0
\$\begingroup\$

In Altium, it seems no connect (NC) pins in a given IC create a net that wants to connect them all together. I've been looking for some parameter we may have set when the part was created that forces a NET on these pins, but haven't found one yet. Anyone know why this is happening?
It generates a DRC unless these NC pins are tied together. There is no net on these pins on the schematic.

I have IC symbols on a schematic that have NC pins. These pins are identified as NC via the special DRC marker (i forget what it is called) that identifies them as NC nodes). On the PCB layout, these want to be connected together with a net (the ratsnest lines show up for these, connecting them together), even though the 'Not connected" symbol or marker is placed on the NC pins. It could be that the issue is that the pins on the schematic symbol are grouped symbolically into a single pin, with the pin numbers listed with commas. However, this is a legitimate way of grouping similar pins together (VCCs, GNDs, etc) where the symbol shows just the one pin, and all the pins associated with that function or connection (ie, VCC, GND, NC, etc) are listed in the properties,comma separated. The NC pins on the schematic have the no-connect symbol attached to them, and there are not nets tied to those pins on the schematic.

\$\endgroup\$
7
  • 1
    \$\begingroup\$ This link will take you to an excellent (and official) Altium resource: forum.live.altium.com \$\endgroup\$ Jun 1, 2023 at 15:13
  • \$\begingroup\$ Did you label them "NC"? \$\endgroup\$
    – Mattman944
    Jun 1, 2023 at 15:21
  • 1
    \$\begingroup\$ It migth be useful to see the component on the actual schematic, and maybe also the component in the schematic library editor showing the pin names etc ... \$\endgroup\$
    – citizen
    Jun 1, 2023 at 15:34
  • \$\begingroup\$ @Mattman44, on the schematic symbol in the library? Yes. There are multiple pins named NC on the symbol. \$\endgroup\$
    – jrive
    Jun 1, 2023 at 20:36
  • \$\begingroup\$ What label does it give the net it wants to connect all the NC pins to? \$\endgroup\$
    – brhans
    Jun 2, 2023 at 0:41

2 Answers 2

1
\$\begingroup\$

After speaking with Altium, the problem stems from the way in which the pins were created in the schematic symbol. Basically, if you assign multiple pin numbers to a single pin, Altium will not treat them as individual pins to which to attach the "NO DRC Marker", but instead will connect them together. So, the solution is to individually create all the NC pins (which you can then make invisible -of course). enter image description here

\$\endgroup\$
1
  • 2
    \$\begingroup\$ I believe you could also avoid this problem by not having the NC pins on the schematic symbol (not just hiding them, but not having them at all). The PCB program should not complain if the PCB footprint has more pins than the schematic symbol. \$\endgroup\$ Jun 6, 2023 at 17:38
0
\$\begingroup\$
  1. Make sure the footprint has unique pin numbers
  2. Make sure the NC pins are not tied together in the schematic
  3. Turn off the DRC rule for NC pins
\$\endgroup\$
1
  • \$\begingroup\$ 1 and 2 confirmed....don't want to do 3....I contacted Altium....I'll post response here when I get it.... \$\endgroup\$
    – jrive
    Jun 1, 2023 at 20:22

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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