11
\$\begingroup\$

I've been bashing my head against a wall for the last day trying to get this to work.. I have a custom schematic and pcb library, when I try to update my pcb document I get the following error:

Unknown Pin Error

I have checked both the schematic symbol and the pcb footprint about a million times and am certain that I have correctly designated the pins.

Pin mapping

I have learned a little bit about using Altium at university, and I have had some success using custom schematic/pcb libraries in the past but for some reason I just can not get this one to work. I've done some searching on the forums for this error but have not yet been able to find a solution that worked for me.

Any ideas/suggestions are welcome! Thank you

EDIT: This is the schematic: schematic

here are the properties of pin 2: Pin properties

and here is the PCB footprint: PCB footprint

\$\endgroup\$
  • \$\begingroup\$ Can we see the schematic? \$\endgroup\$ – MathieuL Jul 8 '15 at 14:32
  • 1
    \$\begingroup\$ Can we see the symbol and the footprint. \$\endgroup\$ – efox29 Jul 8 '15 at 14:50
  • \$\begingroup\$ The pins in the schematic and the PCB libraries must match perfectly. As others have asked, could you post the component symbol and the PCB footprint? \$\endgroup\$ – DerStrom8 Jul 8 '15 at 15:11
  • \$\begingroup\$ I suspect that the footprint for SW1 doesn't have a pin 2. Perhaps the pin is named "2", but has some other number. The pin number on the footprint must match the pin number on the schematic symbol. \$\endgroup\$ – Peter Bennett Jul 8 '15 at 16:38
  • \$\begingroup\$ Maybe you've failed to update the schematic symbol on the schematic and/or the footprint? The library symbol may be perfect (now) but you've got an older version on the schematic, etc. \$\endgroup\$ – Spehro Pefhany Jul 8 '15 at 17:56

11 Answers 11

9
\$\begingroup\$

You probably have edited the the schematic symbol in Sch library after placing its footprint on the layout design.

In situations like this, you need to update your schematic design from library (Tools/Update From Libraries...), then update your PCB with the updated schematic. If problem still there, remove the footprint from PCB file and update the PCB file with schematic again.

Also make sure the symbol in schematic sheet has the same footprint model name as it has in Schematic and PCB libraries.

\$\endgroup\$
  • 2
    \$\begingroup\$ This seems like a thorough and reasonable method to ensure it updates. +1 \$\endgroup\$ – KyranF Aug 21 '15 at 16:17
  • 1
    \$\begingroup\$ I had the same problem, and checked every thing,I updated schematic and all. The solution was update only the footprint (rigth click on component and update PCB with...). \$\endgroup\$ – user94639 Dec 16 '15 at 13:44
3
\$\begingroup\$

To associate pins between schematic documents and footprint documents the pin designators must match. The pins on my schematic were A01, A02, A03, while the pins on the footprint were labeled A1, A2, A3. Changing the schematic to A1, A2, A3, or the foot print to A01, A02, A03, fixed the unknown pin situation.

\$\endgroup\$
  • \$\begingroup\$ Single line answers are subject to downvotes or deletion. Please explain why your solution works, and why the OP's choice is wrong. There is an attempt at some education here... \$\endgroup\$ – Sparky256 Jul 26 '16 at 1:06
2
\$\begingroup\$

I have the same issue with Altium 14 (14.3.20). The resolution is easy and unintuitive.

Design > Import Changes From [PCB] The dialog is displayed. Click the validate button. The errors are shown. Click the execute button. The errors are cleared. Click the validate button again. The errors remained cleared.

(This scenario is user unfriendly as I expected the validation errors to prevent execute from working.)

\$\endgroup\$
2
\$\begingroup\$

Be aware of pin designators: I had issues with designator "1(C)" which had to be the name, but did accidentally fill in field of designator. Spend lot of time to solve. After renaming those pins to for example "1" I didn't see this errors anymore. I got errors like "unknown pin T1-", while pins that moment has designators like T1-4(C) for example (As you can see, 4(C) wasn't printed in error, which leads me to invalid designator as the reason for this pin-error issue). So: designators should be numbers or letter (0-9, a-z), but not all characters other than that are supported.

To anyone having this issue and came here by google ;)

\$\endgroup\$
1
\$\begingroup\$

I came across this error when creating a part using a custom schematic symbol and footprint. For my situation, I solved the error by changing the schematic symbol type from Mechanical to Standard (No BOM). I believe having a schematic symbol with the type set to Mechanical does not allow the part to link to pins in the PCB layout.

\$\endgroup\$
1
\$\begingroup\$
  1. Delete the component that generated the Unknown Pin from the PCB
  2. Before updating the schematic, right-click on the schematic file and click ‘Compile Document’
  3. Right-click in the Project.PrjPcb and click on the ‘Compile PCB Project’
  4. After these steps, if there is no error, you can update your schematic
  5. If the problem is not resolved, go to ‘Component Links’ from the project menu in PCB and check if all components are in the right window
\$\endgroup\$
0
\$\begingroup\$

This error can also be caused by components like ICs being defined with a "mechanical" rather than "standard" type (typically used for items like stand-offs which you want on the BOM but not in the layout). Access this option by right clicking on the schematic component - in the "properties" section there is a "Type" drop down menu.

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

Here's another way this can go wrong: Beware of trailing spaces! I spent a fair amount of time scratching my head until I realized the footprint pin was called "1 ", not 1.

You'd expect Altium to trim/ignore trailing spaces but it doesn't.

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

It could also be this issue:

For example a resistor.

The resister footprint is not matching with your schematic.

In the schematic, the resistor R1 terminals were named like R1-1 and R1-2.

But, footprint pads name not 1 and 2.

Go to the corresponding library and Edit the footprint pad name.Then it will be Okay!

\$\endgroup\$
-1
\$\begingroup\$

In my case when clicked Validate Changes button "Unknown Pin" error occurred but when clicked Execute Changes button the error is gone.

\$\endgroup\$
-2
\$\begingroup\$

Check if your pad designator name in pcb foot print and pin designator name of the schematic symbol are same. If the are different change it to the same name so you will get rid of the error.

I had the same error I had a diode with designators "a" and "k" on its pads and designators "1" and "2" in its schematic symbol. So I got the error "unknown connection pin 1 to unknown pin".

\$\endgroup\$
  • 3
    \$\begingroup\$ Please change this from all capitals to normal mixed-case. "All capitals" is generally perceived as shouting, and will often mean that you get a negative reaction. So, for your own sake, please follow my suggestion, and not some misguided attempt to make us "see it" (as you said). Thanks :-) (P.S. Your answer seems to be effectively the same as this one.) \$\endgroup\$ – SamGibson Feb 5 '19 at 5:21

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.