4
\$\begingroup\$

I want to make a footprint for a mini USB connector. Here's the recommended layout from the datasheet:

enter image description here

I'm not very experienced with making footprints and find the dimensions inconvenient since they are all relative and not with respect to an origin.

My current plan is to choose the center of pin 1 as the origin and then work out the coordinates of the center of every pad using a pen and paper. This isn't going to be very efficient, though, and I'm wondering if there's a better way.

What would you use as your origin? What would your approach or process be when tackling a footprint like this?

\$\endgroup\$
9
  • 1
    \$\begingroup\$ I'd probably do exactly what you said you'd do. Use the center-left hole as an origin, place the bottom-left and top-left GND pads, then place the top-left pin-pad, then you can use relative measurements/symmetry from there to do the rest pretty quickly. This is one of those cases where overthinking the process is more time consuming than just doing the task at hand, IMO. \$\endgroup\$
    – Shamtam
    Jan 26, 2015 at 16:24
  • 3
    \$\begingroup\$ See Designing Pick-and-Place-friendly CAD library parts \$\endgroup\$
    – Tut
    Jan 26, 2015 at 16:26
  • 1
    \$\begingroup\$ I would do it in your pad layout program and not on a piece of paper, just so you don't have to do the same thing twice. Besides that I'm not sure there is a better way. Shouldn't take more than a couple minutes though. \$\endgroup\$
    – I. Wolfe
    Jan 26, 2015 at 16:26
  • \$\begingroup\$ @Shamtam I see dimensions relating the mounting holes to the GND pads, but none relating either of those to the signal pads. How do you deal with that? \$\endgroup\$
    – Nate
    Jan 26, 2015 at 16:34
  • 2
    \$\begingroup\$ The degree of terrible expressed by the datasheet drawings carries a pretty heavy weighting in my decision to use a given connector. \$\endgroup\$
    – Matt Young
    Jan 26, 2015 at 16:43

5 Answers 5

4
\$\begingroup\$

In my PCB CAD package I am free to select the origin anyplace I want. When I am in the midst of creating a footprint I will place some pads and then move the origin around as suits the task at hand and according to the drawing. When the thing is completed I then place the final origin at a place that makes the most sense for the part centroid.

\$\endgroup\$
2
  • \$\begingroup\$ Great idea, thanks for sharing. If I could ask a quick follow-up question, what does "bottom view" mean as indicated in the recommended layout? I'm not sure if it means the bottom of the PCB, or the bottom of the component. When I see a footprint I typically view it as how it would look when on the top of the board, but the "bottom view" text is confusing to me.. \$\endgroup\$
    – Nate
    Jan 26, 2015 at 19:49
  • 1
    \$\begingroup\$ @Nate: It's the opposite side of the board from the component. Just about useless for surface-mount, but remember that through-hole components exist also. \$\endgroup\$
    – Ben Voigt
    Jan 26, 2015 at 20:33
6
\$\begingroup\$

In the general case, you want the origin to be at the centroid of the part. That makes the placement coordinate used in manufacturing and the part origin the same thing (usually).

However, in this case, I'd pick the origin more for benefit when placing the part outline on the board during board design. This kind of part needs to placed relative to the board edge, so I'd put the Y of the origin (using the orientation in your drawing) at wherever the edge of the board is supposed to be relative to the part. I'd then center the X of the origin.

Yes you can move a part around so that it is lined up properly with the board edge regardless of where its origin is, but that's not so easy. Most CAD packages will snap coordinates to some grid, which may have to be disabled if the offset from the board edge to the origin is not a nice multiple of a reasonable grid resolution. Also, you'd still be left eyeballing the placement. With the origin at the board edge and centered around the part in the other dimension, it's much easier to type in the placement coordinate and put the connector exactly where it's supposed to be.

Another thing I'd do is add some silksrcreen or at least something in a documentation layer that indicates the board edge. Don't assume you'll remember the details of this particular connector when you lay out the board, or lay out a different board a year later.

For example, here is a connector where I've done as described above:

The dashed line indicates where the board edge should be. This connector actually hooks around the edge of the board a bit for better mechanical strength. The blue rectangles are in the bottom keepout layer to indicate nothing should be placed there because the connector is taking that space.

The text "Board edge" is in the top documentation layer, and is only for use in placement. It indicates the meaning of the dashed line, which is easily forgotten months later after the connector package was created, or for other people that never knew this in the first place.

Note also the arrow indicating the direction the mating connector will be plugged in. This may seem obvious given the pads at the opposite end of the connector and the board edge, but it can be confusing on some connectors. I generally add this when the mating connector comes in sideways. Long ago I once placed a RS-232 connector the wrong way because the placement of the pads alone gave the opposite impression of which way the mating connector came in. Since then I've added arrow to sideways-mating connectors and haven't made that mistake again.

The origin of this connector is at the board edge in the middle, right where the arrow crosses the dashed line.

\$\endgroup\$
1
\$\begingroup\$

My approach is

A) Pick a reference point B) Do all of my calculations either in Excel, Matlab, or Octave, where I have some ability to check, recheck, and easily recalculate. C) If I'm really feeling fancy, I have Octave output scripted code for whatever layout package I'm using, and then run the script in the package D) Check, recheck and triple check, and repeat A-C as needed.

For USB connectors in particular, I've had some sales documents on the family of connectors show amazingly detailed land patterns, only to have them not match the actual datasheet, so beware!

\$\endgroup\$
0
\$\begingroup\$

It seems all Y dimensions are given in relation to the lower horizontal line in your drawing so this could be your zero for Y. For zero X I'd take a centerline of pin 3 (alignment holes would stand 4.45 mm from it).

On a side note: using mini USB connectors in new designs is a bad idea.

\$\endgroup\$
2
  • \$\begingroup\$ Why are mini USB connectors a bad idea? \$\endgroup\$
    – Nate
    Jan 26, 2015 at 17:19
  • \$\begingroup\$ I'm quite familiar with those. It's a weak connector, mechanically. SMT-only mounting is weak too, a customer will break it off the board rather quickly, if you don't support the connector externally. If you can, switch to micro USB, and choose one where you can have mounting holes to solder it to. \$\endgroup\$ Jan 26, 2015 at 17:24
0
\$\begingroup\$

I normally keep changing my origin. I find its a lot quicker than trying to work out what the absolute dimensions are. It also helps if the software you use has a relative move command.

\$\endgroup\$

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.