Just a question about part simplified reps and drawings.

[rw]

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,

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[TomD.inPDX]

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

[rw]

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

[TomD.inPDX]

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.

[mender]

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.

[TomD.inPDX]

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).

[Kevin]

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.

[TomD.inPDX]

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.

[Kevin]

‌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

WF3

CREO 2, CREO 3

[TomD.inPDX]

Funny; enough room to label it twice but not enough room to be clear

[mchandrashekar]

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.