Stats

  • Locked Locked
  • Replies 19
  • Subscribers 167
  • Views 14081
  • 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

Create an assembly drawing - revised to create fab notes 11-9-11

engineer66219
Hello everyone, I am attempting to learn how to create assembly drawings from within pcb editor. I have searched the forums here and looked through the cadence software documents; however, I cannot find any information on how to create an assembly drawing. When I click on the assembly drawing command in pcb editor, I get an error stating variants.lst not found. Can someone explain how I can create an assembly drawing or please point me to some literature that will explain. Please keep in mind that I have no idea where to even start with this process, so please be as thorough as possible. Thank you,

  • Hi,
    1. For create assembly  drawing. In allegro you must visibility package geometry- assembly, refdes - assembly. Then sort refdes.
    2. Assembly drawing usualy must larger than dimension board outline. For scale dimension. In allegro you export ->.dxf . Then you use software AutoCad for scale (scale 2X, 3X...). Then import back allegro.
    3. In allegro -> Artwork ->create assembly drawing (add subclass drawing format ...)

    For your reference !!!

  • For item 2, this step is unecessary. You can just create a drawing blank (for the border) at the scale you need, then let the printer plot the page to fit. If you really want to scale the assembly drawing up use the Manufacture - Drafting - Create Detail, set the scale in the options menu then draw a rectangle around the items you wish to scale up. The scaled detail will be on your mouse ready to place.

    You can then either set the display to show the layers on/off that you need (to cover notes, details etc) then plot (or create an artwork)....

  • I believe I have asked for the wrong report here I apologize. What I meant to ask for was how to export fab notes from within pcb editor. I believe this is possible. I thought I saw somewhere a screenshot of board house fab notes that were created from within allegro (and possibly even an assembly drawing). Can someone explain how to export fab notes which includes layer stackup and text.
  • Hello,

    Manufacturing > Variants > Create Assembly Drawing is used in conjunction with the Variant Editor used by Allegro Design Entry HDL (Variant Editor will generate the variants.dat file).   Basically, it generates the appropriate assembly views in Allegro based on the population status defined in Variant Editor and that is all it does. (effectively deleting the outlines of unpopulated components and pushes the view to a different subclass)

    You can create your assembly drawings in Allegro and do not need to export it to an external CAD tool to generate them.  The only real issue is that to generate a Bottom Assembly drawing you will need to create a plot file and load it back into Allegro mirrored so you can see the assembly text right reading.    The main issue is the Bottom Assembly view can become out of date if you make placement changes and will have to regenerate the plot and load it back into Allegro mirrored.  Steve provided a suggestion about generated a scaled down format to maximum your assembly views which is a great tip – have used it myself.

    By “create plot a plot file” I mean use File > Export > IPF that generates a Cadence intermediate plot file of what is displayed than it can be loaded back into Allegro at different a scale, different class/subclass or mirrored for assembly documentation.  Using Manufacturing > Dimension/Draft > Create Detail can do the job as well but the Text Strings will get exploded in the resulting Assembly view which will make any resulting PDF not text searchable.

    Hope this helps – good luck.

    Cheers,

    Mike Catrambone
    Plexus Engineering Solutions

     
  • This is what I am trying to do: [http://www.youtube.com/watch?feature=player_detailpage&v=B5JgivLpjAs] (not sure how to post a hyperlink on this forum) Do I have to have this software or is something similar to this available locally from within pcb editor?
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.