Stats

  • Locked Locked
  • Replies 18
  • Subscribers 171
  • Views 30115
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

basics of thermal pad / power pad footprint creation

erivas

Hello, I'm new to Cadence, coming from Altium. I'm using Allegro Design Entry HDL and PCB Editor, rev 16.3.

As part of the new design and "new to designing with Cadence" process, I am creating parts for our library and I'm having some trouble with a TI SON part that includes a thermal pad or power pad. Here is a snap shot from the TPS6120:

 TI TPS61202 Footprint

At this point, I've made the pads in the padstack editor (but made them rectangles since I didn't know how to make it a rect at one end and rounded at the other) and used the symbol creation wizard to make a SOIC. To make the thermal pad I placed a filled polygon on the Etch/top layer and it is one large pad with the outline like above.

Question: How do turn my filled polygon into a ground pin (or should I not?) and how do I add the soldermask layer to something I've drawn like this?

Question: How do I add vias to my footprint? My plan was to create the via in the padstack editor then place them in the appropriate places but I have some confusion as to whether the pad/via structure is just supposed to sit there dangling or if it should be assigned a pin # (ground).

I did search the forum and came across the thread Thermal Pad Shape with Vias In it a poster mentions that he makes these pads using multiple surface mount style pins. I think I can figure out how to do this but I'd appreciate any tips on setting up the tools and pads so that things are properly done.

Picture of the pad made from pins:

pad of pins

  • steve

    You can draw non standard shaped pads by creating a shape symbol (*.ssm) then add that shape to a pad using Pad Designer. You can add multiple shapes for etch, mask and paste using the same process or use null for the layers in pad designer and draw the mask and paste when creating your symbol. Add the vias to the thermal pad by either going into add connect mode and double clicking to add vias (the same as in PCB mode). You will get DRC's until the symbol is loaded into PCB Editor with a netlist, the vias then take on the.e same net as the pins. The tab pad would be another pin (i.e. pin 21) which would need to be on your schematic symbol connected to GND.

  • erivas

    steve said:

    You can draw non standard shaped pads by creating a shape symbol (*.ssm) then add that shape to a pad using Pad Designer. You can add multiple shapes for etch, mask and paste using the same process or use null for the layers in pad designer and draw the mask and paste when creating your symbol. Add the vias to the thermal pad by either going into add connect mode and double clicking to add vias (the same as in PCB mode). You will get DRC's until the symbol is loaded into PCB Editor with a netlist, the vias then take on the.e same net as the pins. The tab pad would be another pin (i.e. pin 21) which would need to be on your schematic symbol connected to GND.

     

     

    Thanks Steve, I will look into the process for creating a shape symbol. I've seen reference to them in my searches but wasn't sure what they were or how you made them.

    I wonder if I could copy the shape I already made on the board and paste it into the shape symbol tool?

  • redwire

    erivas said:

    I wonder if I could copy the shape I already made on the board and paste it into the shape symbol tool?

     

    Yes, but it's not called copy/paste in Allegro.  Allegro can export a "subdrawing" (File->export menu).  Follow the prompts and think about the origins of the items you want to export (use right mouse to select a body center for example).

    Then in the symbol editor use File->Import->Sub Drawing.  Again, the origin will need to be thought out.

    One thing to be aware of is that the layer names being exported/imported have to be identical.   Shapes for pads would most likely be on etch-top and etch-bottom so that won't be an issue for your problem at hand.

    Use your color control and find box to filter out junk you don't want to copy.

  • erivas

     thanks again, this was helpful. I ended up making the shape from scratch as a flash instead of trying to copy or export it. added it as the 11th pin and everything looks pretty good.

  • Gopintj1

     Dear Members,

     Please guide me how to create Special Symbol (.ssm) file using Cadence allegro 15.2

     

     

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.