Can you save views?

[bridgel]

I was wondering if you can save the current view in Creo Parametric. For instance. I would like one view where everything is unhidden, and another view where I have a bunch of stuff hidden. I am also using sheet metal. I have a bunch of parts in the assembly that are sheetmetal and a bunch that are not. It would be great if it would also store the state of the bendings. So the one everything would be bent, while the other everything would be flattened out with stuff hidden. That would be ideal. It takes awhile to click each one and unbend it.

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[JamesBurcham]

Have you tried using simplified reps? Should should be able to create a simplified rep for each view type you want. As far as having one view showing flat states and another showing formed. I would say you need to model in both the formed and flat state as seperate parts and then create a simplified rep for each.

Here is a PTC link for simplifed reps

https://www.ptc.com/appserver/cs/view/solution.jsp?n=CS44198&posno=2&q=simplified reps&nav=ptcproductgroups||creo||Product+Group||creo

There are also several tutorials on youtube that you can reference.

[bridgel]

The assembly is comprised of other assemblies. In these, I have some of the parts grouped. This doesn't seem to be working with groups. They will never show. Am I doing something wrong?

[JamesBurcham]

In the rep creation window you should be able to expand the subassemblies and groups to select the individual parts. Without being there to see what you are doing its difficult to say what the problem might be.

[bridgel]

I seem to have messed up the groups entirely. Nothing I do will make them show. Is there some way to reset the view manager. It looks to be normal to me.

[JamesBurcham]

You should be able to just set the "master rep" to active and then create a new rep.

[bridgel]

I am getting this message when I load the design:

"All the objects which were not displayed have been erased."

Any idea what that is about. I think this is why my parts are not showing up.

[JamesBurcham]

The only time I have ever seen anything like that is when I select the "earse not displayed" button.

Not sure I can help with that one.

[bridgel]

I have no idea what happened there, but I had fortunately made a backup copy of the design so I restored to that and it is fine now. I got the simple rep to work to allow me to switch between showing or hiding parts. Now if I could get the bending/unbending to work that would be great. I do not want to have two sets of parts because then I have the chance of them getting out of sync with each other. If anyone knows of a way to store the bent state as well that would be fantastic. My current design has 9 different sheetmetal parts in the assembly. Selecting each one and unbending it is a pain.

[JamesBurcham · Accepted solution]

Create the flat as a family table instance of the bent part. Then all you ever have to edit is the bent part (generic) and the flat should update automatically.

[bridgel]

Never done that before. I will look into it. How then in the assembly can I have the two parts linking to the same other parts? How will it know which one to use? Does it just use the one currently activated and you can only have one of the family parts active at a time?

[JamesBurcham]

They will function as separate parts in an assembly. You just assemble each instance separately, no matter how many instances are in a family table. There are things you can do with programing if you want them to swap dependent on certain parameters. Or you can assemble them both and turn them on and off with simplified reps, or with programing.

I did a quick google search for part swapping in assemblies and didn't find anything useful, but I'm sure if you search the PTC support or even the help system in Creo you can find something.

[gkoch]

If you manage to assemble the sheetmetal parts using only references that stay as they are during unbend, then you may also use an assembly family table and use it to replace the bend with unbend part instances.

But if you need different constraints/orientation/location for bend and unbend versions of the parts, then this will not be an option and James' suggestion seems to be your best bet.

[TomD.inPDX]

Creo 2.0 Sheetmetal - Simplified Reps for flat pattern drawings

[TomD.inPDX]

Remember that you can add multiple models to the drawing including family table instances. So you can have the flat pattern parts included as single parts for independent views. You can also make a reference assembly that has multiple flat part representations that is only used in the drawing. This too would maintain associativity.

[bridgel]

This is great. Works wonderfully and I can make all kinds of variants to show off different aspects.