Creo Elements/Direct Modeling allows you to cut specified faces or recognized features from a part while keeping a valid solid model. You have a high degree of flexibility in modifying parts without needing to specify precise machining operations.
When cutting faces or recognized features, Creo Elements/Direct Modeling removes the faces and their edges. It also reconnects those edges which have identical geometry.
You have the option to keep the cut faces or features as a named tool. The new tool, a face part, can then be positioned, modified, and copied as usual. If you do not keep the part, Cut deletes it.
You can also specify that blends be kept on the part from which faces or features are cut. The Redo Blend option first suppresses any blends touching the cut faces or features, and then replaces them on the original part. This option is important for dealing with freeform blends, which may not otherwise be repairable.
The graphic below shows an example of cutting a boss (1). (Please note that the boss is not a recognized feature.) The neighboring edges can be reconnected because they have identical geometry.
To cut a face or feature,
1. Click Modeling and then, in the Modify 3D group, click Cut. The Cut Faces dialog box opens.
2. Select the face(s) or feature(s) to cut:
◦ Click Faces, then click on a face to cut. Hold the Shift key to select multiple faces.
◦ Click Rec.Feat, then select the feature in the Viewport. Hold the Shift key to select multiple features. You can select from the following options:
▪ Feat Select allows you to choose from the type of feature to select.
▪ Allow Face Splitting automatically splits faces if necessary to select the entire feature.
▪ Automatic selects the boss/pocket, rib, or slot with the smallest number of faces.
3. Set the following options:
◦ Keep Tool: Select if you want to keep the cut faces or features as a named tool. The new tool, a face part, can be positioned, modified, and copied.
◦ Redo Blend: Allow the operation to make automatic adjustments to blends.
◦ Chk & Fix: Use when you suspect a part is corrupt. Chk & Fix checks for self-intersections, knife edges, and void shells and attempts to fix them. If a part fails the check and fix, it is not modified and remains in its original state.
4. Click Next to finish the current operation and cut another face or recognized feature.
5. Click to complete the operation.
Limitations
• When cutting faces, you must select a group of faces which together represent material in the form of a boss, pocket, or hole.
• It must be possible for Creo Elements/Direct Modeling to repair the part by closing the face or growing the edges.
• Cut will fail if it requires the creation of a new face.
• Multiple solutions are not possible.
• The generated tool part must be new or must have been previously empty.
• Cutting a feature depends upon the recognition of the feature by the system or by the user defining it. Cutting a feature may result in a change to underlying features.
• If you select the Redo Blend option, the system will attempt to recreate the blend with the same blending options. However, in some situations that may not be possible. If the blend was created with the RollAtSharp or RollAtSmooth options, the blend may be recreated without those options.
Cut. The Cut Faces dialog box opens.
to complete the operation.