Stats

  • Locked Locked
  • Replies 4
  • Subscribers 164
  • Views 19008
  • 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

Issue: Updating footprints and padstacks in Allegro 17.2

VipulP

Hello,

I am encountering issues when updating a footprint and its padstacks in Allegro PCB Designer version 17.2 for Windows 8.  This is for a footprint with a fairly specialized application.  I am creating the land pattern for a 32 pin QFN device where, instead of assembling the part on an exterior layer, we will be milling away a cavity post PCB lamination where the footprint will become exposed on an internal layer.  Since SMD pins in the Pad Editor are only offered for the Begin and End layers, I need to create this padstack using a thru pin pad.  My thought is to pick an unused drill size that I can remove from the drill file later, define the internal pad shape and the top pad that will be milled away--much like a blind via. The bottom layer will be undefined since I will have routing on this layer.  

I am able to successfully define and update such a pad for the center thermal/ground pad of the QFN; however, the peripheral lead pads of the QFN will not update to include the internal layer pads that need to be populated to connect the device.  I am using the following command sequence to update symbols: Place->Update Symbols->Package Symbols->[Device of Interest]->Refresh.  I have also tried checking the "Update symbol padstacks from library" option with no success.  Additionally, I have double checked my pad path to ensure that duplicate pads have not been defined in the various libraries I have included.  Nothing is working. Attached are images of the Pad Editor for the pads I'm using.  Any thoughts or ideas would be greatly appreciated!! 

Cheers,

Vipul

QFN Ground pad that successfully updates to include the bottom and internal layer.

QFN lead pad that will not update to include internal layer

  • mcatramb91

    The "Update symbol padstacks from library" option should pull the updated padstack from the library.  Have you tried Replace Padstack (Tools > Padstack >Replace) and enter "old padstack" and "new padstack" as the same name and click Replace button under the Options tab, this will refresh the padstack as well.  Also try placing the symbol in a fresh design to see what happens with the QFN Lead Pad.

    Do you have access to Allegro PCB Designer and the Miniaturization option?   Using this license you can place components on an inner layer which automatically re-targets the padstacks and create the cavity for you.   This would save you a lot of time and effort.

  • VipulP
    in reply to mcatramb91

    Thanks for the quick response!  Replacing the padstack with the same name and with a new name did not work.  I have the miniaturization option so I'll give that a shot. Thanks!!

    -Vipul

  • mcatramb91
    in reply to VipulP

    Hi,

    I will give you a quick crash course on how to embedded a component.

      1. Open the Cross Section Editor and change the Embedded Status to "Body Up" for the layer you want the component placed
      2. Change the Embedded Status on the all layers above the Body Up layer to "Protruding allowed"
      3. You can adjust the clearance information under the Embedded Layers Setup tab, along the bottom, as required
      4. In Allegro, add the property "EMBEDDED_PLACEMENT" with a value of "OPTIONAL" using Edit > Property to the component to be placed internally
      5. Place > Manually > [Device of interest] or select the component already placed, RMB > Place on Layer > [Embedded layer]
      6. That's it.

    For more information check out the Best Practices doc: https://support1.cadence.com/tech-pubs/Docs/embbp/embbp17.2-2016/embbp.pdf
    NOTE: The document still shows the Embedded Component Setup in a separate form, it was incorporated into the Cross Section Editor in 17.2

    Hope this helps,
    Mike Catrambone

  • VipulP
    in reply to mcatramb91

    Thanks Mike!  I was unaware of this feature, but it worked out great!  The only problem is that one of the pads in my footprint has a plated via array embedded in the padstack that connects to a pad on the bottom layer.  These vias and the bottom layer pad were removed when I retargeted the footprint to an internal layer.  I had to manually edit the drill file and hand draw the bottom pad to get this to work.  I will look through this document to see if it covers such an application.  

    Cheers, 

    Vipul

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.