Stats

  • Locked Locked
  • Replies 4
  • Subscribers 163
  • Views 16849
  • 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

Silkscreen questions

arcwilson

I've finally finished my first layout in PCB Editor (whoo!) and I'm trying to generate the artwork files, but I'm having some silkscreen issues.

1.  I'm trying to use "Manufacture->Silkscreen.." to generate the Autosilk layers in the Manufacturing class, but for some reason it copies everything from "Package Geometry/Silkscreen_Top" EXCEPT a logo that I imported using Dave Elder's logomaker skill (which is fantastic btw!).  When I check the info on the logo, it all its shapes show "Package Geometry/Silkscreen_Top", and I've set the Auto Silkscreen options for Package Geometry to both Silk and Any, but still get the same results.  Is there something I'm not understanding about how Auto Silkscreen works?

2.  The second question I have is whether there is a way to set the silkscreen line widths for a layout on a global level, instead of pre-defining them within the individual package symbols.   For example, create all library symbols with a silk line width of 0, and then once the symbols are placed in a design, define a global silk line width for the entire design.  

 Once again, thanks for the help.

--Chris

  • eDave
    Hi Chris,

    1/ Another of my utilities (in widespread use) handles this and other issues with silkscreen.
    Look for autosilkUtils.il (http://sourcelink.cadence.com/docs/files/SKILL/Allegro_SKILL_Code/autosilkUtils.il)

    2/ That would be relatively easy using Skill. I don't know whether you could do it easily otherwise.

    Cheers, Daev
  • oldmouldy

    On the second Q, setting the "Undefined Line Width" on the FIlm Control tab will do this. This value needs to be set for each film and will override ANY item in the output that has a 0 width, there will also be a message in the log that the line width was replaced with the override.

  • BillZ

    Hi,

    It is easy to change all of the silkscreen widths. Just display the layers and do an edit change windowing around the design to the desired width.

    The reason the logo doesn't copy to the autosilk layer is porbably due to the fact it is a shape. Autosilk works on Lines and text. It does not work on every silk element on the layer choosen.

    I would not use the undefined line width in the film record because it may create errors. There is no check to see if the silk is touching a pad. Set the silk width in the board or symbol and use the checks built into the tool.

    I find it is best to build your footprints to a standard this would include line widths and text block settings. In the long run it will save you time. If your design needs some variation from the standard you can override it in the board.

     

    Regards,

    BillZ

    EMA Design Automation  

  • mcatramb91

    I personally don't use the Silkscreen cleanup routines (AutoSilk) because it doesn't always do the best job with moving Ref Des Text around.  Basically, I clean up the Ref Des Silkscreen manually (doesn't really take that long) and instruct the fabricator to trim an silkscreen to the soldermask openings.  This way the important silkscreen text is placed / visible on the PCB and I don't have any chance of having silkscreen on top any soldermask exposed areas which could cause issue during assembly.

    Of course my component library silkscreen_top layer has already been modified at the symbol level to avoid pins / vias with a clearance to insure that the Undefined Line Width used for the silkscreen during artwork generation is still clear of any component pins.

    My two cents,
    Michael Catrambone
    UTStarcom, Inc.

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.