Altium: custom pads issue when exported to Gerber

Hi all,

A few days ago I have created a custom pad shape in Altium to be used at the end of a FPC (ZIF connector). All went apparently well and I was able to draw the desired circuit, however when exporting the circuit to Gerber and using gerbv to view the file I noted something strange: within each pad there is a thin "island" which is not covered by cooper.

Attached a print screen from gerbv vs. the original as shown by Altium:
Gerber file opened with Grbv
original design in Altium

I have no clue why this is the case, hence looking for help.

Some more info:
- I have created the pads by drawing first the outlines and then converting to regions; I'm pretty sure that this is where the trick lies as prior to the current shape I had a slightly different version, drawn using different tolerances / dimensions (mm vs mil in latter) and the Gerber export had been even worse (some pads did not show up at all)
- The pads are tiny (e.g. the thinnest portion and the spacing measure just 4 mils)
- I have prepared the Gerber files using a tried and tested method (true, never with circuits including custom pad shapes and never with traces smaller than 8 mil)
- I tried some other Gerber viewers and the result is the same.

Thanks in advance.

Try making solid region directly rather than converting lines to region.

Thanks Ricky. I gave it a try (created one of the pads directly as solid region and replaced it in the the custom shape) but there's no difference. So it does not seem to be a "convert line to solid region" issue.

I'm wondering if someone has a clue about what would cause the error / seen this before. Could it be just a glitch in how AD works (I would not be surprised given that the custom pads creation feature is rather new)?

- - - Updated - - -

One more thing, looking closer at the gerber file I noted one other anomaly with one of the pad shapes (pads 3, 5, 7, 9, 11) - this can be seen in the picture attached in my first post. Basically the passage from the narrow portion in the middle to the thicker one on the right hand side is not smooth/progressive but shows some kind of dents. Again, this does not appear in the original shape as seen from within AD but only once the gerber (and CAMtastic) files are generated.

Hi,

Remove solder mask expansion for the region.

anilrock87 said:

Hi,

Remove solder mask expansion for the region.

Click to expand...

That's how I created the shapes in the first place, no solder and no paste masks expansion. Those are manged on different layers in any case, whereas the issue I have encountered concerns only the top (copper) layer... Thanks for the suggestion anyway.

I've spent some quality time with this and I think I found the cause.

When exporting to gerber, the solid regions are converted by default to shapes composed of line strokes which cannot be arbitrarily small/thin (pcb fab house limitation). As a result, the exported shapes are only an approximation of the originals. The smaller the original polygons/sharper the angles, the less accurate the approximation. This is why I've never noticed such an issue before - this is the first time I'm working with such small shapes.

This conversion can be eliminated (by unchecking the "Convert polygons to Vector Fill (Line Strokes)" option during the export, thus keeping the original shapes untouched. I'm not sure that the fab houses would be able to accommodate this however, but this is something I'll find out soon.