SolidWorks FeatureWorks Guide

Contents

FeatureWorks is the SOLIDWORKS feature-recognition add-in that converts “dumb” imported solids into editable, parametric SOLIDWORKS models. Instead of being limited to a single Imported body, you can recover bosses, cuts, holes, fillets, chamfers, drafts, patterns, and even sheet metal features, and then edit them just like native SOLIDWORKS features.

This guide explains what FeatureWorks does, when it makes sense to use it, how the Automatic and Interactive recognition modes work, and walks through a practical step‑by‑step workflow (with screenshots) to turn a neutral file into a fully editable model. You’ll also find best practices, limitations, and troubleshooting tips, especially for sheet metal parts.

What is SOLIDWORKS FeatureWorks?

FeatureWorks is supplied as an add-in for SOLIDWORKS that performs geometry-based feature recognition on imported solids in part documents. When you open a neutral or foreign CAD file, FeatureWorks analyzes the boundary representation (B-rep) geometry and attempts to reconstruct a feature tree that mirrors how the part might have been modeled originally.

As of current releases, FeatureWorks is included with SOLIDWORKS Standard, Professional, and Premium licenses, so you do not need to purchase a separate product. Once enabled, FeatureWorks:

Recognizes features on imported solid bodies in a part document.
Creates “real” SOLIDWORKS features (boss extrudes, cuts, fillets, chamfers, ribs, shells, etc.), not just annotations.
Lets you edit those recognized features (dimensions, end conditions, pattern definitions, etc.) just like native features.
Can work with both prismatic/machined parts and many sheet metal parts.

Supported file types

FeatureWorks operates on imported solid bodies from file formats that preserve B‑rep geometry, for example:

STEP (AP203/AP214/AP242)
IGES
Parasolid (X_T / X_B)
ACIS SAT
VDA‑FS
Various other supported neutral and CAD formats that SOLIDWORKS can import as solid bodies

Mesh-only formats such as STL or OBJ are not suitable for FeatureWorks. These are faceted polygon meshes, not analytic surfaces, so the recognizer cannot infer true cylinders, cones, or planes from them. In those cases you generally have to remodel or use different reverse‑engineering tools.

Accessing the FeatureWorks add‑in

To enable FeatureWorks in SOLIDWORKS:

Go to Tools > Add‑Ins…
Enable FeatureWorks in the Active Add‑ins column.
Optionally enable it in the Start‑Up column so it loads automatically with SOLIDWORKS.

Once enabled, you can access FeatureWorks from:

Insert > FeatureWorks (commands such as Recognize Features).
The right‑click menu on an imported body in the FeatureManager tree (FeatureWorks > Recognize Features).
Automatic prompts when opening certain imported parts, depending on your FeatureWorks options.

When should you use FeatureWorks?

FeatureWorks is most useful in workflows where you need to modify geometry that did not originate in your current version of SOLIDWORKS:

Vendor or customer parts: You receive STEP/IGES/Parasolid files and want to tweak hole sizes, adjust fillets, change draft angles, or add machining features.
Legacy models from other CAD systems: You want to bring Inventor, Pro/ENGINEER/Creo, CATIA, NX, etc. models into SOLIDWORKS and continue parametric work.
Backwards compatibility: A colleague is on an older SOLIDWORKS version that can’t open your native files. You export a neutral file and let them reconstruct a feature tree using FeatureWorks.
Repairing lost design intent: You have a model where the feature tree is missing or heavily corrupted, but the solid body is still valid.

In general, FeatureWorks works best on geometrically regular, prismatic or machined parts and on many sheet metal parts. Complex organic surfaces, heavily sculpted freeform models, or heavily faceted geometry are poor candidates and are often faster to remodel manually.

FeatureWorks recognition modes

FeatureWorks has three key ways to recognize features:

Automatic Feature Recognition
Interactive Feature Recognition
Step‑by‑step recognition (a hybrid strategy applied over time)

Automatic Feature Recognition

Automatic recognition attempts to scan the entire imported body and identify as many features as possible in one pass. You choose which feature types to look for (extrudes, revolves, holes, fillets/chamfers, ribs, drafts, sheet metal features, etc.), and FeatureWorks computes a feature tree without additional manual selections.

This mode is:

Fast: Minimal user input – mostly just selecting options and clicking Next.
Best for simpler parts: Prismatic geometry, simple holes and pockets, straightforward rounds/chamfers.
Limited on complex geometry: It might leave some portions as unrecognized “leftover” geometry, or choose a modeling strategy that doesn’t match your design intent.

