Skip to main content
R
rw_011-Visitor
1-Visitor
December 29, 2015
Question

Just a question about part simplified reps and drawings.

  • December 29, 2015
  • 4 replies
  • 7654 views

Hello,

About 6 months ago I was using CREO2 .  I made about 4 parts and drawings using it.

The parts had simplified reps in them that I was able to use in the drawings.

Now we are using CREO 3.  However I need to make a fifth part and drawing.

I was able to make the simplified rep again. However when I go to the drawing and create a view it doesn't let me select a simplified rep.

It is grayed out and set to "Master".

Is there a setting I am missing .

Thanks,


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

4 replies

T
TomD.inPDX17-Peridot
17-Peridot
December 30, 2015

I'm going on memory here but did you add the simplified rep model to the drawing?

R
rw_011-VisitorAuthor
1-Visitor
December 30, 2015


Hello Antonius,


In CREO 2 I was able to create the simplified reps in the model. But it appears that CREO 3 doesn't have this function.

Reading some of the discussion on this topic gave me an idea for a work around.  I just created an extra model.

I use one model for the first sheet and the second model for second sheet of the drawings.  It too a couple of hours to figure out but my drawing will be finished today.

Thanks for replying,

RW

T
TomD.inPDX17-Peridot
17-Peridot
January 1, 2016

This is Creo 3; this dialog is the same as I remember.  As other confirmed, it all depends on what model is loaded and active.

This dialog pops up on a couple of different occasions.  Below is the "add model" dialog response.

M
mender12-Amethyst
12-Amethyst
December 31, 2015

If the part is not already in the drawing's list of models, Drawing Models > Add Model, select the part, then select the rep from the list.  If the part is in the drawing as Master Rep, and you wish to add the simp rep for use in the drawing, Drawing Models > Set Model (if the part is not the current model), then Set/Add Rep and pick the rep.  If the rep is already present, and you want to make it set current so that a new general view will be made of it, Set Model and/or Set/Add Rep.

T
TomD.inPDX17-Peridot
17-Peridot
January 1, 2016

I just noticed that if you use combined states, it also adds and activates the model automatically.

In the part model:

Each time you create a general view, you are prompted for a combined state.

If the simplified rep is not already loaded, it will be when you create the view.

Also note that it becomes the active model.

The dialog that appears to not cooperate is the view properties "edit" dialog.

These have always been limited, and in some cases logically so.

The cube on the left is the master; the one on the right is a simplified rep that removes two features.

COMBINE1 was created to use the simplified rep.  The simplified rep dialog in the UI below doesn't allow editing (Creo 2).

K
Kevin1-Visitor
1-Visitor
December 31, 2015

For parts you need to have the simplified rep you want for a view active before making the view. This goes back to early Wildfire releases or prior Pro/Engineer releases when the description was labeled Assembly Simplified Rep. Ever since Assembly was removed from the description it has caused a lot of confusion. The option was originally intended to change between Assembly Simplified Reps, the help documentation points this out. I'm not sure if PTC was working to allow this option to also switch between part simplified reps, at least I haven't seen anything that says they were. The Creo 2 Detail Drawings documentation still shows that Simplified Representation in the Drawing View>View States is used for assembly views not part views. Based on what you describe I'd say the functionality hasn't changed.

Simplified Representation.jpg

T
TomD.inPDX17-Peridot
17-Peridot
January 1, 2016

Happy New Year, Kevin.

I do not use simplified reps or combined states on a normal basis.

The fact that the Drawing View dialog should say "assembly simplified rep" gives me another avenue to explore.

It does seem that some of the assembly rep functionality in drawings should have also been ported to parts as well.

That is why I found it interesting, and useful to note that combined states is one means to add new models.

The model is a lot more forgiving about quickly making useful simplified reps and combined states.

These can be "ready made" views determined before starting the drawings.

Highly configurable parts can really benefit from this capability.

Oh well, as said before, the detailing module is pretty much what it was decades ago with new facades.

That's the main reason I won't start new projects in Creo 3.0.  I still loath to draw in Creo 3.

K
Kevin1-Visitor
1-Visitor
January 2, 2016

‌Another work around that has been used is to add the part by itself to an assembly model and create assembly simplified reps with the part reps.

I was able to determine that WF3 was when the change was made.

WF2

WF2.jpg

WF3

WF3.jpg

CREO 2, CREO 3

CREO2.jpg

    M
    mchandrashekar1-Visitor
    1-Visitor
    January 4, 2016

    Hi,

    I feel when there is a migration of data from CROE2 to CREO 3 it's always recommended to redefine your Simp reps and regenerate along with your newly created Reps.

    Later your drawing should definitely pop up the required reps to use and will never be greyed out.

    Hope this helps :-).

    Regards,

    Mohan.

    Terms & ConditionsAccessibility statement