – preview and customize printing options (size, scale, colors, etc.) before printing.

Print – print current design. We recommend to print from the Print Preview panel. Sheet settings and titles are set in the Titles and Sheet Setup dialog box.

Layout Information – general information about the circuit board: current and a maximum number of pins, patterns, nets, vias, jumpers, holes, layers, routed nets, a length of traces, board width, height, total board area, and related schematic.

Update Layout from Schematic – synchronize the PCB layout with the source schematic file. New components, footprints, and nets are added automatically while preserving the existing board layout and routing whenever possible.

Update Layout from Netlist – update the PCB layout using an netlist file. Supported netlist formats include Accel, Allegro, Mentor, OrCAD, PADS, P-CAD, Protel, Tango, and KiCad.

Recover Board – recover the latest project. Use this feature when the program was incorrectly closed or the project was not saved for some reason. Recovery file is saved automatically every 10 steps.

Recovery Options – configure the recovery options: turn ON/OFF recovery and change number of steps to record.

Exit – close the PCB Layout. If current project has unsaved changes, DipTrace offers to save it.

3.1.6.2. Edit

Undo – one editing step backward.

Redo – one editing step forward. It is active only after Undo. If you edit the layout after using the Undo tool, the Redo becomes inactive.

Undo/ Redo Zoom – select if to consider Zoom a separate editing step or not.

Cut – move selected objects to the clipboard.

Copy – copy selected objects.

Paste – paste objects from the clipboard.

Delete – delete selected objects.

Select All – select all objects on the design area.

Edit Selection – select objects by type, layer, etc. automatically.

Cross Selection - enable cross selection between Schematic Capture and PCB Layout, choose objects and actions to be included in this function.

Find in Layout – find specified component or net on the layout. Search layout by full or partial RefDes, Value or Name.

Copy Matrix – create the matrix based on selected object/s. Specify the number of rows, columns and row/column spacings.

Keep RefDes while Pasting – keep all reference designators when pasting another layout. Select this option if panelizing different layouts on a single board.

Rotate – rotate selected objects 90 degrees counter-clockwise. If objects form a group, they have a common center of rotation. Otherwise, each has its own center of rotation.

Rotate Group – rotate selected objects around one common center point.

Flip Group – flip selected objects vertically and horizontally.

Align Objects – align selected objects horizontally or vertically and distribute them equally.

Radial Placement – place selected objects radially with defined placement center, radius, step or distribute them equally between specified circonference angles. The feature can be applied to components, pads, mounting holes, vias and fiducials.

Group – unite all selected objects into a group. This tool is active only if several objects are selected.

Ungroup – ungroup selected objects. This tool is active only if at least one group is selected.

Lock Selected – lock moving and editing of selected object/s.

Unlock Selected – unlock moving and editing of all selected objects, if they were previously locked.

Lock Components – lock moving and editing of all components on the top or bottom side of the board.

Properties – the properties of selected objects.

3.1.6.3. View

Toolbars – show/hide the toolbars.

Display Hint – select whether to show a standard or detailed pop-up hint (containing pad/via/hole dimensions, trace length) for the objects on the design area. The hint is always displayed in the bottom-left corner of the screen.

Place Component Preview – show component's footprint before placing it on the design area.

Component Markings – configure default component markings, font, location, etc.

Pad Markings – enable/disable the display of Pad Numbers, Net Names or both as markings of the pads.

Trace Markings –  enable/disable the display of Net Markings showing the net names on the traces.

Move Component Texts (F10) – use this tool to move reference and other designators to desired position.

Objects – show/hide layout objects by types. All objects (except pattern dimensions) are visible by default.

Ratlines – optimize, show/hide ratlines (connections).