Polygonal pads....

Making your own components and patterns, organizing and using libraries.
Post Reply
Message
Author
luisr
Posts: 13
Joined: 12 Mar 2013, 19:24

Polygonal pads....

#1 Post by luisr » 09 Apr 2013, 14:19

How is the best way to create this footprint http://www.st.com/web/en/resource/techn ... 039389.pdf

I've tried two ways (polygonal pads or normal pads + rectangle in signal) but got some issues with both, one throws DRC errors and the other the trace won't snap where it should.

I added the library and image to illustrate the issues, please see the comments on every file

Regards

EDIT:seens like using polygonal pads is the way to go in order to avoid having to add soldermask manually... I just can't the trace to align properly :?


EDIT2: I just figured out that, in some cases, the trace snaps to the first point of the polygon... so, playing with the position of the first point I can make the trace to snap were I want, but for other pads this doesn't work an the trace snaps to the center of the pad's bounding box. Worth mentioning that it works for the pads that are located to the left of th pattern. Also here's a drawback: Diptrace stops reducing the trace width automatically for pads that are defined this way.

EDIT 3: Diptrace can't be tricked by putting the first point inside the polygon, doing that will cause errors in the solder mask generation. See the attached image (Top Mask.png)


It would be nice to be able to add aditional snap points to polygonal pads... may be in the future ;)
You do not have the required permissions to view the files attached to this post.

Alex
Technical Support
Posts: 3241
Joined: 14 Jun 2010, 06:43

Re: Polygonal pads....

#2 Post by Alex » 10 Apr 2013, 09:14

You can create a polygonal pad by points in the way where zero point X0.0 Y 0.0 will be within the pad. In PCB Layout, a trace will be connected to this point.

luisr
Posts: 13
Joined: 12 Mar 2013, 19:24

Re: Polygonal pads....

#3 Post by luisr » 10 Apr 2013, 09:50

Alex wrote:You can create a polygonal pad by points in the way where zero point X0.0 Y 0.0 will be within the pad. In PCB Layout, a trace will be connected to this point.
Thanks for answering...
Unfortunately sometimes is not desirable set the first point at the center of the polygon, as you can see in the attached image.

I'm also attaching another lib, in this one all the polygonal pads have its first point set at the edge, just in the middle of the longest side; For some reason this method is working for the pads that are on the left (1 and 8) but not working for the pads on the right (4 and 5).

Hope you can give me some light on this

Kind Regards

-- 10 Apr 2013, 21:30 --

Another finding... this has nothing to do with pad's position but pad's rotation instead... just to clarify:

On the lattest attached library rotate pads 1 and 8 (the ones that are working fine) 180°, then try to create a trace from those pads... voila! the firts point of the polygon is no longer the snap point (seens like it falls back to 0;0 coordinate).... rotate the pads to their original position and the problem disappear.

the same its true for pads 4 and 5 (the ones that aren't working), if you rotate them 180° and trace to create a tracción from any of them you'll find that the trace will snap at the edge of the longest part of the pad as expected.

even further, seens like the problem arise when the X value of the first point becomes negative... in that case the snap point falls back to (0;0)

Kind Regards
You do not have the required permissions to view the files attached to this post.

Alex
Technical Support
Posts: 3241
Joined: 14 Jun 2010, 06:43

Re: Polygonal pads....

#4 Post by Alex » 11 Apr 2013, 09:16

DipTrace doesn't allow to define evidently a point where pad will be connected with traces. This point is calculated automatically. First, DipTrace calculates a circumscribed rectangle and finds middle point of the rectangle. If the point is within pad's polygon then traces will be connected to this point. If the point is outside pad's polygon then traces will be connected to one of polygon points. It is not true that this will be the first polygon point, I can't see it in codes.

You can do in different way. Create two overlapping rectangular pads instead one polygonal. In Component editor, you can link one pin to two pads when you attach the pattern to a component. Then there shouldn't be any DRC errors in PCB Layout.

luisr
Posts: 13
Joined: 12 Mar 2013, 19:24

Re: Polygonal pads....

#5 Post by luisr » 11 Apr 2013, 10:21

Alex wrote:DipTrace doesn't allow to define evidently a point where pad will be connected with traces. This point is calculated automatically. First, DipTrace calculates a circumscribed rectangle and finds middle point of the rectangle. If the point is within pad's polygon then traces will be connected to this point. If the point is outside pad's polygon then traces will be connected to one of polygon points. It is not true that this will be the first polygon point, I can't see it in codes.
Sorry, you're right... is not always the first point :roll:, I did some test with other polygonal shapes and wasn't able to make the trace snap to the first point... but is very interesting how diptrace behave with this specific L shape pad.
Alex wrote:You can do in different way. Create two overlapping rectangular pads instead one polygonal. In Component editor, you can link one pin to two pads when you attach the pattern to a component. Then there shouldn't be any DRC errors in PCB Layout.
Yep,... that gets the job done 8-)
Many Thanks

woz
Posts: 1
Joined: 20 Jan 2019, 01:29

Re: Polygonal pads....

#6 Post by woz » 25 Jan 2019, 16:21

Alex wrote:You can do in different way. Create two overlapping rectangular pads instead one polygonal. In Component editor, you can link one pin to two pads when you attach the pattern to a component. Then there shouldn't be any DRC errors in PCB Layout.
Sorry to dig up this thread :roll: I am having similar issues with pad origin in polygons .... how do you "link one pin to two pads when you attach the pattern to a component".

Thanks!

Serg
Technical Support
Posts: 345
Joined: 09 Jun 2010, 08:12

Re: Polygonal pads....

#7 Post by Serg » 28 Jan 2019, 10:22

woz wrote:
25 Jan 2019, 16:21
Alex wrote:You can do in different way. Create two overlapping rectangular pads instead one polygonal. In Component editor, you can link one pin to two pads when you attach the pattern to a component. Then there shouldn't be any DRC errors in PCB Layout.
Sorry to dig up this thread :roll: I am having similar issues with pad origin in polygons .... how do you "link one pin to two pads when you attach the pattern to a component".

Thanks!
You can create inner wire between several pads. It is similar Ratline in PCB Layout.
To create wire: left click on first pad + dragging + left click on second pad.
To delete wire: create wire above wire.
You do not have the required permissions to view the files attached to this post.

Post Reply