duplicate board/schematic 6 times

Drawing Schematics, Hierarchical Design, BOM, Exporting net-lists, etc.
Post Reply
Message
Author
dhgrundysr
Posts: 7
Joined: 08 Mar 2016, 11:49

duplicate board/schematic 6 times

#1 Post by dhgrundysr » 18 Jun 2016, 23:28

Is there a way to duplicate an existing schematic / board 6 times onto a new board/schematic and then have the new board and schematic match up with each other without having to reroute all the new sections?? (After that i will be adding in some more support circuitry and doing the extra routing for it).

thanks,

Dave Grundy

Tomg
Expert
Posts: 1385
Joined: 20 Jun 2015, 14:39

Re: duplicate board/schematic 6 times

#2 Post by Tomg » 23 Jun 2016, 05:19

dhgrundysr wrote:"...Is there a way to duplicate an existing schematic / board 6 times onto a new board/schematic and then have the new board and schematic match up with each other without having to reroute all the new sections?..."
Not to my knowledge. It sounds like you are looking for a feature similar to Altium's "Room" and Allegro's "Module". I was thinking that you could layout one sub-circuit in DipTrace's PCB Layout editor and then copy and paste it as many times as you want. The reference designators would automatically increment with each paste operation. Unfortunately, DipTrace does not have complete backward annotation, which would allow you to bring everything including the Net structure into the schematic. To accomplish what you want, DipTrace needs a special tool that works in conjunction with the hierarchy tool. You might want to try submitting this idea in the Feature requests forum.

-- 22 Jun 2016, 09:21 --

*** EDIT ***

After a little experimentation, I finally figured out how to create multiple sub-circuits in DipTrace. It's a bit involved...

Schematic Editor
1) Create the first schematic sub-circuit above the schematic page border (away from any other circuitry) on the left side without connecting it to any other circuitry, group it (select all of its elements and press Ctrl G) and resave the schematic.

PCB Layout
2) In the Main Menu click on File, choose Renew Layout from Schematic in the drop-down menu, select By Components... in the fly-out menu and choose the related schematic file. The new sub-circuit components should appear on the right side of the PCB outline.
3) Place and route the new sub-circuit above the PCB outline (away from any other circuitry) on the left side without connecting it to any other circuitry, group it (select all of its elements and press Ctrl G) and resave the PCB.

Schematic Editor
4) Copy the first sub-circuit, paste the desired number of copies to its right (above the schematic page border), line them up across the same row (identical vertical coordinates) and resave the schematic.

PCB Layout
5) Copy the first sub-circuit, paste the same number of copies to its right (above the PCB outline) in the same order and line them up across the same row (identical vertical coordinates). Make sure that all PCB sub-circuit reference designators match their schematic counterparts. If a correction is needed, do it manually; do not use the reference designator renumbering tool.
6) In the Main Menu click on File, choose Renew Layout from Schematic in the drop-down menu, select By RefDes... in the fly-out menu and choose the related schematic file. The sub-circuit routing should remain intact.
7) Resave the PCB.
8) Test for proper linking to the schematic: In the Main Menu click on File, choose Renew Layout from Schematic in the drop-down menu, select By Components... in the fly-out menu and choose the related schematic file. The sub-circuit routing should remain intact.

Schematic Editor
9) Move all sub-circuits to the desired locations, connect them to the rest of the schematic and resave the schematic.

PCB Layout
10) Move all sub-circuits to the desired locations, in the Main Menu click on File, choose Renew Layout from Schematic in the drop-down menu, select By Components... in the fly-out menu and choose the related schematic file. New ratlines should appear showing the new Net connections between the sub-circuits and the rest of the layout.
11) Route the new Nets and resave the PCB.
Tom

Post Reply