Create a Shrinkwrap Feature in Creo for a Better Large Assembly Performance




A “shrinkwrap” collects and copies surface data from an assembly into a single, lightweight feature. With shrinkwrap features, much of the internal detail is excluded, so you can also use it to protect your intellectual property when you share an assembly. Plus, if you struggle with downloading and manipulating large assemblies (see the video below), shrinkwrapped features provide one way to make large assemblies  more manageable. Here’s what you need to know to get started

Create a New Part in the Assembly

Before you create a shrinkwrap feature, create a new part in the assembly. Follow these steps:

  1. In an open assembly, click Create. The Create Component dialog box opens.

  2. Select Part and Solid.

  3. Accept the default name (in the demo below, this is PRT0001) or enter a new name, and click OK. The Creation Options dialog box opens.

  4. Click Browse, and click OK. You are now working as though the new model is the active model. The Choose Template dialog opens.

  5. Double-click a start part, click Open, and then OK.

  6. Right-click in the graphics area, click Default constraint > Complete Component.

Create a Shrinkwrap Feature

To create the shrinkwrap feature, follow these steps:

  1. In the Model Tree, right-click the part you created, and then click Activate.

  2. Click Shrinkwrap. The Shrinkwrap tab opens with the top-level assembly as the reference model.

  3. In the dashboard, select the Subset button to choose your collection method. Click Outer Shell to create a shrinkwrap of the exterior shape of the model. You can learn about other methods (such as autocollecting all solid surfaces or manually collecting surfaces) in the video below or on this help page.

  4. In the Shrinkwrap Comps dialog, click any parts you want to exclude from shrinkwrap consideration to highlight them. Right-click and select Ignore. Then click OK.

Shrinkwrap component chooser

  1. In the dashboard, click References and select additional shrinkwrap references to always include or exclude.

  2. In the dashboard, click Options to define shrinkwrap settings as follows:

    • In the Subset options area, select Exclude then Shrinkwrap. The system will base the Shrinkwrap only on the selected components (used with subsets).
    • In the Quality area, in the Level field, type a value (1–10) for the shrinkwrap quality level. The default setting is 1. The higher the quality, the longer the processing time.
    • In the Attributes area, select Auto Hole Filling. The system will fill all holes or cuts that intersect a single surface.
    • In the Attributes area, select Ignore Small Surfaces. The system will exclude surfaces smaller than the specified value (percentage of the model’s size). Type a whole number (0 is the default) in the Threshold as percentage of model size box to specify the relative size of the surface to be ignored.
  3. Then click the green check to complete.

Shrinkwrap Options dialog

PTC University has an online tutorial to show you how it works. An instructor shows you how to create a new part and create a shrinkwrap feature using outer shell collection (as described above).

You’ll also see how to open and observe your feature, add a shrinkwrap feature by autocollect all solid surfaces, and update a shrinkwrap when the source model changes.

Click the video below to view the tutorial for free; no login needed. If you’d like to see more, I’d recommend a visit to PTC University Learning Exchange. You’ll need to create an account—but it’s free and there are 700 more PTC tutorials just like this one waiting to show you how to use Creo effectively.

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