Stats

  • Locked Locked
  • Replies 6
  • Subscribers 167
  • Views 17971
  • 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

A question about merge two PCB design in the same panel?

Leeya

Hello,

I am merging two PCB layout into the same panel. I did merge the schematic first, and then import one PCB layout into another design. This process takes a lot of time and energy. 

I am just wondering is there anyother way or software could simply merge two pcb layout together. Not too expensive~~

Thanks 

  • steve

    Have a look at Downstreams CAM350. You can import either IPC2581, ODB++ or gerber from Allegro from both PCB's to make your panel. The alternative (and free solution) would be simply to draw the panel on a layer in Allegro which shows both board outlines only and then let the PCB Fabricator put the actual data in. He only needs to x y locations of the boards.  

  • Leeya

    Hello Steve,

    Thanks for you suggestion. I did contact with Downstream and request for a software quote from them. It doesn't look like a cheap software, staring from 3,000$. 

    However, I am very interesting in the second way. Do you think if I give the general panel information, and then they will help me put two design in panel?

    I would like merge two design together, but it takes too long time to clean up a simple merge. I am looking for a long term solution. Thanks you so much.

     

     

     

  • Leeya

    Hello Steve,

    I am trying another way, make one of design as module, and then place it into another design. it work much better. However, I looks like I have to add a character and "_" before it original refdes name. How to avoid add any other character while merging two design?

    If this solution works, This will become the our long term solution.

    Thanks

  • Azertyop
    Hello,

    Here is the way I process.
    It works for different boards with SAME layer number.
    First, I use it only to create drill, artwork data, and fabrication drawing.
    By this way, PCB fabricators don't need to manipulate data. It's your responsability to give the right data.

    In each board, I create a view file (.color) with all necessary layers.
    Then I create a module of each board.

    In a new "panel" brd, I add the modules. No matter what are the refdes, i don't use them for cabling.
    I can draw a panel outline, additionnal drills, cuttings, text... I can rotate the modules to fit space.
    Like any other board, I create drill, artwork and fabrication drawing for the panel.

    When changing something in a board, I create again the module and I refresh it in the panel, like a symbol.

    Be careful with route_keepin and package_keepin from boards:
    If they belong to a symbol, don't select 'symbols' in the find filter when creating the modules.
    If you take this data in the modules, you should not be able to paste the module in the panel.

    Also, take a look to keep some space between boards for overlapping components.
  • Ejlersen

    Hi

    An alternative to downsteam is FloWare panelization but the cost will be about the same, however CAM350 will do a lot more with respect to DRC analysis.

    http://orcadmarketplace.com/ProductDetails/tabid/93/ProductID/24/Default.aspx 

     

    Also GerbTool from  Wise technology is a very capable piece of software.

     

    If you want to place safe, I would let the pcb manufacturer do the job and responsibility - that might end up being cheaper and more secure for starters. 

    Best regards

    Ole 

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.