Hi,
I have an schematic that I’ll use to route two pcbs (left and right). Which process flow do you recommend?
Thank you
Hierarchical sheets. One for each schematic.
Then you should give more information. Do both pcbs share the same signals?
Are they one circuit and two independent boards?
I’d recommend creating two directories, one for each board. Then just copy the *.sch and *-cache.lib files from one to the other.
I want to share the same schematic for both pcbs (left and right) since one is a mirror of the other.
That is the direct way of doing this but this way someone can apply changes to left schematic per example and forget to update the right schematic.
Hierarchy is convenient, but in fact you don’t ever need hierarchical sheets, although splitting the design into (two in your case) hierarchical sheets has the advantage that when you import the netlist into PCBNEW, the parts come out grouped by sheet.
But you don’t have to split your schematic if you don’t want, as you can lay out and route several boards at once from the same schematics. Only if you have common nets between the two boards (like GND and VCC typically), PcbNew will insist that you have to connect them and will show the ratsnest lines if you don’t do so.
As an example, the image attached shows two boards I’m doing at present. The schematic design is hierarchical, with one sheet per final board.
Then hierarchical sheets sharing the same file is what you need because a change in one of them will be automatically mirrored in the other sheet. ONLY if both schematics are identical.
Who is “someone”? Call one project “xxx_master” and the other “xxx_copy_do_not_edit_schematic”.
Hierarchical sheets don’t help in this case. On Linux you could create a link in the file system, but anyway, if the schematic changes “someone” needs to remember to update both PCBs, so you still need some discipline.
I also do separate schematics/pcbs/projects for left & right, although I have them all in one folder (along with a PSU board).
But is this really a requirement? You can copy the schematic and have double up of every component (in same schematic, separated by sub-sheets or not), then layout both boards in the same layout and have them separated by breakout tabs or V grooves.
Because project-wise, I think it is untidy to refer to the same schematic file for two different end products. I would also consider making two alike, separate projects with only mirrored layouts.
Yes, for both solutions you would have to make the same change twice, but at least in the first suggestion you only need to care for one document package.
Now that I think about it, I think they could. You create a sheet with the schematic, then you create two separate projects and have their schematics simply instantiate the common sheet.
That’s different, though, because DRC will catch the problem when the schematic does not match the PCB.
If you want one schematic to accommodate two boards use the Unit Numbering Method of reference designating from ANSI/ASME Y14.44 (used to be IEEE Std 200), which uses reference designation prefixes. Assign ref des prefix A1 to the left PCB and A2 to the right PCB. You will have A1R1 and A2R1, A1C1 and A2C1, A1U1 and A2U1, etc. The parts list (PL) will list the parts alpha numerically by the ref des prefix but when sorted by part number or value you will see, for instance, A1R1 and A2R2 listed together.
Since I want to have two separate boards I created two schematic.
Hierarchical sheets work if I have both pcbs on same project.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.