Oval shape for custom paste file

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
dhgrundysr
Posts: 7
Joined: 08 Mar 2016, 11:49

Oval shape for custom paste file

#1 Post by dhgrundysr » 13 Apr 2019, 23:28

How do i make an oval shape for an IC for a special smt paste requirement? Oval is an option for pads but not for shapes.

thanks
Dave Grundy

Tomg
Expert
Posts: 1386
Joined: 20 Jun 2015, 14:39

Re: Oval shape for custom paste file

#2 Post by Tomg » 14 Apr 2019, 08:18

Do you want something like this?...
oval_paste.gif
You do not have the required permissions to view the files attached to this post.
Tom

dhgrundysr
Posts: 7
Joined: 08 Mar 2016, 11:49

Re: Oval shape for custom paste file

#3 Post by dhgrundysr » 15 Apr 2019, 23:26

Yes. How??
Thanks!

Tomg
Expert
Posts: 1386
Joined: 20 Jun 2015, 14:39

Re: Oval shape for custom paste file

#4 Post by Tomg » 16 Apr 2019, 08:28

You can import one oval shape from a DXF file created in your favorite 2D CAD program and then copy and place it as many times as you need* or, if you don't have a 2D CAD program, you can use DipTrace to make all of them at once as follows...

1) Open a new (empty) session of the PCB Layout editor and place the standard version of the desired pattern centered around the origin of the Design Area.
2) Right-click on one of the pads and select "Pad Properties..." in the pop-up menu to bring up the Pad Properties dialog window.
3) In the Pad Properties dialog window disable (uncheck) the []Use Pattern's Pad Properties option, choose an Oval pad shape, select "All Similar" in the Apply To: drop-down list and click on [OK]. All pads should change to an oval shape.
4) In the Main Menu click on "File", choose "Export" in the drop down menu and "Gerber..." in the fly-out menu to bring up the Export Gerber dialog window.
5) In the Export Gerber dialog window select/highlight the Top Paste layer, make sure Units: is set to your current working units, enable the [x]Use Design Origin option and click on the [Export] button to bring up the Save As dialog window.

6) In the Save As dialog window navigate to a convenient folder (e.g. Desktop), give the file a name (e.g. "Top Paste"), click on the [Save] button and, finally, click on the [Close] button to close the Export Gerber dialog window.
7) Right-click on one of the pads and select "Pad Properties..." in the pop-up menu to bring up the pad properties dialog window.
8) In the pad properties dialog window re-enable (check) the [x]Use Pattern's Pad Properties option, select "All Similar" in the Apply To: drop-down list and click on OK. All pads should change back to their original shape.
9) Right-click on one of the pads and select "Mask/Paste Settings..." in the pop-up menu to bring up the Mask/Paste Settings dialog window.
10) In the Mask/Paste Settings dialog window set both Top Paste and Bottom Paste to "No Solder", set Apply To: to "Similar Type/Size Pads" and click on OK. This step will suppress the default paste shape of all pads to allow the modified paste shape to take its place.

11) In the Main Menu click on "File", choose "Import" in the drop down menu and "Gerber..." in the fly-out menu to bring up the Open dialog window.
12) In the Open dialog window navigate to and select/highlight the newly-saved Gerber file (e.g. "Top Paste.gbr") and click on the [Open] button to bring up the Gerber import dialog window.
13) In the Gerber import dialog window set Import Mode: to "Add", Convert to: to "Top Paste" and click on the [Import] button.
14) In the Design Area select all objects (Ctrl + A), right-click on the original component (not its pads) and choose "Group into Component" in the pop-up menu.
15) Give the component a unique name so as not to conflict with other component names in your custom library, eliminate the number suffix on the reference designator, choose your custom pattern library group in the Current Library Group panel (top left side of the screen) and select/highlight the desired target custom pattern library.

16) In the Design Area right-click on the component (not its pads), choose "Save to Library" in the pop-up menu and select Add to "(selected/highlighted pattern library name)" in the fly-out menu to bring up the Confirm dialog window.
17) In the Confirm dialog window click on Yes. You should now see the new pattern name added to the bottom of the pattern list of the selected pattern library on the left side of the screen.**

*Note: If you are going to use a 2D CAD program to create the modified paste shape you will need to perform steps 9 & 10 above to suppress the default paste shapes.

**Note: If the Pattern Editor is open to the same library while trying to save the pattern from the PCB Layout editor, DipTrace will block the action. If this happens, either close the Pattern Editor or choose a different library for the Pattern Editor to be focused on before trying to save the pattern again.
Tom

User avatar
KevinA
Posts: 382
Joined: 18 Dec 2015, 15:35

Re: Oval shape for custom paste file

#5 Post by KevinA » 16 Apr 2019, 12:17

WOW. another collectable from Tomg. Perhaps DT can take the time from creating a board service and address their lack of drawing tools?

Serg
Technical Support
Posts: 311
Joined: 09 Jun 2010, 08:12

Re: Oval shape for custom paste file

#6 Post by Serg » 17 Apr 2019, 09:15

KevinA wrote:
16 Apr 2019, 12:17
Perhaps DT can take the time from creating a board service and address their lack of drawing tools?
We plan to add new drawing tools.
Now we spend our time for new pattern library features.

Post Reply