I have recently started learning Altium designer. I created a simple schematic with a few components. I created the schematic symbols and also the PCB footprints.

In the diode component that I added into the library, the schematic symbol used pin designators 1 and 2 while the PCB footprint symbol used designators A and K. The A and K designators were put into the symbol by the footprint wizard that I used. This mismatch was not detected when I carried out the "Validate PCB project ... " command.

When I started the PCB layout I kept getting what seemed to be cryptic error message saying some pins were "unknown" The diode component was not showing any rats nest wires as well in the PCB layout window too.

I eventually found that the problem was the pin designator (not the pin name) was not matched between the schematic symbol and the PCB footprint for the diode component. Now my question is, is there a way to automatically detect this type of mistake in the future?


1 Answer 1


Once you perform a "Design -> Update PCB" you should get an error message stating that some pin doesn't match.

Error message

I'll elaborate a bit on that. Validate Design does only check for schematic issues. It was previously named "Compile" because it performs a compilation over all schematic sheets, thereby checking interconnects and other ERC related issues.

There are three things you ALWAYS want to have 0 errors once a design is near completion (or even before):

  • In the schematic: Compile/Validate design: The messages window MUST NOT show any errors or even warnings. This basically checks your design against the ERC rules specified in Project Options. A good practice is to not allow single pin nets and not allow any unconnected pins (you'll need to explicitly place No-ERCs on unconnected pins).
  • The transfer from schematic to PCB MUST NOT show any errors. This checks the schematic data against the PCB data
  • The DRC in the PCB MUST NOT show any DRC errors. This checks the PCB against the rules you set in the constraints dialog.
  • \$\begingroup\$ By default where does person get rules to be used in the schematic side and the PCB side? Do PCB manufacturers by default provide files that can be loaded into Altium Designer to describe the rules? I am asking this in comment since it is related to the information in the answer. \$\endgroup\$
    – quantum231
    Commented Mar 14, 2022 at 21:18
  • \$\begingroup\$ @quantum231 You must define the rules, especially in the PCB portion. The rules may have limitations of the PCB house for a particular complexity (say, 5 mil spacing, 5 mil min track width {in inches}), voltage spacing requirements for some nets, impedance requirements, ... Or, you may require a fine pitch board going down to 3-3 rules with micro vias which will have a premium cost. \$\endgroup\$
    – qrk
    Commented Mar 14, 2022 at 23:37

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.