Interactive Feature Recognition

Interactive recognition gives you fine control over what is recognized and how:

You choose the feature type (e.g. Boss Extrude, Cut Extrude, Revolve, Hole, Fillet, Chamfer, Rib, Shell, Sheet Metal features).
You manually select the faces and edges that belong to that feature.
FeatureWorks infers the sketch, direction, end condition, and parameters from that selection and creates the feature.

The main advantages are:

Design intent control: You decide whether a cylindrical cut is a simple hole, a Hole Wizard feature, an extrusion, or a revolve, depending on how you want to drive it.
Control over build order: You can recognize features in a logical modeling sequence (e.g. remove cosmetic fillets first, then recognize main cuts and bosses).
Support for more complex features: Interactive mode can recognize sweeps, lofts, shells, and some geometry that automatic recognition might skip.

If an interactive recognition attempt fails, SOLIDWORKS shows an informative error message explaining why it could not recognize the feature and often suggests alternative selections or strategies.

Step‑by‑step recognition

Step‑by‑step recognition is not a separate mode but a strategy: you recognize features in stages, saving your progress as you go. Typical scenarios:

Run automatic recognition to capture a large portion of the model.
Use interactive mode to recognize features that were missed or misclassified.
Save the part, then later reopen and recognize additional features, or apply recognition to other bodies in a multibody part.

FeatureWorks keeps recognized features in the FeatureManager tree alongside any remaining Imported bodies. You can continue using recognition commands on the remaining imported geometry until everything important is converted or you decide the rest is easier to leave as-is.

What types of features can FeatureWorks recognize?

The exact capabilities depend on SOLIDWORKS version and options, but in general FeatureWorks can recognize:

Standard machined features

Boss and cut extrudes (including blind, through all, up to next end conditions for cuts).
Revolved bosses and cuts (often recognized as equivalent extrudes where appropriate).
Simple and complex holes, including recognition as Hole Wizard holes when configured.
Draft features (tapered walls on bosses and cuts).
Ribs (normal to sketch or parallel to sketch, depending on geometry).
Shells (uniform wall thickness hollowing operations).
Sweeps and lofts in interactive mode for certain profiles.

Applied features

Fillets (constant or variable radius on edges, faces, or chains of edges).
Chamfers (on linear and circular edges).

Feature patterns

Linear, circular, rectangular, and mirror patterns of recognized features.
In some cases, recognition of sketch patterns (interactive) for repeated features that were modeled individually.

Sheet metal features

Base flanges (primary sheet metal base features).
Edge flanges and miter flanges.
Sketched bends.
Hems and certain other standard sheet metal forms.

Not every feature type is guaranteed to be recognized in every model, and some features (for example, highly irregular blends, imported text, or complex organic surfaces) may remain as “dumb” geometry.

Practical workflow: recognizing features in an imported part

The following example shows a typical workflow using the screenshots you already have. We’ll assume you’ve imported a STEP/IGES/Parasolid file as a solid body into a SOLIDWORKS part.

Step 1 – Open the imported file

Open the neutral CAD file directly in SOLIDWORKS using File > Open. Make sure:

The file type is supported by SOLIDWORKS and imports as a solid body (not just surfaces or mesh).
Your import options are configured appropriately (for example, 3D Interconnect on/off depending on your workflow).

Step 2 – Start FeatureWorks recognition

With the imported solid open:

Go to Insert > FeatureWorks > Recognize Features, or
Right‑click the imported body in the FeatureManager tree and choose FeatureWorks > Recognize Features.

The FeatureWorks PropertyManager appears on the left. Here you can choose recognition mode and options.

Step 3 – Configure recognition options

In the PropertyManager, choose the optimal options for your case:

Select Automatic or Interactive for Recognition Mode.
Enable the feature types you care about (extrudes, revolves, holes, fillets/chamfers, ribs, shells, sheet metal features, etc.).
Optionally specify whether to recognize Hole Wizard holes, patterns, or sheet metal features.

Click Next (the blue arrow) to begin the recognition process.

Step 4 – Review and refine recognized features

When recognition completes, FeatureWorks lists the recognized features in the PropertyManager and adds them to the FeatureManager tree. At this stage you can:

Highlight individual features in the list to see which faces they represent.
Use Re‑Recognize to attempt a different classification if a feature was not recognized as desired (for example, reclassifying a cylindrical cut as a Hole Wizard hole instead of a simple cut).
Identify any remaining unrecognized geometry and plan a strategy for those areas (interactive recognition, manual modeling, or leaving them as imported faces).

