Automatic Recognition - FeatureWorks

The FeatureWorks software is included within SOLIDWORKS Professional+. It works to recognizes standard or sheet metal features of imported “dumb” models. You can recognize standard or sheet metal features when importing from neutral file formats such as IGES, STEP, Parasolid (.x_t, .x_b), SAT, and VDAFS.  You can use step-by-step recognition with automatic and interactive feature recognition or a combination of these methods.  FeatureWorks will also automatically add dimensions to features that it recognizes. Once these features have been recognized, they are added to the FeatureManager design tree to be modified similar to any other SOLIDWORKS features.

 

In this example, I am using a part imported from an IGES file type. I’ve already gone ahead and ran the Import Diagnostics to check for faulty faces or gaps which produced no errors.
Notice that the Feature Manager Design tree contains only the Imported1 feature that makes up the entire part.

With SOLIDWORKS Professional, I can use FeatureWorks to recognize and add features to the Design tree.
Insert > FeatureWorks > Recognize Features

You can recognize features automatically!
For this first example, I will use the automatic function by selecting it from the property manager and initiate the recognition by clicking on the green check or the blue next arrow.

The automatic recognition will step through the model, analyzing geometry and apply appropriate SOLIDWORKS features to closely recreate the solid part.  We are then given a preview list of those recognized features.
After a quick review of the list I see that there is a revolved feature that doesn’t quite match our design intent. After selecting that feature from the list, I can then re-recognize that feature as a Base-extrusion instead of Base-revolve.
Clicking the Green Check will complete the process.

The automatic recognition did fully apply SOLIDWORKS features to the Import1 solid body, but something still seems a bit off. Upon further review, I can see that the fillets were applied out of order.

Features recognized by FeatureWorks are fully editable!
I went ahead and made a few adjustments to the Design Tree. By simply moving the order of the Fillets and adding a tangent propagation to the final fillet, you can see that the model now cleanly matches the original import.  I also edited the definition of one of the holes, changing it to a 5/8” clearance hole.
I now have the confidence to make modification and introduce my SOLIDWORKS part into my assembly!