Test point not visible in STEP file

[ajaybhargav]

Hi Everyone,

I am exporting 3D file of my PCB in STEP format. All components are ok but test points on my PCB are not visible in 3D. If i export in WRL format, everything shows up perfectly, even the silk screen.

How can I get at least test points to be visible in STEP file? Please help.

Thanks!

[RaptorUK]

In V7 tracks (& pads) and Silkscreen are not exported as part of the STEP file. So you have a few possibilities:

• Add a hole to your test point, holes are exported . . .
• Use V8 RC, it will export tracks and pads (CAUTION ! ! you cannot open a V8 project in V7)
• Use StepUp (with FreeCAD) to get your PCB + Tracks + Silkscreen into FreeCAD and then export a STEP file.
• Create a thin disk (0.05mm), same size as your test point, in 3D CAD and add it to your test point footprint as a 3D CAD object. It will be exported as part of the STEP

[ajaybhargav]

Hi @RaptorUK

Thank you for helping. I think V8 RC is easiest option for me (comes with a CAUTION).

I am trying to use StepUp but i am not familiar with FreeCAD software. Though I feel I have configured most of the things correctly and all components are now showing up in FreeCAD. however when I import PCB in FreeCAD, i still do not see tracks.

And I dont know how to fix this warning:

[RaptorUK]

@ajaybhargav

Though I feel I have configured most of the things correctly and all components are now showing up in FreeCAD. however when I import PCB in FreeCAD, i still do not see tracks

I haven’t used StepUp and FreeCAD for a few years, back then the tracks had to be exported as a DXF and pulled into FreeCAD separately . . . not sure if it’s the same/different these days.

There are other Users here that can help you with StepUP and FreCAD better than I can . . .

[ajaybhargav]

There is option to import DXF geometry, I am able to import it and I can see the tracks now. They do not look good and my worry is, that warning about grid origin, i am not sure if output will be correct.

I am downloading Kicad V8. Lets try that as well.

Thank you so much for helping.

[maui]

just read kSU cheatsheet
There is a button to load tracks directly from kicad_pcb file in FC

[ajaybhargav]

Hi @maui
Yes i have gone through the cheat sheet, but imported PCB does not look good somehow.
And

@ajaybhargav

And I dont know how to fix this warning:

So I gave a try to V8-RC2, the output is still the same. No tracks or footprints on PCB in STEP file.

EDIT:

somehow top pads after importing looks like this:

[dsa-t]

@ajaybhargav

So I gave a try to V8-RC2, the output is still the same. No tracks or footprints on PCB in STEP file.

Have you checked this for tracks and zones?

[ajaybhargav]

@dsa-t

Have you checked this for tracks and zones?

I missed that, it worked thank you. I think this should do the job.

Out of scope, but there are lot of DRC errors in V8 about footprint mismatch:

maybe I will post it in layout forum?

[paulvdh]

KiCad quite easily throws the "Warning: Footprint ‘XXX’ does not match copy in library ‘YYY’ " warning, and quite often it is for very trivial changes. I guess that in quite a lot of instances (but not always) suppressing this warning is a good option, especially if the footprints used are footprints from KiCad’s default libraries.

However, if you want to get rid of the warnings without modifying the DRC settings then:

1. PCB Editor / File / Export / Footprints to (new) Library** (And accept it when KiCad suggests to link the existing footprints to the newly created library.
2. PCB Editor / Tools / Update Schematic from PCB, and make sure that the Update / Footprint assignments option is turned on. The schematic is the main source of footprint links, so this is an important step to keep everything synchronized.

The steps above do all footprints on the PCB. You can also do this for just a single footprint with an extra step (or two). If a footprint is already in a writable (project specific?) library, then first modifying the library footprint, and then updating the PCB is also a viable option.

[ajaybhargav]

hi @paulvdh
I am using mix footprints, most from default and some from custom library. its only resistor and capacitor throwing this error. I know i can disable it, but i choose not to do so just in case.

ok, I am not sure if this is 8.0 bug, I tried to update footprint by right click on part (R50) and then update footprint from library. The error goes away, then I select another part (R58), did the same thing and error is still there. turned out that R58 is marked DNP and exclude from BoM. so update symbol is not taking effect. Am I missing anything here? This did not happen with v7 I am sure.

Every time I click update, I get “OK”

It should say “(no changes)” instead.

[paulvdh]

@ajaybhargav

It should say “(no changes)” instead.

Why?

DNP and “exclude from BOM” are fabrication attributes, and if you do not select those in the Update Options then those do not get updated, and as a result there is still a difference between the library footprint and the footprint on the PCB.

But maybe you are right. You can make an argument for these fabrication attributes to be a part of the schematic symbol and not of the footprint at all and it may be preferable if this warning was a bit less trigger happy.

[ajaybhargav]

PCB artwork should not be mixed with fabrication attributes i believe. but I may be wrong.

This is for my understanding, so by this means even if I make footprint changes in schematic to a DNP component, will it not reflect in PCB?

[paulvdh]

@ajaybhargav

PCB artwork should not be mixed with fabrication attributes i believe.

I think I agree here, but I do not use this feature myself, and thus don’t have a good opinion about it.

@ajaybhargav

so by this means even if I make footprint changes in schematic to a DNP component, will it not reflect in PCB?

KiCad has no automatic synchronization between schematic and PCB. Normally the BOM is generated from the schematic (Schematic Editor / Tools / Generate BOM), and that strengthens the idea that the fabrication attributes do not have much in common with footprints. But KiCad also has: PCB Editor / File / Fabrication Outputs / BOM. Apparently this only generates a CSV file. I’m not sure whether this is an intended feature, or a historical leftover that could be cleaned up. The Fabrication Outputs can also generate a placement file, and this also needs the fabrication attributes.

[ajaybhargav]

@ajaybhargav

This is for my understanding, so by this means even if I make footprint changes in schematic to a DNP component, will it not reflect in PCB?

I think my question created confusion. with this, i was mentioning update PCB button which i use very often when I make changes to component attributes. I always do changes in schematic and sync with PCB.

so with DNP component, a footprint change in schematic will reflect in PCB or not was my question. so I tested it and it does reflect if I change footprint of a DNP component.