Home > Community > Forums > PCB Design > Creating symbol package 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 symbol package in PCB Editor 

Last post Sun, Nov 28 2010 1:07 PM by aneter. 5 replies.
Started by Olek 19 Feb 2009 08:41 AM. Topic has 5 replies and 4178 views
Page 1 of 1 (6 items)
Sort Posts:
  • Thu, Feb 19 2009 8:41 AM

    • Olek
    • Not Ranked
    • Joined on Mon, Sep 22 2008
    • Posts 9
    • Points 210
    Creating symbol package in PCB Editor Reply

    Where symbol package (footprint) origin (datum) should be placed?

    I decided to be consistent and I place it always at pin 1 of the footprint for both through hole and SMD footprints.

     Is it the best location?

    I understand that the origin location matters when selecting or moving footprint on a board.

    How footprint origin location effects generation of pick and place machine coordinates?

    Does origin location matters in this case?

    • Post Points: 20
  • Thu, Feb 19 2009 10:12 AM

    • mcatramb91
    • Top 75 Contributor
    • Joined on Thu, Jan 3 2013
    • Chelmsford, MA
    • Posts 101
    • Points 4,995
    Re: Creating symbol package in PCB Editor Reply

    Hello,

    Using Pin 1 for the symbol origin on Thru Components is normally a good thing to do but I would recommend using the centroid or center point for SMD Components. Certainly, being consistent is always the best way to go.

    For the most part the origin location doesn't really matter too much in regards to the Pick and Place machine coordinates.  The body center information is driven by the calculated center point of the shape defined on Package Geometry > Place_Bound_Top but this can be overriden by defining the component centroid using Package Geometry > Body_Center, normally by adding a text sting like a period "," at the desired center point.  This will give you a consistent location vs. a calcuated one for your pick and place centroid point and it can be easily extracted to generate Pick and Place data.

    Hope this helps,
    Mike Catrambone

    • Post Points: 20
  • Fri, Feb 20 2009 8:07 AM

    • Olek
    • Not Ranked
    • Joined on Mon, Sep 22 2008
    • Posts 9
    • Points 210
    Re: Creating symbol package in PCB Editor Reply
    I use OrCAD PCB Editor currently.Unfortunately, this software doesn’t have any tool that allows for automatic placement  of package origin at the geometrical center of the component.(For example OrCAD Layout, that I used previously, allows for automatic placement of “insertion” origin in the geometrical centre of the footprint (with respect to the pads)).The easiest, (and fastest) way of  placing the origin, using PCB Editor is to place it  at pin #1 of the footprint. (This method provides consistency also).Also, when translating footprints from OrCAD Layout to PCB Editor, the origin is placed at pin #1. (My OrCAD Layout footprints have “datum” placed at pin #1 and “insertion origin” at the center of the footprint.)

    Placing manually an origin at the geometrical center (in respect of the pads) may be very difficult and not practical in case of some asymmetrical components (using PCB Editor).
     

    Because of that, I prefer to place PCB Editor SMD footprints origin at their pin #1.
     

    My concern is if SMD footprints origins defined in such way (placed at pin #1) may present any problems to assembly shops.
     They prefer probably  placement file that provides coordinates of the geometrical center of the components rather than pin #1 of the components.However, I think, that pick and place machine software allows for easy origin location modification, so it shouldn’t be a problem.Am I correct?
    • Post Points: 20
  • Fri, Feb 20 2009 8:56 AM

    • mcatramb91
    • Top 75 Contributor
    • Joined on Thu, Jan 3 2013
    • Chelmsford, MA
    • Posts 101
    • Points 4,995
    Re: Creating symbol package in PCB Editor Reply

    Hello,

    I am not familiar with Orcad Layout but I believe OrCAD PCB Editor is very similar to Allegro PCB Editor so everything I provided so far is how I have done it inside Allegro PCB Editor.

    Its really up to you as far as where the symbol origin is placed. There is some Allegro SKILL Code on Sourcelink that will automatically generate the Body Center for you but I have never used it to give any other further guidance nor do I know if it will run inside of OrCAD PCB Editor.

    As far as the Assembly shops placement file, it is best that the placement data does not need any modification or maybe just slight modifications. From past experiences with other companies, clean placement data will make the whole process go much faster and prevents any mistakes that may cost you extra time and money. 

    You have the ability to output generic placement data from the File menu (File > Export > Placement) and specify whether the data is driven by Symbol Origin, Body Center or Pin 1.  Selecting Body Center will use the data provided on Package Geometry > Body_Center first and if it is not present it will calculate the Body Center using the Place_Bound_Top Shape.

    Hope this helps,
    Mike Catrambone

    • Post Points: 20
  • Fri, Feb 20 2009 9:53 AM

    • Olek
    • Not Ranked
    • Joined on Mon, Sep 22 2008
    • Posts 9
    • Points 210
    RE: Creating symbol package in PCB Editor Reply
    Thank you,
     
    Aleksander
    • Post Points: 5
  • Sun, Nov 28 2010 1:07 PM

    • aneter
    • Not Ranked
    • Joined on Fri, Sep 24 2010
    • Posts 2
    • Points 25
    Re: Creating symbol package in PCB Editor Reply
    Grazie!!!! (thankyou)
    • Post Points: 5
Page 1 of 1 (6 items)
Sort Posts:
Started by Olek at 19 Feb 2009 08:41 AM. Topic has 5 replies.