Step-by-Step Recognition

You can recognize some imported body features from a part, save the part, then recognize more features from the same imported body at a later time. You can also recognize features of partially recognized parts (parts that contain imported bodies and recognized features). You can save the partially recognized document to preserve its various stages of recognition. Step-by-step recognition is supported by automatic and interactive feature recognition or by a combination of these methods.

• Step-by-step recognition is available for multibody parts or parts with sheet metal features.

• Feature names before recognition are not retained after recognition. For example, a hole feature named DHole-50 before recognition is renamed to Hole1 after recognition if it is the first recognized hole.

• The Find Patterns, Combine Features, and Re-Recognize commands are available only for the features currently displayed under Recognized Features in the Intermediate Stage PropertyManager. You cannot run these commands on previously existing features.

If a part contains an imported body and any of the following features, FeatureWorks can recognize these features:

• Base flanges

• Sketched bends

• Chamfers, including face chamfers

• Drafts

• Boss and cut extrudes

• Fillets, including face and full round fillets

• Edge flanges

• Hem flanges

• Miter flanges

• Hole Wizard holes (all standards for all types of Hole Wizard holes.

• Base lofts

• Patterns, including circular, linear, mirror, and sketch driven

• Boss and cut revolves

• Revolves without a centerline

• Ribs

• Shells

• Boss and cut sweeps (without guide curves)

• Boss and cut thickens

To recognize imported body features using step-by-step recognition:

1. Open a part with imported body features.

2. Click Recognize Features (Features toolbar) or Insert, FeatureWorks, Recognize Features.

The FeatureWorks dialog box warns you if features are not supported. You have two options:

• Delete unsupported features. Deletes those features and dependents from the final document

• Map unsupported features as thicken features. Maintains the geometry of the final part and retains child features (Available only for boss and cut loft, boss and cut sweep, and non-legacy holes).

3. In the FeatureWorks PropertyManager, select the features to recognize, then click .

If you use Interactive Recognition Mode, you can click Recognize. The FeatureWorks PropertyManager remains displayed. FeatureWorks removes recognized features from the model.

In the Intermediate Stage PropertyManager, under Recognized Features, note that FeatureWorks recognized only the selected features.

4. Click .

The recognized features appear in the SolidWorks FeatureManager design tree.

5. Save the document.

Now you can recognize other features contained in the partially recognized imported body.

1. In the SolidWorks FeatureManager design tree, right-click the imported body and select FeatureWorks, Recognize Features.

2. In the PropertyManager, select more features to recognize, then click .

FeatureWorks recognizes the features, and they appear under Recognized Features in the Intermediate Stage PropertyManager.

3. Click .

4. Save the document as a different name.

5. Complete recognition of the remaining features in the imported body.

When recognition is complete, the imported body no longer appears in the SolidWorks FeatureManager design tree.