1
\$\begingroup\$

I've routed a board, and redid my designators in the schematic and updated the changes to the pcb. In doing so, the nets which I have routed, now give me an error. Basically what's happened is that some of the traces netnames haven't been updated.

Yesterday a trace from component A to B had a netname of net_a_to_b. Today after i changed the designators, the trace still holds the net_a_to_b, but the components are now C and D. The trace should have updated to net_c_to_d.

There aren't that many nets, and I can just redo them, but I shouldn't have too.

Does anyone why this happens and how to get it right every time ?

\$\endgroup\$
1
  • \$\begingroup\$ your PCBdoc does not know that other nets have become obsolete, so you near to either "Clean nets" or "clear all nets" as in my answer. \$\endgroup\$
    – KyranF
    Oct 27, 2014 at 22:17

4 Answers 4

2
\$\begingroup\$

In your PCB Doc go to Design tab up in the top toolbar, then Netlist, then Clear all nets. Then re-import changes from schematics, and it will re-assign all the nets, and re-establish traces which do not 'collide' anymore.

Be aware that this may bust the net labels given to polygon pours and vias which are 'free' in the document. I guess just in case, copy the PCBdoc file somewhere as a backup before doing this.

\$\endgroup\$
8
  • \$\begingroup\$ Good tip. Did not know about that. I tried it, but it didnt work. \$\endgroup\$
    – efox29
    Oct 27, 2014 at 22:19
  • 1
    \$\begingroup\$ You can use the PCB inspector to highlight all "track" objects, and with the "same" net name as whatever a_to_b is, and then change them directly to c_to_d or whatever it's real name is. \$\endgroup\$
    – KyranF
    Oct 27, 2014 at 22:24
  • \$\begingroup\$ @efox29 you may also check out the Netlist manager window, and the component classes window perhaps there is something you can fix in there. \$\endgroup\$
    – KyranF
    Oct 27, 2014 at 22:25
  • 1
    \$\begingroup\$ ya or I can just rerun the track. But there has to be another way. If I had more tracks that did this, this would be a time consuming problem. I have like 5 tracks that need some work,I can do it manually, but I'm looking for the correct way to correct this. :( \$\endgroup\$
    – efox29
    Oct 27, 2014 at 22:26
  • \$\begingroup\$ Ill have a look at the netlist manager..heres hoping \$\endgroup\$
    – efox29
    Oct 27, 2014 at 22:28
1
\$\begingroup\$

To avoid having things like this happen, first, make sure your component links are good, and keep them up-to-date. (From within the project, right click on the pcb file, and select components from the context menu.. follow the cues). When all the component links are intact, it is much harder to get the schematic out of sync. I suspect this is your main problem. NEVER change reference designators unless the component links are up-to-date.

Second, when you import changes from schematic, you should have an opportunity to manually match old and new nets. When Altium can figure it out it does it without prompting you. But I think if you change the net name AND add or remove pins, Altium might not be sure how to handle it. In that case, manual matching may help in terms of how it assigns net properties to existing copper.

\$\endgroup\$
2
  • \$\begingroup\$ Is there an easy to match nets ? I do get that prompt, and I just skip it. I see two columns but how do you match nets when you cant even see your schematic anymore ? \$\endgroup\$
    – efox29
    Oct 28, 2014 at 16:15
  • \$\begingroup\$ Usually I can kind of match it by exploring the net. You can expand each net name to see which pins are members of that net. Usually when I expand it and browse the pins, I can figure out what makes the most sense. While not ideal, you can also abort at that point, and go look at the schematic and layout to gather more information if you realize you are not sure what to do. \$\endgroup\$
    – mkeith
    Oct 28, 2014 at 18:26
0
\$\begingroup\$

I had the same problem, I solved it with renaming all mismatched components in schematic editor and then import changes into PCB. After that the nets were OK and I renamed the components back and I once more imported the changes into PCB

\$\endgroup\$
0
\$\begingroup\$

When something like this happens to me I usually shelve the polygons, select the erroneous nets (shortcut E-S-C), cut them at a specific location e.g. a pin, and past them again. This should solve the DRC errors and you will not have to redo the routing.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.