I want to learn to make nonstandard shaped pins

Here you can find discussions pertaining to finding or creating Symbols and package footprints. Anything to do with Schematic or layout parts will be placed in this discussion.

Moderator: Sunstone Moderators



I want to learn to make nonstandard shaped pins

Postby BoardsAreFun » Fri Jul 20, 2012 12:30 pm

I am working on a board and I have a part that I want to add that has large rectangular pins for a high current connection (see http://www.digikey.com/product-detail/en/ACS756SCA-100B-PFF-T/620-1238-ND/1829841). Now I understand that PCB123 has a limited drill selection which makes the boards very economical. However, is it possible to create pads with multiple round holes that overlap to create a roughly rectangular hole? Also around the large connections, the specsheet recommends having many smaller vias to create a good electrical/thermal connection. Is it possible to place smaller vias in the pad around a hole? If anyone knows how to do these things I would really appreciate some assistance.
BoardsAreFun
 
Posts: 3
Joined: Fri Jul 20, 2012 12:17 pm

Re: I want to learn to make nonstandard shaped pins

Postby Sal Hernandez » Fri Jul 20, 2012 2:36 pm

The data sheet is missing the R1, R2 and R3 dimensions. Do you know what those dimensions should be?
Regards,

Sal Hernandez
Software Support Engineer I
Sunstone Circuits
13626 S. Freeman Road
Mulino, OR 97042
Phone: 503-829-9108 x226
Fax: 503-829-5482
User avatar
Sal Hernandez
 
Posts: 396
Joined: Wed Jul 06, 2011 12:00 am

Re: I want to learn to make nonstandard shaped pins

Postby BoardsAreFun » Fri Jul 20, 2012 4:10 pm

I do not know the values for those and I am currently trying to contact Allegro Microsystems to get this information.
BoardsAreFun
 
Posts: 3
Joined: Fri Jul 20, 2012 12:17 pm

Re: I want to learn to make nonstandard shaped pins

Postby BoardsAreFun » Mon Jul 23, 2012 1:46 pm

I have received a reply back from Allegro Microsystems' technical support and the measurements are as follows: R1 is 0.039", R2 is 0.079", and R3 is 0.118". So now, how would I go about making this footprint?
BoardsAreFun
 
Posts: 3
Joined: Fri Jul 20, 2012 12:17 pm

Re: I want to learn to make nonstandard shaped pins

Postby Sal Hernandez » Tue Jul 24, 2012 7:59 am

The part is not one that can be made in PCB123 easily. And once you have it made it will result in lots of errors. Select Design > New Footprint to begin. Start with pins 1 – 3. The data sheet gives you the size, shape and positions. The pads for the slotted pins are especially difficult. PCB123 does not support slots so you can set your grid to 1mm and use overlapping 1.016mm holes to create the slots (EDIT: slots are now available in PCB123 v5). Once you have the slots in place you will need to create the custom pad shape for the slot. Right click on the center pin in your slot select Use Pin as origin. Next set your grid to R3. Use the draw polygon toll to draw a box around your pins. Now move your origin to one of the pins at either end of the slot. Left click a corner of the box and move it to the first grid point beyond the slot. Repeat these steps until you have rectangular boxes round your slots.

Right click on a corner of your rectangle and select convert corner to arc a then enter in the appropriate radius. Repeat for all corners. Now that you have oval outlines, we will create the gap between pads. Set your origin so that it is centered between your two slots by right clicking on Pin2 of you part. Now set your grid to .5mm. If you don’t already have your grid visible you will now want it. Go to the Edit Panel and make sure the box next to grid is a color and not a red x.

Your oval shapes will overlap. Go to the edit panel and select the box labeled Wire Frame then place your mouse at the point the ovals overlap and press the d key to delete corners until you are near the first .5mm grid points. Once you get close to the grid point, click on the straight segment and move the corners on the nearest grid point to ensure you have a straight vertical line that is .5 mm from the center point. Repeat these steps for the other pad.

The pads are now the correct shape. Right click on the oval outline and select Toggle Filled/unfilled to fill the shape. Right click again on the shape and change the layer to top. You can either repeat these steps for the bottom layer pads and top mask openings or just copy the pads you have just created and paste them on the appropriate layers.

Placing the stitching vias in a round pattern is discussed in the forum post below.

PCB - How To Create A Footprint With A round Pin

Once you have all of the pins in place you can use the draw polygon tool again and draw in the component shape then save your work.

The only issue that I now see is that the custom pad shape does not have the appropriate solder mask opening for the bottom layer. Please see the attached file. I had to manually add the mask openings by copying the polygon shapes from my footprint and pasting them onto the layout, moving them to the bottom mask layer then moving them into position.

Since this footprint requires a slot you cannot order this design directly through the PCB123 software. You must go to the Sunstone Printed Circuit website and order through the PCB Full Feature service.

I have attached my attempt at the footprint. You can copy the information from my 123 file into your design if you like. The information above is specific to your question. The link below is a general description of the

PCB123 parts creation process.

Please feel free to contact customer support if you have any questions.
Attachments
example.123
(19.25 KiB) Downloaded 203 times
Regards,

Sal Hernandez
Software Support Engineer I
Sunstone Circuits
13626 S. Freeman Road
Mulino, OR 97042
Phone: 503-829-9108 x226
Fax: 503-829-5482
User avatar
Sal Hernandez
 
Posts: 396
Joined: Wed Jul 06, 2011 12:00 am




Return to Schematic and Layout Parts (Libraries)

Who is online

Users browsing this forum: No registered users and 0 guests