Home > Community > Forums > PCB Design > help with board outline gerber

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: *

 help with board outline gerber 

Last post Sun, Jan 19 2014 12:14 PM by mfris. 4 replies.
Started by mfris 18 Jan 2014 06:28 AM. Topic has 4 replies and 903 views
Page 1 of 1 (5 items)
Sort Posts:
  • Sat, Jan 18 2014 6:28 AM

    • mfris
    • Top 500 Contributor
    • Joined on Tue, Sep 18 2012
    • Durham, NC
    • Posts 20
    • Points 440
    help with board outline gerber Reply

    Hi everyone,

     

    I'm having a great deal of difficulty completing/verifying what should be an easy task - I would like to generate a .art (gerber) file that describes the board outline.  In this case, I just want to generate a simple rectangular outline.  I'm using 16.5.

     What I have done:

    -turn off all layers in Display->Color Visibility

    -turn on Board Geometry->Outline in the same color dialog box

    -set active layer to Manufacturing->Photoplot_Outline under Options

    -trace the Board Geometry->Outline layer in the Manufacturing->Photoplot_Outline layer

    -turn off Board Geometry->Outline layer so that my newly drawn Manufacturing->Photoplot_Outline layer is the only layer shown

    -go to Manufacture->Artwork, rt-click on existing film, Add

    -leave undefined line width as 0 for the new layer (or change to non-zero values 1 or 10 - tried multiple values)

    -open a new job, File->Import->Artwork, select newly created Outline artwork

    -in the same import window, leave default class/subclass options (or select new options, but Manufacturing/Photoplot_Outline is not a selection option) 

    -try to load, get a message that says No Photoplot file specified

     

    Questions:

    1) Am I generating the board outline gerber in a wrong/difficult way, or am I trying to view the board outline gerber in a wrong/difficult way (or both)?

    2) Help? 

    Any help or advice is greatly appreciated!  Thanks in advance.

     

     

    • Post Points: 20
  • Sat, Jan 18 2014 8:13 AM

    • mcatramb91
    • Top 75 Contributor
    • Joined on Thu, Jan 3 2013
    • Chelmsford, MA
    • Posts 97
    • Points 4,930
    Re: help with board outline gerber Reply

    Hello, 

    Manufacturing->Photoplot_Outline subclass is used to define the overall extents of your gerber file and it is not used to define the board outline. The Manufacturing->Photoplot_Outline subclass is not required as Allegro will default to the drawing extents when generating Artwork, if it doesn't exist.

    Basically, the Artwork film record must contain Board Geometry->Outline subclass and the Undefined Line Width must be set to a number higher than 0.  I updated your steps below:

    What I have done: (updated)

    -turn off all layers in Display->Color Visibility

    -turn on Board Geometry->Outline in the same color dialog box

    -set active layer to Manufacturing->Photoplot_Outline under Options (SKIP)

    -trace the Board Geometry->Outline layer in the Manufacturing->Photoplot_Outline layer (SKIP)

    -turn off Board Geometry->Outline layer so that my newly drawn Manufacturing->Photoplot_Outline layer is the only layer shown (SKIP)

    -go to Manufacture->Artwork, rt-click on existing film, Add

      leave   define the undefined line width as   0    10 for the new layer (or change to non-zero values 1 or 10 - tried multiple values)
          ---> You must define an Undefined Line Width and it cannot be 0.  I normally use 10.
     

    Hope this helps,
    Mike Catrambone

    • Post Points: 20
  • Sat, Jan 18 2014 11:51 AM

    • mfris
    • Top 500 Contributor
    • Joined on Tue, Sep 18 2012
    • Durham, NC
    • Posts 20
    • Points 440
    Re: help with board outline gerber Reply

    Thanks for the detailed and quick response Mike.

     

    I tried your modified procedure, but I find that I am still unable to import the generated file in order to review it (maybe I'm missing a setting somewhere else entirely?)  In fact, when I open the "Load Cadence Artwork" window, I can select "Board Geometry" Class, and "Outline" Subclass, but when I actually point the Filename field to my generated file, I hear a beep and my subclass field selection automatically changes to "Plating_Bar", and "Outline" is no longer offered as a subclass selection.  I am not offered a "Load file" button to select in the bottom middle of the window as I am with my other artwork layers.

     If it helps, here's what I see when I look at the contents of my outline file in a text editor:

     G04 ================== begin FILE IDENTIFICATION RECORD ==================*

    G04 Layout Name:  C:/SPB_Data/test.brd*

    G04 Film Name:    Outline*

    G04 File Format:  Gerber RS274X*

    G04 File Origin:  Cadence Allegro 16.5-S014*

    G04 Origin Date:  Sat Jan 18 14:00:43 2014*

    G04 *

    G04 Layer:  BOARD GEOMETRY/OUTLINE*

    G04 *

    G04 Offset:    (0.00 0.00)*

    G04 Mirror:    No*

    G04 Mode:      Positive*

    G04 Rotation:  0*

    G04 FullContactRelief:  No*

    G04 UndefLineWidth:     10.00*

    G04 ================== end FILE IDENTIFICATION RECORD ====================*

    %FSAX25Y25*MOIN*%

    %IR0*IPPOS*OFA0.00000B0.00000*MIA0B0*SFA1.00000B1.00000*%

    M02*

     
     
    Best Regards,
     
    Mark 

     

     

     

     

    • Post Points: 20
  • Sun, Jan 19 2014 3:16 AM

    • oldmouldy
    • Top 10 Contributor
    • Joined on Tue, Jul 15 2008
    • Woking, Surrey
    • Posts 1,382
    • Points 23,540
    Re: help with board outline gerber Reply

    It seems "pretty likely" that, whatever Class / Subclass you drew the outline on, it's was not on Board Geometry / Outline since this file contains no data, "M02*" is the "end of file" marker and the preceding contents are just control records.

    Check that you do not have any objects defined on Manufacturing>Photoplot_Outline since no Artwork data is generated for any design objects outside of the Photoplot_Outline objects, set only the Manufacturing>Photoplot_Outline colour to visible and delete all objects from that subclass. You can usually ignore getting the warning for not having any Photoplot_Outline defined.

    Also, when you import the Artwork data back into PCB Editor, you should avoid using the "database" classes and subclasses in most cases since the "database" classes and subclasses can rely on some design intelligence and the Artwork data is just collections of instructions to control a photoplotter and, as such, contain no design intelligence. A typical practice is to use Setup>Subclasses and add user defined Manufacturing Subclasses to import the Artwork data into since these will not try to impose any intelligence onto the imported data. 

    • Post Points: 20
  • Sun, Jan 19 2014 12:14 PM

    • mfris
    • Top 500 Contributor
    • Joined on Tue, Sep 18 2012
    • Durham, NC
    • Posts 20
    • Points 440
    Re: help with board outline gerber Reply
    Thanks oldmouldy,

    I did have something in Manufacturing->Photoplot_Outline - I had never deleted it from previous attempts and didn't realize that it might cause problems.  I also created a new subclass to use when pulling in the newly created outline.  One or both of those actions apparently resolved the issue I was having - I can now create board outline artwork and import/view that artwork in a separate job.

    Thanks again to you and Mike for the help both of you were able to provide.

    Best regards.
    • Post Points: 5
Page 1 of 1 (5 items)
Sort Posts:
Started by mfris at 18 Jan 2014 06:28 AM. Topic has 4 replies.