Kicad 8.0.1 odd behaviour of 3D view

[shoka]

Hi

I suspect this is a bug, but Gitlab will not play ball at the moment.

I gave created a footprint, for a 5 pin Molex connector, not using the one in the standard library because this one has little “spurs” that mount it to the board, so needs edge cuts detail.

As is normal for me I have created the pads with an asymmetric extension on the B side to make them easier to solder.

That was something of a drama initially, but I’ve now found my way around the pad editor, and remembered the trick of overlaying two pads with the same pad numbers, with a SMD pad on the b side. I’m now very happy with my new footprint.

However the 3D view of the footprint is odd. The a and b sides are revered, with the the extended pads on the top surface, along with the front side silk screen, and the 3d Model, and the standard pads on the reverse side.

The non 3D view of the footprint is normal, and gerbers are as I would expect with the extended pads correctly on the b side.

I suspect a bug in the 3D viewer. In most cases the confusion of the swap of the a and b side copper details would not be very noticeable as for most footprints the a and b side copper is the same.

I have built a simple test board with just the footprint, and an edge cuts outline that shows the issue pretty clearly. I can post it here, though I’m not sure the 3D model of the connector will transfer with the board archive.

File:
K8_testing-2024-04-15_140109.zip (6.1 KB)

Harry

ps I checked the downloaded file, and it contains all the info, including the 3D model

[mf_ibfeew]

No bug, you have just forgot to change some settings for your bottom pads. For all smd pads on the bottom side you also have to move the Paste + mask layer from top–>bottom. See picture below.

This mistake happens if you use the F.Cu/B.Cu pulldown menu in the pad properties dialog. Instead use the “Flip” command (standard hotkey: “F”), which automatically flips not only the copper layers but also all other top/bottom layers (mask, solder, …).

Regarding the 3D model: this is not preserved in your archive. The 3D model path still points to your kicad installation and your user libraries: /home/harrym/ShokaShared/Northfrost_catalogue/3D_models/Molex_5pin.wrl

edit: added the picture:

edit2: The FP editor allows a rough check of your footprint design. Running FP-editor–>Inspect–>Footprint checker will show you a warning regarding these pads.

[shoka]

Thank you, you are correct, no bug. Still slightly puzzled why the back side copper did not show on the 3D view with the misplaced mask and paste layers, but correcting the errors in the mask and paste layers fixes the issue.

I downloaded the file I uploaded and opened the board, and had a 3D model, so assumed it was preserved. Outwitted by Kicad again.

That footprint was not really complete, the purple cast on the backside copper pads was nagging at me, I knew it was a problem. I remembered seeing the odd colour pad issue way way back at least several releases of Kicad, but could not call the actual issue to mind. I traced it then when I checked the gerbers before sending a board for manufacture. As soon as I saw your note, I remembered the whole issue. Thanks a lot. I think I’d have found it the same way as I found it before, but you may have saved me a batch of useless boards.