Shrinkwrap (or other methods) for distribution to customer

[JustinSauber]

I am looking for the best method of "dumbing down" a solid model to send to customers to avoid giving away proprietary information.

Basically I need the 3D equivalent of a 2D outline dimension drawing (ODD) to send to current and prospective customers.

I have been creating shrinkwraps (save a copy ---> merged solid) and it is aggravating. Sometimes the detail is too little and others it is too much. I can never find the correct balance.

Does anyone have any pointers they can give me?

Creo 2.0

M090

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[GaryLinscheid]

Have you looked at excluding features using Simplified Reps?

[JustinSauber]

Is that possible to do at the assembly level with released sub components? We would prefer to not up the revision level just to make a simplified rep.

[GaryLinscheid]

Yes, that is an issue. You would need to create the simplified rep. at the part level so you can select it at the assembly level.

[tpartridge]

Hi Justin. By saying that sometimes the detail is too little or too much, if you mean you would like better control over what components are included in the Merged Solid, then you could try the following. This eliminates the guess-work of the automatic selection:

- in the Shrinkwrap dialog box, set the Quality level to zero

- select the arrow button for "Select Components", and select the components you want to include

- Tip: you can use Shift+select to select all the components in the Model Tree by doing the following:

- expand all assemblies that you want to include (components in collapsed assemblies will not be selected using this method)

- select the first component in the Model Tree to be included (do not pick the Assembly, but the Component)

- scroll down the Model Tree to the last component to be included; hold down Shift and select the last component (not the Assembly)

- this should select all of the components between the first and last selections.

Regards,

Terry Partridge

[WayneN]

Not sure what you mean by too much or too little detail. Could you export an iges file. I would choose solids from the export options. After saving open the iges file and select part from the dialog box. The assembly is now one part.

[JustinSauber]

By too much or too little I mean the following:

- Leaves too much proprietary data within the model basically leaving the model intact.

- Removes too much: Non-Proprietary information such as threaded holes. Which would be nice to leave in for the customer to interface with their design.

[JustinSauber]

Steven - I tried the Creo View file and the level of detail was the same as my prt file.

I need to solidify the model or make it a surface (only) model while leaving the customer interfacing connections intact.

I was able to get what I need for my current need but I will not be able to reproduce the result the next time without another trial and error session.

[David_M · Accepted solution]

Hi Justin. Do you mean you want only the external surfaces, and no internal geometry?

If you have a watertight assembly, first make your assembly into a single part (by exporting and importing as a part) then Seed-and-Boundary select the outside surfaces so that you get all of them, and copy that into a new part file. Solidify and export.

If it isn't watertight, make it watertight.