I'm a big fan of this feature embedded in Altium. However some of the component generators have flaws:

  • Chip resistor and chip capacitor generators making me a wrong component height (despite the "minimum height" setting the resistor appearing too high, and the capacitor is too low)

  • SOD123FL body have no cathode designator

I think that there should be an editable file which I could edit to correct these errors or a setting section. But I did not find any.


2 Answers 2


The STEP model created by the Alitum Wizard is not editable, at least inside Altium. Actually you can't modify any STEP model in Altium.

I suppose you could go around this doing this:

  • Placing the footprint in a PCB
  • Exporting the PCB into a STEP model
  • Modifing the STEP model in a CAD tool such as Solidworks.

It doesn't seem worthy at all.

I would suggest one of the next options:

Failing all this, you can create a basic 3D model in Altium extruding basic shapes.

  • 1
    \$\begingroup\$ +1 I also would suggest the 'next options'. The 3D models created by the wizard are very rudimentary. Be a bit careful with the free models from non-manufacturer sites, they often have small errors and sometimes really big ones (like the wrong index mark position). \$\endgroup\$ Commented Nov 6, 2016 at 17:05
  • \$\begingroup\$ Actually I'm on the path you suggested. I took the 3D bodies from 3d content website. Thank you for providing one more link! \$\endgroup\$ Commented Nov 6, 2016 at 17:27

There isn't an editable file to prevent these errors, but you can easily fix them post footprint creation.

First off, I would make sure you are entering the inputs right. I say this because for chip capacitors/resistors/inductors, it asks for the MAXIMUM height, not the minimum.

enter image description here

enter image description here

These generated a correct looking STEP body for me, but if you'd rather just keep the pads and draw the body yourself, here's what you can do. After generating the footprint, click the step body and delete it.

Then first select the layer that you want to draw it in, usually something like Mechanical13.

Click Place -> 3D Body. Select Extruded, type in an overall height (1mm shown here). You can give a standoff height too if desired, this has no effect on shorts detection / DRC. Click OK.

enter image description here

Draw a rectangle where the part should be. IPC wizard will have left behind a prior shape you can follow (we deleted the 3D body already though). Right click to close the polygon. Hit Esc. Switch to 3D view and see the body as drawn. You can double click it to change the color/capacity/etc. or modify settings that were in the initial dialogue box (like change the height).

enter image description here

For your second issue, regarding the SOD123FL footprint, this one is even easier. After generating the footprint, just draw your own cathode designator using the silkscreen layer and the Place -> Line command.

Again, I tried this with the IPC Wizard just now and it created a cathode designator, so maybe your tool is a bit out of date.


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.