Home > Community > Forums > PCB Design > How can I preserve designators from changes?

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: *

 How can I preserve designators from changes? 

Last post Tue, Apr 29 2014 10:29 AM by bradenmarr. 8 replies.
Started by 09127751201 24 Nov 2013 06:41 PM. Topic has 8 replies and 866 views
Page 1 of 1 (9 items)
Sort Posts:
  • Sun, Nov 24 2013 6:41 PM

    How can I preserve designators from changes? Reply

    Hi
    In the Orcad capture schematic environment when we try to copy a page in a project file and paste it into an another project all designators automatically changes.
    How can I preserve them from changes?
    It is important to me to save all designators without changes.
    Thanks a lot

    • Post Points: 20
  • Mon, Nov 25 2013 3:00 AM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,243
    • Points 20,215
    Re: How can I preserve designators from changes? Reply

    Go to Options - Preferences - Miscellaneous tab and check the box for Preserve Reference on Copy.

    • Post Points: 20
  • Mon, Nov 25 2013 9:23 AM

    Re: How can I preserve designators from changes? Reply

    steve:
    Go to Options - Preferences - Miscellaneous tab and check the box for Preserve Reference on Copy.
     

    Thank you for your answer. It was a good idea , but according to the product help this option is not supported for complex hierarchical design. I tested that option in a complex hierarchical design , all designators changed to “?” sign after paste action , for example U1A to U?A, but in a flat design it worked properly and all designators remained without change.

    unfortunately all my designs are complex hierarchical design.Do  you have a better solution for complex hierarchical designs?

    • Post Points: 35
  • Mon, Nov 25 2013 12:17 PM

    • oldmouldy
    • Top 10 Contributor
    • Joined on Tue, Jul 15 2008
    • Woking, Surrey
    • Posts 1,445
    • Points 24,590
    Re: How can I preserve designators from changes? Reply

    In a complex hierarchical design, Capture has one schematic and "n" sets of properties for the parts, if you copy a part, which of the "n" sets of properties to copy? No simple answer so, as things stand, no simple solution. And, for a PCB Design you need to get to unique references, so what real purpose to preserving the reference?

    • Post Points: 20
  • Mon, Nov 25 2013 6:30 PM

    Re: How can I preserve designators from changes? Reply

     

    oldmouldy:
    if you copy a part, which of the "n" sets of properties to copy?

    I agree with you. It has no simple answer. In this condition if you have a “brd” file (PCB File) based on a complex hierarchical design , if you copy these files (including Schematic and PCB files) to another project you will lose designator synchronization between schematic files and PCB file.

    • Post Points: 20
  • Tue, Nov 26 2013 1:29 AM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,243
    • Points 20,215
    Re: How can I preserve designators from changes? Reply

    You will not lose the designator information unless you re-annotate the schematic. If you need to copy the whole project either do it in Windows Explorer or in 16.6 use File - Project Save as.

    • Post Points: 5
  • Mon, Apr 28 2014 5:41 PM

    • bradenmarr
    • Not Ranked
    • Joined on Fri, Jan 18 2013
    • Posts 3
    • Points 45
    Re: How can I preserve designators from changes? Reply

    I have a similar problem, except that I am using a flat design (not heirarchical), and I am using OrCAD 16.6-S001.

    The Options->Preferences->Miscellaneous->Automatically reference placed parts is unchecked/disabled, and Preserve reference on copy is checked/enabled.

    When I try to copy entire pages from Capture project A to project B (both flat designs), the reference designators are reassigned to ?. When I try to copy one or more component symbols from project A to project B, the reference designators are reassigned to the next logical unused reference designators for project B.

    OrCAD is behaving like it is either operating on a heirarchical design, or something else is preventing the preservation of reference designators, such as perhaps I don't have another setting defined properly, or don't understand a concept that I thought I understood.

    I realize I have not got the most recent service patch for OrCAD, so perhaps this is a bug that is now fixed?

    I am unable to progress unless, I suppose, make a copy of design A that I wish to have the designators preserved in and copy paste over the design B that can have its reference designators reassigned, and then save it as design B. Any thoughts? Thanks.

    • Post Points: 20
  • Tue, Apr 29 2014 4:12 AM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,243
    • Points 20,215
    Re: How can I preserve designators from changes? Reply

     What mode is the design in Instances or Occurrences ? I would also say I've just tried this using S027 (latest hotfix) and it works as expected so get to the latest hotfix if you can.

    • Post Points: 20
  • Tue, Apr 29 2014 10:29 AM

    • bradenmarr
    • Not Ranked
    • Joined on Fri, Jan 18 2013
    • Posts 3
    • Points 45
    Re: How can I preserve designators from changes? Reply

    Thanks for putting a lightbulb over my head, steve!

    Using your hint about Instances and Occurrences, I found this blog page:

    http://www.cadence.com/Community/blogs/pcb/archive/2013/05/02/customer-support-recommended-understanding-instance-and-occurrence-modes-of-design-annotation-using-allegro-design-entry-cis.aspx?postID=1323133

    and on project A pushed all occurrence properties to instance properties by doing,

    1. Select the .DSN in the project tree (for project A)

    2. Accessories->Transfer Occ. Prop. to Instance->Push Occ. Prop. into Instance and in the dialog box chose the first option, "This option will push the occurrence level values of the part reference and PCB footprint properties as instance level values." and checkboxed the "Use this to remove all the Occurrence properties from the design and change the preferred mode of your design to instances"

    This generated a report of all components changed, and though it noted that each affected component's reference designator was being changed to ?, it correctly preserved the reference designation on each schematic page. (I haven't yet checked to see if other properties were preserved in this conversion.)

    I was then able to select the pages from project A, copy, and paste them into to project B and the reference designators were preserved on copy! :-)

    I'm not sure why some components were "occurrences", but perhaps this could have happened when editing the schematic with copy paste commands, pasting from other schematics outside of project B, or properties were edited (such as our custom "Populate" property that is either blank/invisible or "DNP"/visible), or perhaps the components added to the schematic from CIS were somehow altered. Now I know that a "flat" design, while it is being created and edited, can somehow spontaneously begin to contain components with modes that are otherwise normally expected for a heirarchical design.

    • Post Points: 5
Page 1 of 1 (9 items)
Sort Posts:
Started by 09127751201 at 24 Nov 2013 06:41 PM. Topic has 8 replies.