Home > Community > Forums > PCB Design > Creating PCB panels in PCB Editor

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Creating PCB panels in PCB Editor 

Last post Fri, Jul 19 2013 12:00 AM by Pete01. 6 replies.
Started by Szabolcs88 22 Sep 2012 09:28 AM. Topic has 6 replies and 1648 views
Page 1 of 1 (7 items)
Sort Posts:
  • Sat, Sep 22 2012 9:28 AM

    • Szabolcs88
    • Not Ranked
    • Joined on Thu, Sep 13 2012
    • Romania, Romania
    • Posts 11
    • Points 335
    Creating PCB panels in PCB Editor Reply

    Can you duplicate your pcb in editor? I've just finished designing a pcb and I want to create a panel with 18 PCB total (9 rows 2 colums) with a technical edge on each side so than i could send the manufecturer a gerb files. How can i make a panel and put 18 same pcb on it? I have to make 18 schematics in capture and after i can copy pcbs in editor? Can it be done in pcb editor or do I need some patch for it..?

    Thanks Szabolcs

    • Post Points: 35
  • Sun, Sep 23 2012 2:43 PM

    • ScottCad
    • Top 50 Contributor
    • Joined on Sat, May 26 2012
    • Roswell, GA
    • Posts 176
    • Points 2,775
    Re: Creating PCB panels in PCB Editor Reply

    Not really like you are expecting.

    When you create a PCB in the editor it will be an electrical representation of your schematic. That is 1 to 1. If you duplicate your board in the PCB editor which you can do you will no longer have that 1 to 1 relationship with the schematic.

    What you need is a cam editor to create your Panel from the gerber files you created in the PCB Editor.

    Normally when you send your gerber files to a PCB Manufacturer they will create the film for you from the gerber files.

    Another way to think of it is this. The schematic and PCD contain electrical information such as Nets. The gerber file is just a graphical representation of your electrical Cad data.

    The gerber file does not contain any "electrical" information per-se.. It is just a graphic.

    Thanks Scott. 

    • Post Points: 5
  • Wed, Jul 17 2013 9:28 PM

    • Pete01
    • Not Ranked
    • Joined on Wed, Jul 17 2013
    • Posts 3
    • Points 45
    Re: Creating PCB panels in PCB Editor Reply

      Yes I don't understand why there is not an easy way to panelize in orcad either, unlike Altium.

    I did come across a company called  flowcad who have a plugin called "FloWare Apps for OrCAD and Allegro" which does what you are asking for, however it's very expensive.

    Has anyone else came across a method which beats this on price/performance.

    • Post Points: 20
  • Wed, Jul 17 2013 10:45 PM

    Re: Creating PCB panels in PCB Editor Reply

    The procedure is quite lengthy

    1,you should refrence designators in your SCH like, C21_1 and net names should also have "_1" in there end.

    once you will have refdesg and netnames like these when you will copy the refdesg will automaticly increses and net names will need to replace from _1 to _2 and so on.

    2, once you copy to the required quantity generate and load the netlist in Allegro PCB editor.

     3, now go to create module and make a module of your current PCB and open that module in new canves then go to export placement.

    4,open the generated placement file in notepad and replace "_1" to "_2" and save the file

    5,now go to import palcement and place the components at new palce and afetr that copy all clines and shapes ect from initial PCB to 2nd one.

    6, repeat point 4 and 5 as many times as needed.

    Regards

    Nayyier 

    • Post Points: 20
  • Wed, Jul 17 2013 11:05 PM

    • Pete01
    • Not Ranked
    • Joined on Wed, Jul 17 2013
    • Posts 3
    • Points 45
    Re: Creating PCB panels in PCB Editor Reply

     Hey Nayyierwajih,

     Well that method is defiantly cheaper, however I don't know if it's a good use of time, keep them coming!

    Also does anyone have any good footprints of panels which they would like to share? I'm looking for an A4 size or 297mmx210mm.

     Thanks
    • Post Points: 20
  • Thu, Jul 18 2013 1:12 AM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,173
    • Points 19,025
    Re: Creating PCB panels in PCB Editor Reply

    Talk to your fabricator who can give you a list of standard panel sizes, tooling hole locations and fiducials should come from the Assembler. In regard to panelization why not just draw the steo and repeat information with just the board outline. This gives the manufacturer all the info he needs. He will probably want to copy the detail himself once he has run through there standard front end processes.

    You can even create a new subclas under Manufacturing called Panel and then draw the outline, tooling holes, route detail and all you need to create the panel. Then make a new artwork showing this detail.

    • Post Points: 20
  • Fri, Jul 19 2013 12:00 AM

    • Pete01
    • Not Ranked
    • Joined on Wed, Jul 17 2013
    • Posts 3
    • Points 45
    Re: Creating PCB panels in PCB Editor Reply

     Thanks Steve, all good points and this probably allows me to limp along. I have done something similar in the past prior to Altium having good panelization support.

     The main reason we do the panels our self is it means the artwork and pick n place file always match each other no matter who the pcb manufacturer or loaders are. In the past we have experienced issues with the PCB manufacturers doing their own thing which causes the loaders all kinds of issues. It also meant the pick n place file needed to be altered to cater for the extra elements in the panel.

    Where is if this is done in your PCB authoring software, the pick n place file is automatically generated correct and gives the PCB manufacturers no ability to introduce errors by doing their own thing even though you defined the position offsets. It simply made ordering PCB's more well defined.

    Another advantage is you can put all kinds of custom information on your tooling strip, we even have some tooling strips which double up as rulers. It does appear that Altium has an advantage over Orcad on this front so crossing fingers it makes it into a release in the future.

     Thanks for the comments.
    • Post Points: 5
Page 1 of 1 (7 items)
Sort Posts:
Started by Szabolcs88 at 22 Sep 2012 09:28 AM. Topic has 6 replies.