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mwesselski1-Visitor
1-Visitor
June 8, 2016
Solved

Replacing Model in Drawing

  • June 8, 2016
  • 13 replies
  • 79217 views

I have a drawing which I copied and renamed.   We are currently creating a development drawing and then later a production drawing in which we use a different drawing number.     I want to replace the model in which the views are created from with an identical model assembly with a slightly different part number.  I've tried the "Drawing Models" commands and I've added the model, so it shows up in my list of models.  I've tried to use "Replace" but it doesn't seem to work.   How would I go about doing this and preserving my views and dimensions, etc.?   Thanks

Best answer by cgorni

To close this community thread on the ability to Replace Model in Drawing.

 

Summary of the proposed solutions, also detailed in article CS109945 :

 

  • For existing models:
    • Only Family Table instances can be used with Drawing Models > Replace command from Layout tab of the ribbon.
    • Starting with Creo 4.0 it is also possible to Replace View Model (and their dependent views) with Family Table but also Simplified Representation or Reference Model (such as Merge or Inheritance). See Creo Help center here
    • The workaround of replacing the drawing model at system level (renaming the unrelated model to the drawing model one on disk) is sometimes used, but is strongly discouraged for data integrity.

 

  • To derive new models:
    • You can use File > Save As > Save a Copy of the model after setting the config.pro option rename_drawings_with_object to both, the model and the drawing MUST have the same name. Then act on the copies.
    • You could also use File > Save As > Save a Backup and then File > Manage File > Rename to change both model and drawing names, be cautious which objects are in session when performing the Rename operation.
    • Above methods are preferred. However some users create temporary Family Table instances, replacing the drawing model with them and, while keeping the instances in session, delete the Family Table before saving anything. The goal is to make them standalone objects and get rid of the generic reference before saving the new objects.
    • If using a PDM or PLM system (like Windchill) it may be easier to collect and copy / rename the dependent objects in the Commonspace or Workspace.

13 replies

M
mender12-Amethyst
12-Amethyst
June 8, 2016

You could take the original drawing and original assembly, and produce the new drawing + assembly with Rename.  If you don't do something like that, you have an assembly that you say is identical, but to Creo it looks unrelated, and replace -type functionality will be unavailable or strip out any references, or if you try to cheat the system, you could end up with references that are to the wrong type of item entirely (for example, information on a shown axis, but when you look it up in the part, it's an edge made by a cross-section).  That can cause all sorts of trouble, so don't try to cheat it.  Instead, copy both the drawing and the assembly so you have newdrawing of newassembly, and then you're set.

D
dschenken1-Visitor
1-Visitor
June 9, 2016

This is really an area with no reliable answers. The tools to repair unlinked items just don't exist. And it is really a big problem if PDM is involved.

I have resorted to a side-step to get the correct names et al for assemblies and drawings to avoid repeating thousands of mouse-clicks to put items back to where they started when low-level parts are to be replaced in an assembly structure that is multiple levels deep.

In my case, both the original and the new name drawings must be maintained as the existing ones are in production and the new ones need to go through the release process. Common changes require double work, but that's how it goes.

D
dgschaefer21-Topaz II
21-Topaz II
June 8, 2016

The replace command in the drawing only works for family table driven models, as far as I know.  It won't work on models that are copies of each other.

Another issue you'll have is that by default Creo stores some of the drawing info (created dims for one) in the model file rather than the drawing file.  So, by swapping models you'll lose some of the dimension info.

You can trick Creo into using the new model by saving a copy of the drawing to an empty folder, saving a copy of the alternate model into that folder and then manually renaming to the original model name.  When you open the drawing Creo will find the old model name and use it for the drawing, but it's pretty likely that a lot if things will either be missing or wrong.


The best path is to put off the creating of the production copy as long as possible so you have the most "mature' development model possible.  Then you use the backup command to create a copy of the drawing and all models in a new folder.  Then, starting from a fresh Creo session, open the new copy and rename the drawing and model(s) accordingly.  You can then use the backup command to put it back in the main folder.

It's important that you fully understand how Creo retrieves files and what happens when you use the backup command as it's pretty easy to mess things up if you don't  All that assumes you are not using a PDM system, if you are, much of that should be done within the system.  I'm not familiar with PDMLink to give you directions on that.

Another path would be to not make a copy but instead just transition your development model into production, but I assume that your company policy prohibits that.

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dgschaefer21-Topaz II
21-Topaz II
June 8, 2016

A colleague points out an obvious answer I missed.

