How Stuff Works – FeatureWorks Part II

Reverse Engineer Modeled Parts

FeatureWorks

How Stuff FeatureWorks, Part II

Part 2: Interactive Recognition

Prerequisite, Part 1: Automatic Recognition

So now that we know a bit more about FeatureWorks, lets look at how we can make it work around our own ideas and design intent. Here you can see that I’ve inserted the same part as before in an assembly. Notice that that the position of the mounting tab falls off the weldment. Lets see how we can use FeatureWorks to deconstruct and rebuild this part, populating a design tree that will give us recognizable features that we can then modify to reflect the changes that need to be made.

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First, we will take a look at the design tree created by the FeatureWorks Automatic Recognition process and really see how this piece was built.

Here I’ve gone back to edit the feature that creates the tab. The automatic recognition does create SOLIDWORKS features, but not how I expected it to. Depending on your level of accuracy and design intent needed, Automatic recognition may not always give you desired results. SOLIDWORKS FeatureWorks give us options though.

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With FeatureWorks, you can recognize features interactively!

Here we will look at another mode of feature recognition, the Interactive mode.

Through the interactive mode we can choose to recognize just a few features or all features!

Starting over from the imported IGES file, I will choose the Interactive Mode from the FeatureWorks property manager

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Leaving the feature type set to Standard Features, I then begin working backwards to deconstruct this part by first selecting Fillet/Round from the Interactive features feature type. After selecting all the fillet surfaces, using chain fillet faces to speed up the selection, I then selected the Recognize button. SOLIDWORKS FeatureWorks then removes all the fillets, creating a fillet feature that we will see in the design tree when we’re done.

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After repeating the recognition process for both the inside and outside corner fillet, I then changed the feature type to Hole. This feature has a few additional options that we can use, including Recognize Similar. This option will allow FeatureWorks to apply additional features to the design tree for each additional hole of the same size. If there was a series of holes, I would elect to use the Recognize pattern option. Again, once recognized, the features will then be populated to the design tree and are removed from the model.

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We can recognize the slot as a Cut Extrude by first selecting the edges (select as loop), then the opposite “up to” face.

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NOTE: The current recognized features can be viewed at any time by hitting the Next button. Here you can find potential patterns as well as re-recognize features as another type. For example, you could re-recognize a Hole wizard hole as a cut- extrude instead. To return to the FeatureWorks, simply hit the Back arrow.

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We can continue to dissect this model by recognizing the remaining elements by using the Boss Extrude feature type and selecting an initial starting face and the Up to face.

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Once the model has been fully recognized down to the last element, FeatureWorks will automatically advance to the “Next” property manager, giving you a last chance to make any corrections or recognize any patterns.

Exiting the FeatureWorks property manager, we can see that there is a fully recognized, editable feature design tree.

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In this example, I went ahead and edited the HoleWizard M18 Clearance Hole1 to be a 5/8 Clearance Hole.

(TEASER) For Fun, I used Feature Paint to copy the properties of one hole to the next just to illustrate how the recognized features are now complete SOLIDWORKS features.

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Making changes is now easier than ever!

For features that are based on sketches, after you recognize the features, you can edit the sketches from the SOLIDWORKS FeatureManager design tree to change the geometry of the features! In this example, I modified the sketch of one of the tabs, flipping its position.

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Now we can see the final product, modified from an imported IGES model thanks to FeatureWorks!

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Follow this link for more information on FeatureWorks!

Next Month!  Line Color and Lofting

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Symmetry Solutions
Symmetry Solutions, Inc. is your official SOLIDWORKS 3D CAD software and training provider for the Upper Midwest. We serve Minnesota, Wisconsin, North Dakota and South Dakota with premier SOLIDWORKS training, support and implementation services for the complete suite of SOLIDWORKS 3D design solutions. For more information on SOLIDWORKS, visit: www.symsolutions.com - Learn more about SOLIDWORKS Training or SOLIDWORKS Online Training - Learn more about SOLIDWORKS Solutions: 3D CAD, Simulation & Design Validation, Technical Communications, Product Data Management, Electrical Design, Quality Control, Education Edition, Free SOLIDWORKS Tools, 3DExperience
Symmetry Solutions
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