Home > Community > Forums > PCB Design > Footprint with custom pad shapes

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Footprint with custom pad shapes 

Last post Mon, Jul 23 2007 9:39 AM by archive. 5 replies.
Started by archive 23 Jul 2007 09:39 AM. Topic has 5 replies and 1840 views
Page 1 of 1 (6 items)
Sort Posts:
  • Mon, Jul 23 2007 9:39 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,910
    Footprint with custom pad shapes Reply

    Hi all, Does anybody know how to translate a custom pad shape .ssm into .pad file in order to edit the layers in padstack designer? I need to create a footprint for a special inductor which has irregular pad shapes, but in the allegro documentation isn't well explained (IMHO). Besides creating an .ssm custom pad shape, I have created a .dra for the inductor and have added two filled shapes in the class/subclass => Etch/Top, but the pin number doesn't appear and cannot edit the padstack for that kind of pad shape, the footprint isn't correct for sure I'm sure I'm missing something, some guidance will be appreciated. Thank's in advance.


    Originally posted in cdnusers.org by luissito
    • Post Points: 0
  • Mon, Jul 23 2007 10:02 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,910
    RE: Footprint with custom pad shapes Reply

    You will need to define a padstack which references the shape symbols (.ssm). Create a surface mount padstack with the padstack type "Single" and define your Regular pad as a Shape using the Geometry pulldown. The box to the right of the shape field that has three dots inside it is a browse button so you can select the shape symbol (.ssm) to be used. You will probably need to create a solder mask shape symbol to follow the contour of the top layer pad and may need one for the solder paste as well if you don’t reuse the top layer pad shape symbol. I attached images of the pad_designer forms for reference. Hope this helps, Mike Catrambone UTStarcom, Inc.


    Originally posted in cdnusers.org by mcatramb91
    • Post Points: 0
  • Tue, Jul 24 2007 1:36 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,910
    RE: Footprint with custom pad shapes Reply

    Thank's for the help Mike. I have followed your instructions, but I have used the same .ssm for the Begin Layer and for the soldermask_top as I want the same aperture. But now, when I try to save the padstack it gives me the error "Pad stack origin outside all pads" Regards Luis.


    Originally posted in cdnusers.org by luissito
    • Post Points: 0
  • Tue, Jul 24 2007 6:37 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,910
    RE: Footprint with custom pad shapes Reply

    Most likely when you created your shape symbols with the 0,0 origin outside of the shape area. When creating shape symbols you should have the 0,0 in the center of the shape or where you want the pad center to be but it must be inside of the shape area. Another requirement for shape symbol is that the shape is defined on Class ETCH and Subclass Top which you probably already have correct but I figured I would mention it anyway.

    Let me know how you make out,
    Mike Catrambone
    UTStarcom, Inc.


    Originally posted in cdnusers.org by mcatramb91
    • Post Points: 0
  • Tue, Jul 24 2007 8:04 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,910
    RE: Footprint with custom pad shapes Reply

    Thank's a lot Mike, I've followed your steps and now it seems to be ok. You were right, the pad shape was created in Etch/Top. The only thing it could be wrong, is the fact that I haven't used flash shape for the thermal relief and antipad under padstack designer, simply I didn´t fill the thermal relief and antipad columns because I'm not going to attach any pad to a plane, and if a copper area surrounds the component it will be applied the cleareance of the plane, won't it? Thanks again. Regards.


    Originally posted in cdnusers.org by luissito
    • Post Points: 0
  • Tue, Jul 24 2007 1:52 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,910
    RE: Footprint with custom pad shapes Reply

    The thermal relief and antipad values are not required from surface mount pads because they are on the surface layers. You can specify values but by default dynamic positive shape will void the pins accordingly using the Pin to Shape DRC rules.

    Mike Catrambone
    UTStarcom, Inc.


    Originally posted in cdnusers.org by mcatramb91
    • Post Points: 0
Page 1 of 1 (6 items)
Sort Posts:
Started by archive at 23 Jul 2007 09:39 AM. Topic has 5 replies.