Strange Behavior - Can't figure it out

Question

Trying to Interactively Route, none of my connections will complete, even though they are clearly shown on the schematic.

If I try to update the PCB after a compile (compiles with no errors) I get a dialog which shows my Unmatched Nets. The Unmatched Reference objects show my desired connections. But the Unmatched Target Objects show connections which no longer exist on the board.

I made the *.CSPcbDoc from an older board to inherit the outline, placement of mounting holes, placement of components. But the circuitry itself is quite different than in the old design. None of the listed Unmatched Target Objects are relevant in the new design.

Is there some kind of "lock" that is in place so that new nets are not being created? The Unmatched Target Objects are those peculiar to the older design which was copied.

I also don't understand why the EDIF output has 6 files, one for each page of my schematic. But the nets I've tried to interactively route are shown "joined" in the EDIF.

tarribred61 · Answer

Hi,

What you describe sounds quite normal to me. I will typically reuse the files from an older project to start a new one. I reuse an older PCB doc as a template that I made and it has my sheet symbol and a generic PCB outline and fabrication notes. It has some old ICs, nets and such that won't match my schematic. In your case you want to maintain some of the mechanical features of the old PCB so you are doing the same.

I then start a new PCB project, to create the place to put the existing schematics and PCB template. Existing schematics are often also from an old project that I want to reuse.

You have your schematics compiled and ready to update the PCB. So, all good so far. Presumably the schematic(s) and the PCB are all associated with the project and there is only one PCB for whatever number of schematics you have.

Open the PCB and then use the Tools > Component Links ribbon command to view the un-matched components. You should probably have none matched or maybe only a few. That is OK for now. The matching is based on unique IDs in the schematic and the PCB. However, since you haven't yet gotten the PCB to synchronize to the schematic and the PCB has old parts this would be expected. You cannot match them yet. So,for now just close the edit component links box we just opened and we will get back to this later.

As you mention, it is time to update the PCB based on the schematics. In the schematic view, use the command ribbon, Home > Project > Update PCB... command. You get the failed to match pop up message box. Press yes. It will ask if you want to match manually. When you press yes, you can see the old nets in the PCB (which seems to be what you did). At this point just continue without matching any nets.

You should then have the ECO box declaring what will change. Review this and verify it isn't doing anything you don't want. But it is likely all the things can be done. Click the Validate Changes box. Some errors such as missing footprints are likely if the paths to libraries cannot be resolved. That is OK for now. Execute the changes. In the future, you want to review the ECO box in case you put parts on the PCB that might not be on the schematic. For example, mounting holes, fiducials or other mechanical parts that might be deleted from the PCB by this update process. Note, if your mounting holes you wanted to save will be deleted from above you can untick the boxes before executing the changes. I usually put mounting holes and fiducials on schematics with the footprint call outs to allow these to synchronize properly.

In the PCB the old components should be deleted and the new ones it found footprints for should be brought in and placed off the PCB. Your net lists should now somewhat match and many of the components should have proper links based on the unique ID. Save the PCB. Go back to the PCB > Tools > Component links and looks at the Edit Component Links box. There should be a lot of matched components and some unmatched. I would then match the components based on Designator only. It is likely there are some old PCB parts that have the same designator as the newer schematic. However, they did not match up the unique IDs. Click Add Pairs Matched By button with the Designator checkbox checked. Most of the unmatched parts should move to the matched column and remaining unmatched parts in the schematic are ones it didn't find footprints for. You can deal with that later on. Click the Perform Update button. When completed, save the PCB again.

At this point you should have a reasonable rats nest of nets and can start parts placement. Older PCB parts that it matched are probably still on the PCB area where they were, updated PCB parts that it took from libraries are placed off the PCB and you need to start the process of grouping and placement.

Now you can go back to the schematic and start to go through the PCB update process again. This will show you what footprints cannot be found. Figure out what library links are missing or what footprints you are missing and resolve those issues or you can do that later and work with only what you have done so far.

Once you can synchronize the schematic and PCB without unexplained errors you should be on solid ground.

Good luck.