Home > Community > Forums > PCB Design > Artwork Generation

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: *

 Artwork Generation 

Last post Wed, Jun 19 2013 9:41 AM by B Price. 8 replies.
Started by stellar 20 Jan 2010 03:39 AM. Topic has 8 replies and 3506 views
Page 1 of 1 (9 items)
Sort Posts:
  • Wed, Jan 20 2010 3:39 AM

    • stellar
    • Top 75 Contributor
    • Joined on Fri, Nov 13 2009
    • Posts 105
    • Points 1,890
    Artwork Generation Reply

    Okay how do the pros set this up quickly? I find for each board it is a very tedious and painful process to get the correct folders set up and the classes and subclasses to get the silkscreen and soldermask and etch all setup.  I turn colors on and off in the workspace then add the folders and still find I work to do to get it all correct. In this regard I definately liked the simplicity of Layout but hope it's just operator ignorance. 

    • Post Points: 35
  • Fri, Jan 22 2010 1:54 PM

    • oldmouldy
    • Top 10 Contributor
    • Joined on Tue, Jul 15 2008
    • Woking, Surrey
    • Posts 1,445
    • Points 24,590
    Re: Artwork Generation Reply

    Setup the films that you need for the data other than "ETCH" layers. Then in Film Control, select these layers checkboxes, NOT the etch, hover the mouse over a film name and right-click>Save All Selected - this will write a file called "Film_Setup.txt". Move this from the design folder to "somewhere" that you store common design data. Then, for the next design, go to the Artwork, Film Control and use the "Add" button, pick the saved "Film_Setup.txt", and your "other films" will be added to the output list. NOTE: the Film_Setup.txt file will have the parameters from you original design embedded so check carefully if your designs have some english and some metric databases, or use differing resolutions, decimal places - since the parameters stored are "numbers" and do not have units attached.

    • Post Points: 35
  • Fri, Jan 22 2010 6:34 PM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,243
    • Points 20,215
    Re: Artwork Generation Reply

    Allternatively you can use a Parameter file. Go to a board that has everything defined and use File - Export - Parameters, Make sure that at least Artwork is checked but there is also design settings, color layer and palette, text size and application / command parameters, export the file, then on your new board file use File - Import - Parameters, browse to the location and import, everything is defined.

    • Post Points: 20
  • Fri, Jan 22 2010 9:00 PM

    • Ejlersen
    • Top 10 Contributor
    • Joined on Mon, Jul 28 2008
    • Aalborg, Copenhagen
    • Posts 569
    • Points 10,080
    Re: Artwork Generation Reply

    Hi Stellar

    You could try the attached skill program, place it in your skill folder and run using "ns_gerber" command. Feel free to edit the code to suit your needs.

    Best regards

    Ole

    Best regards Ole
    • Post Points: 20
  • Tue, Jan 4 2011 7:56 PM

    • LYHLYL
    • Not Ranked
    • Joined on Wed, Dec 29 2010
    • Posts 1
    • Points 5
    Re: Artwork Generation Reply

    HI ejlersen,

      why i can not run Revision 15.7?

    • Post Points: 5
  • Thu, Mar 21 2013 11:40 AM

    • DonlAZ
    • Top 200 Contributor
    • Joined on Tue, Aug 28 2012
    • Chandler, AZ
    • Posts 38
    • Points 535
    Re: Artwork Generation Reply
    oldmouldy:

    Setup the films that you need for the data other than "ETCH" layers. Then in Film Control, select these layers checkboxes, NOT the etch, hover the mouse over a film name and right-click>Save All Selected - this will write a file called "Film_Setup.txt". Move this from the design folder to "somewhere" that you store common design data. Then, for the next design, go to the Artwork, Film Control and use the "Add" button, pick the saved "Film_Setup.txt", and your "other films" will be added to the output list. NOTE: the Film_Setup.txt file will have the parameters from you original design embedded so check carefully if your designs have some english and some metric databases, or use differing resolutions, decimal places - since the parameters stored are "numbers" and do not have units attached.

    Thanks so much for this oldmouldy!!! I don't know how many hairs I would have left if it wasn't for this forums and the contributers here!!
    • Post Points: 5
  • Wed, Jun 19 2013 8:31 AM

    • B Price
    • Top 500 Contributor
    • Joined on Wed, Jul 20 2011
    • Posts 25
    • Points 510
    Re: Artwork Generation Reply

    I had the same question as the OP.  The methods steve and oldmouldy outlined both look great.

    If I save a board template with the film control configured correctly, will it carry into a new design if I use that template board as an input file?

    I guess it boils down to whether the Parameter file contents are automatically part of a .brd template...

    • Post Points: 20
  • Wed, Jun 19 2013 9:11 AM

    • Ejlersen
    • Top 10 Contributor
    • Joined on Mon, Jul 28 2008
    • Aalborg, Copenhagen
    • Posts 569
    • Points 10,080
    Re: Artwork Generation Reply

    Hi

    No, the parameters will not follow your board file.

    I would recommend you to setup a site environment, it involves the following

    1. create env variable inside system settings and call it cds_site with a value of a path on the Network e.g., u:/rd/Cadence

    2. create folder structure u:/rd/Cadence/pcb/nclegend and place your golden nc_param.txt in this directory.That will be the basis for all your new boards with respect to drill parameters

    3. inside folder structure u:/rd/Cadence/pcb/ place your golden art_param.txt in this directory.That will be the basis for all your new boards with respect to artwork parameters

     

    You can enhance this with a lot more functionality if you want, for example

    site.env file with default shortcuts, settings etc. inside u:/rd/Cadence/pcb folder  

    If more than one user, just create the cds_site variable on each client and then you share the setup.

    You can read more about this in the readme.txt file inside C:\Cadence\SPB_16.6\share\local\pcb

    Also a complete example configuration directory structure is shown at C:\Cadence\SPB_16.6\share\local\pcb

     

     

    Best regards

    Ole

    Best regards Ole
    • Post Points: 20
  • Wed, Jun 19 2013 9:41 AM

    • B Price
    • Top 500 Contributor
    • Joined on Wed, Jul 20 2011
    • Posts 25
    • Points 510
    Re: Artwork Generation Reply

    Thanks, Ole - I'll give this a try.  It sounds very reasonable.

     

    Edit:  I looked into that readme.  Am I correct in assuming step 3 should read as follows?

     3. inside folder structure u:/rd/Cadence/pcb/parameter place your golden art_param.prm in this directory.That will be the basis for all your new boards with respect to artwork parameters

    • Post Points: 5
Page 1 of 1 (9 items)
Sort Posts:
Started by stellar at 20 Jan 2010 03:39 AM. Topic has 8 replies.