Solved: Re: 2 positions of a component in one drawing view...

mkowallik · ‎Oct 30, 2017

Is it possible with Creo to show 2 positions of e.g. a lever to show two states (open / closed) in one drawing view? I played a little bit around with mechanism but haven't rellay found a solution. Copy part position from other snapshot delivered not the desiered result.

Is it in general possible? Any ideas how?

TomD.inPDX · ‎Oct 31, 2017

Considering the core of your question defines a quantum state, no you cannot.

Can you have a view include a phantom outline for the second state, of course.

Regardless of the end result, the could mean is a lot of work depending on the complexity.

In order to get this phantom reference, you will need to do one of many tricks to obtain this.

It all depends on your pain tolerance for the level of effor required to embody a consistent means.

View solution in original post

KenFarley · ‎Oct 30, 2017

When I've needed to show this type of thing, I've added a family table entry in the assembly that has the component in both positions. Once I placed the view on the drawing, I changed the component in one or the other of the positions to be phantom transparent, or phantom opaque, depending on the situation.

Others likely will have better ways to do this, but it has worked for me.

TomU · ‎Oct 30, 2017

Yes, definitely. Move the lever to each position and take a snapshot. Make sure the snapshot is set to be visible in the drawing. Then create a drawing view with the explode state set to the snapshot name. See this link for more info: http://support.ptc.com/help/creo/creo_pma/usascii/#page/assembly%2Fasm%2Fasm_four_sub%2FTo_Make_Snap_Available_Exploded_Views_Drawing.html%23

manjunathrv · ‎Oct 31, 2017

You can also create Simplified representations and show each rep in each view.

mkowallik · ‎Oct 31, 2017

Up to now I haven't really seen the answer to my question.

In 2 different (drawing) views I'm able show it with mechasnism snapshots, family table, simpl. reps or as exploded state. No doubt about that.

But is it possible 2 states in one view (without having the part twice in the assemly --> basis for BOM)? e.g. cylinder in (dotted line) and cylinder out (as line) to indicate stroke (just as expample).

manjunathrv · ‎Oct 31, 2017

at the top of my mind I can first think that you can create a sketch curve (dotted line line style) using the outer boundary of one position and the other is the actual part...

dschenken · ‎Oct 31, 2017

Probably not. Views are of actual geometry, not speculative geometry. An item cannot be in two or more places at the same time. I suppose you could copy/paste-translate the sufaces of the part in the assembly, but I haven't tried. It should work and not add another item to the BOM.

KenFarley · ‎Oct 31, 2017

Here's another trick that might work:

Make an assembly family table that defines the component in each position.

In the drawing, create the view you want with the assembly that has the component in one of the positions.

Add an identical view that has the component in the other position.

Using the alignment tools for one of the views, align it first vertically, then horizontally with the other view. You're basically overlapping all the geometry. If the views are truly identical, it will look like a view with the component in both positions, without botching up the bill of materials.

TomD.inPDX · ‎Oct 31, 2017