Hi,
After adding the 3D model (step files) in the component properties (right click on component in the PCB editor, then “properties/3D Models”), 3D view is generated as expected. However, PCB DRC throws:
Warning: Footprint 'CMI1210595T' does not match copy in library 'CMI'
Footprint LS80
Then, after running in the Schematic Editor “Update PCB from schematics”, PCB DRC does not throw anymore the above warning. But the 3D model disappears from the PCB component properties. And hence the 3D view of this component is not generated.
Did I misunderstand the procedure of setting-up the 3D model ?
Version is 7.07 on a Mac
The latest KiCad versions flags all differences between footprints from the libraries, and footprints which are on the PCB, and adding or modifying a link to a 3D model is a footprint change that gets flagged. It is up to you how yo want to handle this.
For people who use for example database libraries, they send a message or updated footprint to the person who does the library management (this may or may not be another person). For people with a more ad-hoc design workflow, you can either export the new footprint to a project specific library or simply disable the warning itself in the board setup.
Understood, but this is a bit annoying.
In the above mentioned case, the 3D is added to a component lying in a project library, not in the standard library.
As a suggestion, could the 3D model be set-up in the component library itself (in a project library), not at the PCB (footprint) level ?
This would prevent detecting change in the PCB footprint.
The issue is that disabling DRC errors has downside …!
It’s not a DRC error, but a warning, and if you go to PCB Editor / File / Board Setup / Design Rules / Violation Severity you will see that a few are already set to “ignore” by default.
But as long as the footprints on the PCB match with whatever library is the source of those footprints, then KiCad is happy about this and won’t complain.
Why do you find it annoying?
Apparently the footprint is already in a project specific library. Which means that if you added the footprint link to that library footprint and then updated the PCB, all instances of that footprint would have gotten the footprint link in the same update.
Once you get into the habit of keeping the PCB and the library footprints in sync with each other it really is not such a big deal.
Agreed, it is a DRC warning, not a DRC error.
To clarify: I previously set-up the 3D model in the PCB. It was annoying as the component in the PCB was updated according to the library when running “Update PCB from schematic” and then the 3D model was lost.
I found the procedure to set the 3D model in the component library: footprint Editor, “File/Footprint Properties”. Now the component comes with the 3D model. Upon “Update PCB from schematic” the 3D model is not lost any more. Definitely less annoying !
Regarding warning and errors, I believe it is better to solve, not to ignore …
There’s something else going on. If you have used the normal workflow of updating PCB from schematic and don’t change the footprint pointer in the schematic symbol, you won’t loose the changes you have made in the board footprint. This happens only if the fp library pointer is different in the schematic and in the board, i.e. the footprint is changed from one footprint to another.
“Update PCB from Schematic” function can not update footprints at all by reloading them. It can only change to different footprints. That’s very deliberate decision which has been discussed and decided explicitly when designing the dialog and its functionality.
Update Footprint(s) function in the layout editor, on the other hand, reloads footprints from their libraries and has options to keep certain properties even when the footprints are reloaded from the libraries.
Hey folks, been following this thread and just wanted to drop in my two cents. Ran into something similar with KiCAD and 3D models a while back. There’s one forum thread that worked for me: