Circuit Studio STEP export still fails to output PCB

Hi,

Is it possible to share the PCB file?  It may help to reduce the design to something as simple as possible the exhibits the problem first though.  If possible, just the outline would be best to see if this is purely related to shape.  This would help reduce size of the file and also to isolate the cause.

I have not had problems on PCBs with curved edges but I have only done a few so far as they are not all that common for me.

Also, there is a beta test of the new CS going on so if the problem can be reproduced it would be a good check for the new beta software version.

Hi,

Thanks for the reply.

When I get to the office tomorrow I'll pare it down to the bare minimum and attach it.

Hi,

For what it is worth, I made a simple PCB using two arcs and two straight lines on an outline layer and then set the board shape.  I added four holes and a couple of 0603 footprints and a couple of tracks.  The step file it generates is something like you got.  An export as a 3D PDF format looks correct.

In CS, on the left is the PCB in 3D view mode and on the right side is the step file that was exported and then placed as a 3D body.

Pretty underwhelming.

I tried to modify the PCB by getting rid of one of the two straight sections and completing the arcs instead.  It would then have only one straight edge and the rest is a circle.  The board shape is 100mm diameter with a straight line edge from angle 170 to 190 degrees.  That is, outline is made of two arcs; 0 to 170 and 190 to 360 with a straight line connecting these.  This cause CS to crash when generating a step model.  It even crashes with an exception even after restarting.

For what it is worth I have attached my zip file of this simple project.  I also posted this into the Altium forum for the beta testing of the next version of CS.  The beta version seemed to generate a proper step file so that is good news.

By the way, if the PCB is a full circle then it generated the step file in CS 1.5.2 correctly.

This isn't exactly intuitive but I think it might work for you if you make the outline arcs slightly longer than the straight sections.  I did this on the top part of the arc and here is what I get. A message box saying cannot find the outline.  I clicked Yes so it would generate the shape anyway.

And the result is this. If I zoom in I can see that the straight edges have "features" due to outline thickness. So, if you try this, make sure your outline primitives are thin (perhaps 0.1mm) so there is little difference between it and the center of the primitive.

So, to solve this for me, I made the top arc which used to go from 10 deg to 170 degree instead be 9 degree to 171 degree.  Bottom arc was given a similar slight overlap.  You could play with the overlap slightly.  Maybe even a fraction of a degree would work.  I'm betting the vertices of the board shape are at fault for the step renderer and there is probably some precision error or something.

Looks like a bug to me for sure.

Good luck.

Thanks for the work-around Thomas.

I just did the same as you - making a new PCB with 2 arcs and 2 straight sections - and got this;

It seems a shame that Altium can't sort this out. The issue is that if I elongate the arcs to make the STEP export work the client will get PCBs with little "horns" at the edges of the boards so it mens that the arcs have to be extended to export the STEP file then reset to output the fabrication data.

I might have a play with this later during an idle moment...

I also attached me very basic project that shows the bug.

Thanks for the work-around Thomas.

I just did the same as you - making a new PCB with 2 arcs and 2 straight sections - and got this;

It seems a shame that Altium can't sort this out. The issue is that if I elongate the arcs to make the STEP export work the client will get PCBs with little "horns" at the edges of the boards so it mens that the arcs have to be extended to export the STEP file then reset to output the fabrication data.

I might have a play with this later during an idle moment...

I also attached me very basic project that shows the bug.

Hi,

I found my curiosity getting the better of me and I had to test, I made the arcs go beyond the intersection by 1/1000th of a degree; thus the upper arc went from 9.999deg to 170.001 degree.  The step file seemed to generate correctly then.  If the outline had such a small amount of overage and the outline line thickness is very thin (e.g. 0.1mm) then the PCB should be quite smooth and within the typical tolerance of manufacturing.  So, yes, this is a workaround but should get the job done.

As I mentioned above, this issue does seem to be fixed in the (hopefully) soon to be released version update for CircuitStudio.  And I took the opportunity to notify beta testing of this issue as well.  Also, I saw that the 3D PDF rendering appeared to be correct.  It would be very disturbing if the Gerber or ODB++ board shape is wrong.  I did not attempt to test that to confirm the expected result.

You mileage may vary; as they say.

Thanks for that Thomas.

I look forward to trying the new version, when it's finally ready!