0
\$\begingroup\$

I have a pcb design which has two layers with two star ground polygon pours respectively, and all the components are throughhole. When I generate gerber files however, on both layers the border of the component connects to the trace and the polygon pour. I am confused. Why is altium considering the component borders to be part of the polygon pour?enter image description here

enter image description here

\$\endgroup\$
3
  • \$\begingroup\$ On which layer are your component borders drawn? \$\endgroup\$
    – brhans
    Nov 3 '20 at 19:11
  • \$\begingroup\$ I do not know. I cannot select the component footprint border outlines. However I can select the components themselves in both top and bottom layers, as well as the mechanical layers. \$\endgroup\$
    – A.boj
    Nov 3 '20 at 19:17
  • 1
    \$\begingroup\$ It appears you are adding some documentation layer to "print on all layers" option for output generation . \$\endgroup\$
    – crasic
    Nov 3 '20 at 19:20
4
\$\begingroup\$

Check your Gerber output configuration and make sure that none of the shown boxes are checked:

enter image description here

If you check any of those boxes that particular mechanical layer will be merged with each of the other layers, something you seldom want.

\$\endgroup\$
4
  • \$\begingroup\$ I believe the intent is to put frame, notes, and doc rev info on every layer which is subsequently cropped out by fab, problem here is whatever it may be is encroaching on the main copper area , while this may fix the output, I think @Parker may be on to something with respect to how the part library is designed . But ultimately every org/designer needs to decide for itself the layer standard and which, if any, mechanical layers are included on output files. \$\endgroup\$
    – crasic
    Nov 3 '20 at 20:00
  • 2
    \$\begingroup\$ The issue with "mechanical" layers is that there doesn't seem to be any standard as to which layer should be used for what, so a library designer may use a layer to indicate component outline, while a board designer may choose to use the same mechanical layer to indicate global information that should be plotted on every layer. \$\endgroup\$ Nov 3 '20 at 20:05
  • 1
    \$\begingroup\$ The borders disappeared after unchecking. Thank you. \$\endgroup\$
    – A.boj
    Nov 3 '20 at 20:16
  • \$\begingroup\$ @PeterGreen this is very true, however the result is every organization is responsible for its own library and layout standards, much like a code style requirement for the software folks. \$\endgroup\$
    – crasic
    Nov 5 '20 at 15:17
0
\$\begingroup\$

Open up the footprint associated with the parts in question.

This will allow you to click on the outline of the part. I believe that the part footprint was made incorrectly and that the outline was drawn on a physical layer.

First, select all the lines/polygons that should be on top/bottom overlay layer instead of the physical layers.

Next, change their layer to the top/bottom overlay layer.

Finally, save changes and update your pcb. Tools->update from pcb library

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.