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: *

 Gerbers 

Last post Thu, Apr 4 2013 12:53 AM by oldmouldy. 3 replies.
Started by Bob M 02 Apr 2013 06:30 PM. Topic has 3 replies and 585 views
Page 1 of 1 (4 items)
Sort Posts:
  • Tue, Apr 2 2013 6:30 PM

    • Bob M
    • Not Ranked
    • Joined on Wed, Feb 27 2013
    • Posts 2
    • Points 40
    Gerbers Reply

    Sorry for the low level post but I am a new OrCAD user and it's a very difficult tool to come up to speed on. I'm highly proficient in Altium and PADS but I can't believe how hard they make it to use this tool. Here are my current issues:

    1) In putting down a polygon I'm expecting to see thermal relief connections to pads of the same nets, instead of thermal relief I only see the pads being connected to the net. 

    2) I created gerbers at Manufacture>Artwork>Create Artwork but all I get is Top, Bottom and Inner1 (GND) layers, no Silkscreen, Soldermask, Solderpaste, Drill Drawing or Board Outline.

    3) I have about 200 vias assigned to GND and I should certainly expect to see thermal relief connections to the GND layer for them but I don't.

    These things are probably easy for everyone but tediously difficult to learn for new users and I gotta send out gerbers. Is there anyone willing to help?

    Thanks in advance.

    • Post Points: 20
  • Wed, Apr 3 2013 12:49 AM

    • oldmouldy
    • Top 10 Contributor
    • Joined on Tue, Jul 15 2008
    • Woking, Surrey
    • Posts 1,440
    • Points 24,520
    Re: Gerbers Reply

    The Polygon needs to be a shape, the shape needs to be Dynamic, the pins need to be pins not vias.

    You need to create the "other" films for output, open Manufacture>Artwork, Film Control tab, leave this open, set the colours in Display>Color/Visibility for the required Film details to on, for example, only turn on all the Silkscreen_Top colours, back in the Film Control tab, right-click>Add on an existing film name entry and give the new Film a name, the Film definition contents will match the dispalyed objects. There is also a right-click>Match Display if you need to change the contents.

    Vias are Full Contact by default, since they are unlikely to be soldered to, thermal relief would not usually be a requirement. You can set the Thermal Relief type globally, Shape>Global Dynamic Parameters, Thermal Relief Connects tab, or for each individual shape, select the shape and right-click>Parameters, Thermal Relief Connects tab.

    • Post Points: 20
  • Wed, Apr 3 2013 10:10 AM

    • Bob M
    • Not Ranked
    • Joined on Wed, Feb 27 2013
    • Posts 2
    • Points 40
    Re: Gerbers Reply

    Thank you for the input, it's really helpful.

    The only part of the above is about the artwork. I'm not sure if it matters that I'm using PCB Deigner 16.6 but in Artwork the tab is named Create Missing Films and it's greyed out. So in Display>Color/Visibility I have everything enabled and yet I can't seem to create the other films. Any idea why?

    • Post Points: 20
  • Thu, Apr 4 2013 12:53 AM

    • oldmouldy
    • Top 10 Contributor
    • Joined on Tue, Jul 15 2008
    • Woking, Surrey
    • Posts 1,440
    • Points 24,520
    Re: Gerbers Reply
    Any PCB Editor looks after the Etch layers automatically, if the Cross Section gets changed after Artwork generation, there may be some missing Etch Films, that is what the button is about, since you likely have not changed the board cross-section, the button remains disabled. You, the user, are going to need to create the "other" Film Control records to generate the required Gerber output from the data that you have defined. Refer to this document on Preparing Manufacturing Data, algroman.pdf in the doc\algroman directory of the installation. You probably want to ensure that the Shape>Void Controls and Manufacture>Artwork parameters are both set to RS274X
    • Post Points: 5
Page 1 of 1 (4 items)
Sort Posts:
Started by Bob M at 02 Apr 2013 06:30 PM. Topic has 3 replies.