2
\$\begingroup\$

I made a manual footprint for a USB micro-B receptacle that is now giving me problems on my PCB in Altium Designer 16.

Here's the footprint drawing that I was going off of: USB Footprint Drawing

And here's what my footprint looks like: USB Footprint

I'm now getting a bunch of clearance constraints.

USB Footprint Clearance Constraint

I tried editing the Manufacturing constraints in the Rules to set the minimum clearance to 0.1mm instead of 0.254mm but that doesn't seem to work.

EDIT: What is the point of the rectangular pad in the middle? I ask because if I can get rid of it then maybe I can route underneath it and resolve some of my clearance constraints.

\$\endgroup\$
8
  • \$\begingroup\$ Did you re-run the DRC? \$\endgroup\$ Commented Jan 17, 2019 at 23:37
  • \$\begingroup\$ Yes, I did re-run the DRC and also reset the error markings. \$\endgroup\$
    – YNGVV
    Commented Jan 17, 2019 at 23:53
  • \$\begingroup\$ The rectangular 'pad' in the middle is not a pad, it's a keepout. You still can't run tracks under it though. \$\endgroup\$
    – brhans
    Commented Jan 18, 2019 at 0:16
  • \$\begingroup\$ What are your pad dimensions? I see they specified the solder mask opening should be 0.4 mm in the y-direction, but I don't see where they specify the pad dimension. \$\endgroup\$
    – The Photon
    Commented Jan 18, 2019 at 0:28
  • \$\begingroup\$ If you specify the pad y-size as 0.25 (equal to the pin width) and solder mask expansion 0.075, you'll get the 0.4 called out. Then you should have about 0.25 mm solder mask slivers between the pads, not the something-less-than-0.1-mm that it looks like you have now. \$\endgroup\$
    – The Photon
    Commented Jan 18, 2019 at 0:31

1 Answer 1

1
\$\begingroup\$

From the notes on the footprint definition the cross hatched areas are the solder pads, not the solder mask area. The white rectangles over the five signal pads are the actual connector pin fingers and you would find their dimensions on the connector drawing.

According to what I see the signal pads are all 0.4mm wide and 1.2mm length. Center to center spacing between these pads is 2.6mm/4 = 0.65mm. This leaves a total of 0.25mm between each pad. This is equivalent to a 10mil clearance if you think in typical USA type units. You need to set your pad to pad clearance rule to 10mils (0.25mm) or less.

\$\endgroup\$
2
  • \$\begingroup\$ OP's image shows violations with a clearance setting of 0.254 mm, which is exactly 10 mil. \$\endgroup\$
    – The Photon
    Commented Jan 18, 2019 at 5:40
  • 1
    \$\begingroup\$ Even though Altium may be displaying 0.254, the calculation may be something like 0.2539. Set the clearance to 9.9mil or 0.25mm and see if the error still exists. It probably will go away. \$\endgroup\$ Commented Jun 17, 2020 at 4:20

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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