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banderson-21-Visitor
1-Visitor
February 27, 2014
Solved

help on copy paste options in creo 2.0

  • February 27, 2014
  • 15 replies
  • 12330 views

We just switched from Wildfire 4 to Creo 2.0.

The copy paste functionality in assemblies has changed a bit with dependancies of parts when you copy more than one at a time. An example of something that I do regularily is a bolt and nut combination. A lot of times Patterns aren't the best option, and I generally don't like patterns a whole lot anyways.

Old (desired) way:

What I would do it constrain the bolt, and then constrain the nut to only the bolt for the first pair. Then to copy the same pair I to a different hole, I would select both the bolt and the nut, hit ctrl-c and then ctrl-v. The paste/place component of the bolt would show up and I would set the constraints and then hit OK. The nut would keep the same constraints onto the bolt and I would just hit ok.

New way:

Creo makes me define every constraint of both the bolt and the nut, irregardless of how I have them constrained in the copied components.

I'm sure that there are options to define this behavior, but I am having trouble interpreting the cryptic option list that is the configuration file.

Anyone willing to help me figure out what options are available to set this up?

Thanks

    Best answer by banderson-2

    Ok, I found a solution to get the copy and paste work like it used to. You have to set a hidden config.pro option.

    This came from the PTC help tickets.

    Set hidden config.pro option use_temp_interface_for_paste no

    https://www.ptc.com/appserver/cs/view/solution.jsp?n=CS7786&posno=3&q=copy%20and%20paste%20group&nav=ptcproductgroups||creo||Product%20Group||Creo

    Gotta love it, they change something that isn't broken........again.

    15 replies

    A
    akrenzer1-Visitor
    1-Visitor
    February 27, 2014

    Why not use the repeat command? It will allow you to choose which constraint you want, or any combination of constraints.You can place numerous parts in seconds.

    B
    banderson-21-VisitorAuthor
    1-Visitor
    February 27, 2014

    I'll have to try that. Can it do multiple groups of components?

    A
    akrenzer1-Visitor
    1-Visitor
    February 27, 2014

    No, just one compnent at a time, but it is very quick.

    T
    TomD.inPDX17-Peridot
    17-Peridot
    February 27, 2014

    Try this option in config.pro:

    create_temp_interfaces yes

    This creates an interface feature for the 1st assembled part so that subsequent parts will follow the same inputs. This means that if you place a bolt by axis and surface, subsequent assembly of this part will only request the assembly's reference and not the component so all you need to pick is the axes and surface you want to mate to.

    You can overwrite this behavior during placement.

    Using pattern relation is nice, but only when they work reliably.

    B
    banderson-21-VisitorAuthor
    1-Visitor
    February 27, 2014

    Would that mean that every other engineer in my company that pulls up that bolt would get that same interface? Or is is temporary?

    T
    TomD.inPDX17-Peridot
    17-Peridot
    February 27, 2014

    The reference seems to stay with that assembly, not the part you are installing.

    A
    akrenzer1-Visitor
    1-Visitor
    February 28, 2014

    If you all use the same screw as a library part, you can add an interface to that screw, so it would be the same placement prompt for every user, every time.

    B
    banderson-21-VisitorAuthor
    1-Visitor
    March 3, 2014

    Yeah, one of the guys tried to do that (made sense to me) but some of the other engineers didn't like it, so we don't want the interface on the regular part.

    B
    banderson-21-VisitorAuthor
    1-Visitor
    March 7, 2014

    So I've tried the repeat command and it works really well for what it was designed to do, repeat a single component. It, however, does not handle multiple components. An example would be a wheel, hub, spindle group with all of the hardware. I used to have to select the parts I wanted to copy, copy, then paste , and only have to select the constraints from where the the spindle meets it's hinge. Now I have the re-click for every component in the assembly which can be very difficult to remember all of the exact same steps.

    Does anyone else have any suggestions on how to get it to work like it used to?

    D
    dschenken1-Visitor
    1-Visitor
    March 7, 2014

    Have you tried grouping the items before copying?

    B
    banderson-21-VisitorAuthor
    1-Visitor
    March 10, 2014

    yes. Grouping doesn't make a difference.

    B
    banderson-21-VisitorAuthorAnswer
    1-Visitor
    March 10, 2014

    Ok, I found a solution to get the copy and paste work like it used to. You have to set a hidden config.pro option.

    This came from the PTC help tickets.

    Set hidden config.pro option use_temp_interface_for_paste no

    https://www.ptc.com/appserver/cs/view/solution.jsp?n=CS7786&posno=3&q=copy%20and%20paste%20group&nav=ptcproductgroups||creo||Product%20Group||Creo

    Gotta love it, they change something that isn't broken........again.

      P
      ptc-48798801-Visitor
      1-Visitor
      March 17, 2015

      Haha it works.tks.

      D
      dgschaefer21-Topaz II
      21-Topaz II
      March 17, 2015

      I know you've got your answer, but have you tried copy > paste special > advanced reference configuration? This is an incredibly powerful tool that I use all the time for features and components.

      When you use advanced reference configuration, a dialog comes up showing all the refs used to place the items you are pasting. In this case, it should only show the references for the bolt.

        K
        Kirkholm1-Visitor
        1-Visitor
        February 22, 2018

        Creo 3, not sure if this makes a difference, but there is another way.

         

        If the components are mated to each other with few mates to the other parts/assemblies:

        1. Group the wanted components
        2. "Ctrl + C"
        3. Right click the window (long)
        4. "Paste options" and "Paste special"
        5. Tick mark the "Advanced reference configuration" box
        6. Choose the references in the assembly

        This is done each time the group needs to be copied. Please name the groups accordingly.

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