[Solved] Mouser / Ultra libarian Footprint pad polygon problem

[Kipton_Moravec]

Mouser has EDA help for many of the parts it sells.

I am using a TI LM61480Q5RPHRQU. Attached is the Zip file they sent me.

It has a subdirectory for Kicad.

The Symbol works without a problem. The issue is with the footprint.

There are 4 unusually shaped pads that are recognized, but I can not attach a trace to them.

They are pads 1, 6, 10, and 15. When I try to run a trace to any of those pads, the PCB Editor will stop me before I can touch them with my trace.

Has anyone seen this before? Do you know a workaround?

Any help would be appreciated.

Thanks,
Kip

[Kipton_Moravec]

I thought it would let me attach a file. But it posted. Here is the file.

ul_LM61480QRPHRQ1.zip (119.1 KB)

[paulvdh]

The reason is a fault in the ultralibrarian data. It has the copper, but not the definitions. To fix it:

1. Load the footprint in the Footprint Editor.
2. Select a pad (I choose number 1). You can see that the pad itself is quite small:
   
   
3. Press: [Ctrl + e] to Edit pad as Graphic Shape (or select that from the RMB popup menu).
4. Select the polygon around the pad, press [Ctrl+e] again to exit this pad edit mode.
5. The whole polygon has now been added to the pad. You can see this from the much bigger pin number.
   
   
6. Repeat it for the other offending pads.
7. Save the footprint, update library, usual library management, bla bla bla.

[Kipton_Moravec]

@Kipton_Moravec

LM61480Q5RPHRQU

Thank you for the very clear explanation. It worked! It is fixed! Yea!!!

Kip