If you open your model (part or assy) and if the drawing and the model have the exact same name and you have the config option "rename_drawings_with_object" set to "both" (it defaults to "none") and save it to a new name, then Creo creates a new copy of the assy with a new copy of the drawing both with the new name you supply.

J
jthakor1-Visitor
1-Visitor
June 10, 2016

Hi,

You can add drawing in new sheet with insert--> import drawing/data, where you will get new model & drawing. Once you are complete then you can delete first sheet and associated model. I think it might help you..

Thanks,

Jitu

J
jme1-Visitor
1-Visitor
June 10, 2016

yup ran into the same issue was forced to -recreate the drawing with a similar part.. pathetic,.. in SWX you can easily do this.. the dim's  need some cleaning up but you don't have to start from scratch

    C
    cmoreno1-Visitor
    1-Visitor
    July 20, 2020

    As usual it feels like insanity when you're working in Creo and try to do something that is basic functionality in SWX and creo offers no solutions. I'm adding it to my list of things swx can do that creo can't.

      B
      23-Emerald III
      BenLoosli23-Emerald III
      23-Emerald III
      July 21, 2020

      Be sure to keep a list of things that Creo CAN do that SWX can't, too!

        K
        Kevin1-Visitor
        1-Visitor
        June 10, 2016

        If you are allowed to do it, create a family table so you can use replace. If things are similar when you use replace any features that have dimensions should keep their references. If features are removed the dimension should turn purple. If you leave the dimensions on the drawing and replace the model with an instance where the features are present the dimensions should regain the references. There shouldn't be a need to start completely over but it may depend on company practices.

          J
          jme1-Visitor
          1-Visitor
          June 10, 2016

          So do I have to plan ahead if I want to replace one similar model with another.. Is it straightforward or more of the unintuitive/ convolute setup?

          K
          Kevin1-Visitor
          1-Visitor
          June 13, 2016

          Depends on what you are trying to accomplish and how you view it. If you are wanting something that stands by itself you may just need to copy the model and drawing the similar part is based off and modify from there. If you want a connection between the base and similar parts then a family table is needed. You copy the drawing of the base part and use replace in the new drawing to specify the new instance. Shown or created dimensions that are the same between the two instances should remain on the new drawing and you should only need to create or show new ones. Either way things aren't being created from scratch but you may need to provided more info about what you were actually doing and why you needed to start from scratch. Just based on the description(s) I'm not seeing anything that would cause you to have to do that.

            J
            Jose_Costa12-Amethyst
            12-Amethyst
            July 19, 2016

            You can try this Macro:

            J
            jdonovan-21-Visitor
            1-Visitor
            January 25, 2018

            For the life of me I can't understand how PTC creo/proe etc etc can be so bad!  I thought PTC was one of the pioneers of 3-d parametric modeling/drawing etc ..... They have really dropped the ball; this program is so much more difficult to get anything done .... Solidworks is much easier.  I am being forced to use Creo2 now so I read these PTC forums and I keep seeing things like " if you want to get that done you need to stick your elbow in your ear and place your knee behind your back and then do these mouse clicks etc etc"  and hope it works; and it might not work this way if you are using windchill etc etc" ..... it's so frustrating 

              D
              DaveMartin16-Pearl
              16-Pearl
              January 26, 2018

              Then go work for a company that uses SolidWorks.

                J
                jhaston-31-Visitor
                1-Visitor
                January 31, 2018

                Your question/thread was inadvertently highjacked!

                 

                I'd stick with @Kevin on this one. He's definitely pointing you in the right direction.

                 

                @dgschaefer has also pointed out that "The replace command in the drawing only works for family table driven models". This is true.

                 

                I
                ibml_team1-Visitor
                1-Visitor
                March 27, 2018

                I had spoken to PTC directly at a previous job a few yr ago when they 1st rolled out Creo 1.0, we brought up a few issues regarding drawings and this was one of them, i saw very little change in Creo 2.0. For the past year I was on SolidWorks but I am back home in Creo 3.0 M070. I am currently in the same predicament as i need to replace a model bc i need to prototype it and they need drawings so i want to use an old release drawing. I found this video from PTC, but it doesn't have the release or date code. Anyone has a clue what is going on? because this is exactly what we all need. In the mean time i'll go back to coping the old drawing and part, renaming them, copy or model features and add a few dimension in drawing...

                 

                https://www.youtube.com/watch?v=BW66ZBEtdVw

                D
                dschenken1-Visitor
                1-Visitor
                March 27, 2018

                They are replacing a family table instance with another instance from the same family table.

                  I
                  ibml_team1-Visitor
                  1-Visitor
                  March 27, 2018

                  i expanded the video to full screen and can see it... bummer

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