I have a really annoying situation here where Allegro cannot load a footprint after importing a netlist. The error is : ERROR(SPMHNI-196): Symbol 'TO254P1524X483-4_3N' for device 'DIODE_D2PAK_2L...' has extra pin '1'.
The footprint has 3 pins : 1, 3, 4The part has 3 pins : 1 (zero length, pin ignore), 3, 4.
The footpint :
The part :
I tried to remove the "pin ignore" property from pin 1, but then it displays a square on the schematic where the pin is. There is a "pin visible" option but it is only available to power pins...
Why is allegro telling me that the footprint has extra pin 1 when it doesn't ? What should I do in order for the netlist to be imported correctly ?
EDIT : when trying to quickplace, here is the error given for that same problem :
Cannot place symbol: CR153000 / DIODE_D2PAK_2L... / TO254P1524X483-4_3N due to ERROR(SPMHGE-82): Pin numbers do not match between symbol and component. Run dev_check on device file for more information.
I tried running this command on the BRD file, on the DRA file of the symbol with the problem, I tried running it on Capture. The command isn't recognized by any of these.
There is a much better way to handle this. Delete the pin 1 from the schematic symbol and add a new property called NC with a value of the pins you want as not connected. In this example 1 but for future reference this can be a comma seperated list of all the pins you don't want to show on the schematic symbol but they do exist in the PCB Footprint.
Thank you so much Steve ! It worked perfectly.
I didn't knew it could be done like this, I'll do that from now on.