I’m making a 7 segment display for 8 digits - I’ve done the schematic and layout for one digit and want to now replicate it for the rest. The problem is when I get to the point of hitting “repeat layout” then it just tells me “Copied to 0 rule areas” and does nothing. I’m at a bit of a loss…
I have a master sheet with hierarchical sheets within it.
Each hierarchical sheet is a copy
Master is blank
One hierarchical sheet has a full PCB in it
I add all components to PCB as - I now have one properly laid out digit and 7 “random clusters” of components
Tools > Multi Channel - “Generate placement rule areas” - tick all hierarchical sheets (later on I tried including root sheet too, but no improvement). Tick all options. Closes with no visible issues.
Tools > Multi Channel - “Repeat layout”. Tick all digits. Tick all options. Asks me to select the reference layout which I do, and then the dialog closes and leave me with a yellow ribbon bar message of “copied to 0 rule areas”.
Did you read Multichannel layout - tool not pasting the reference layout ? There were two different problems described there. The Status fields in the Repeat Layout dialog should read ‘OK’, otherwise there’s some problem. The messages seem to be cryptic for an average user, but at least you should tell us what they say (in English).
Instead of using the multichannel feature with a full fledged project my advice is: try the multichannel feature first with a example with 2 subsheets, which only contains 2…3 connected resistors. Make it simple and try to get the multichannel feature working with such a simple project.
If this works you could be sure you know the workflow. If this workflow then later does not work with more complicated projects then it could be a bug.
To give you more spedific answers we would need a attached project so we can examine it more deeply. For instance the status/error message in the “repeat layout” dialog (your last step) is important.
Already found issues:
use simple numbering for references (issue #20058 on gitlab)
run a extra annotation cycle after copying all your subsheets (#20173)
a too complicated subsheet schematic can pose problems (#20177)
Taken advice and created a new project with just a handful of components and it works fine. Bizarre given that all it has is a few diodes and resistors, net labels. Will try gradually building up a new copy and run this process at various points to see if I can recreate when it falls over. Thanks for the help.
I was able to make this reproduceable over my lunch break - how can I share the project file please?
Each segment is 9 diodes and 3 resistors.
I then tried deleting certain segments from the subsheets, updating the PCB and trying to run multi-channel tool on the remaining “shape”. Results below…
All segments - Fail
CDEG - Fail
ABC - OK
FBE - OK
ABCDEF - Fail
CDE - OK
Basically, the algorithm which matches the connectivity in the two sets of components is having problems with your schematic. Can you please add the project archive you’ve created to that gitlab issue as another example?
