Stats

  • Locked Locked
  • Replies 7
  • Subscribers 168
  • Views 14313
  • 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

Refdes reappearance and via soldermask problems

shangwu

Question 1:
I accidently deleted a REFDES (top silkscreen class) on a component.  How do I make it to appear again?  I unplaced the component and placed it again, but didn’t help.  I can of course manually type in the text, but it does not attach to the component.

I read the follwing response, but where do I find the "Component Attachment" command?

 http://www.orcad.com/forums/ShowPost.aspx?PostID=23258

Question 2:
How do I delete the soldermask of a via (underneath a chip)?  I displayed the soldermask only and tried deleting it, but it deletes the via itself.  I only want to get rid of the soldermask of that via.
Thanks.

  • girish

     Hi,

     ANS1: Go to place-> updates smbols->select the package symbol [which redes you have deleted accidently] ->do refresh.

    ANS2:Its not possible to delete the soldermask on pad directly . Go to the Tools->padstack-<modify design padstack->slect via[which you want to delete soldermask]->edit padstack ->make soldermask top & bottom value to null.&  do file->update to design& save to file .

     Note that it will affect to all via's of same padstack name. If want to delete SM for some perticular  set of via's then use different naming for padstack .

    HTH

    Regards,

    Girish kumar 

  • steve

    For the soldermask point you can use Tools - Padstack - Replace then select the via in question, then check the Options menu and select Instance, This gives the via in question a new name and any edits will only affect this via. Then continue to edit as per Girish's comments.

  • shangwu

    Hi Girish,

    I tried refreshing the symbol, but it didn't work.  I even deleted the old symbol and replaced it, but still the same.

    The no mask via works though.  The only thing is that I can only replace all the vias or do one via at a time.

    Thanks.

  • girish

    Refreshing the symbol works here!

    * Have you selected the perticular symbol during refresh?

    *Recheck your library whether its having the refdes mark under REFDES/SILKSCREEN TOP class 

    * If above steps not works then change the footprint name  ,update to schematic & import.

    If you are aware of skill files . Check in skill forum Mr.Steve posted some skill files [replace via]  using that you can replace group of vias by temp grouping . It works great I am using it .

     

    Regards,

    Girish kumar 

  • steve

    There is another way to replace padstacks..... In general edit mode window select or RMB - selection set - select by polygon, double click to create the polygon, the vias will hi-light then RMB over any of the vias and choose Replace - Padstack - Selected Instances then pick the via name you want to use....

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.