If the prerequisites are met, you can also use Combine Features to merge compatible recognized features into a simpler, more meaningful feature (for example, combining multiple fillets into one fillet feature), or Find Patterns to identify repeated features and convert them into pattern features.

Step 5 – Inspect the resulting feature tree

After you accept the recognition results, the imported body is replaced (partially or fully) with a set of standard SOLIDWORKS features in the FeatureManager tree. Typical results:

Boss and cut extrudes recreating the main solid volumes and pockets.
Fillet and chamfer features for rounds and edges.
Hole features, possibly recognized as Hole Wizard features if configured.
Sheet metal features if the part was recognized as sheet metal.

Feature names are regenerated by SOLIDWORKS (e.g., an imported feature previously labeled DHole‑50 might become Hole1). This is normal; you can rename features manually if needed.

Step 6 – Edit and reuse the recognized model

Once the features exist in the tree, you can edit them exactly as if you had modeled the part natively in SOLIDWORKS:

Right‑click any recognized feature and choose Edit Feature to change dimensions, end conditions, draft angles, etc.
Adjust pattern counts and spacing for recognized patterns.
Change sheet metal parameters (thickness, bend radius, K‑factor) for recognized sheet metal parts.
Add new SOLIDWORKS features on top of the recognized geometry as needed.

Working with sheet metal in FeatureWorks

For sheet metal parts, FeatureWorks can recognize base flanges, edge flanges, miter flanges, hems, and sketched bends. This lets you convert a generic imported prismatic sheet-metal-like solid into a true SOLIDWORKS Sheet Metal part that supports flat patterns, bend tables, and manufacturing outputs.

When attempting sheet metal recognition:

Ensure the imported body really is a constant-thickness sheet that can be treated as a bent plate (no thick bosses or non-uniform walls in the sheet metal region).
Enable Sheet Metal features in the FeatureWorks PropertyManager and select the relevant options.
Consider recognizing sheet metal features separately from standard features — for example, recognize sheet metal first, then add fillets or other details later.

Note that some sheet metal features (especially complex edge flanges or imported forms) may not be recognized reliably. In those cases, it is sometimes easier to recognize a base flange and bends, then manually remodel problematic flanges.

Best practices and troubleshooting tips

1. Clean the geometry first

Run Import Diagnostics on imported solids to heal gaps, overlaps, and other geometry errors before using FeatureWorks.
Fixing bad geometry up front greatly improves recognition success and performance.

2. Use a recognition strategy, not just a button

On nontrivial parts, treat recognition as a process:

Consider recognizing fillets and chamfers first (or alternately suppressing/removing them) to simplify the main body geometry.
Recognize major cuts and bosses next.
Recognize patterns and remaining details last.
Use step‑by‑step recognition: recognize a subset of features, save, then continue later on the remaining imported geometry.

3. Combine Automatic and Interactive modes

Start with Automatic recognition when the geometry is simple and you want quick results.
Switch to Interactive for areas that automatic recognition missed or misinterpreted, such as complex pockets, lofts, or critical design features.
Use Local Recognition (where available) to recognize specific areas like a single fillet or hole without reprocessing the entire part.

4. Avoid using FeatureWorks on mesh data (STL, OBJ, etc.)

FeatureWorks expects analytic B‑rep geometry (planes, cylinders, cones, NURBS surfaces), not triangulated meshes. If you import an STL as a solid body, FeatureWorks still sees a dense collection of planar facets rather than true cylindrical or planar faces, so recognition will usually fail or produce unusable results. In those cases:

Use the mesh as a reference and model a clean parametric version on top of it.
Or use dedicated reverse‑engineering tools that convert meshes to NURBS surfaces before bringing them into SOLIDWORKS.

5. Know when to stop

FeatureWorks is powerful but not magic. If recognition struggles with a highly complex or poorly defined model, it may be faster and more robust to:

Use the imported model as a reference body and create a new parametric part from scratch.
Recognize only the features you truly need to change (for example, just holes and fillets) and leave the rest as imported geometry.

6. Performance and stability considerations

Recognition on very large or complex parts can be computationally heavy. Consider simplifying the model (removing tiny rounds, cosmetic details, logos, etc.) before running FeatureWorks.
Recognize one body at a time in multibody parts to keep the problem manageable.
Save often, especially before starting recognition on a large imported part.

Disabling or unloading FeatureWorks

When FeatureWorks is not needed, you can disable it to reduce memory usage and simplify the interface:

Go to Tools > Add‑Ins….
Clear the FeatureWorks checkbox in the Active Add‑ins column to unload it for the current session.
Clear it in the Start‑Up column if you do not want FeatureWorks to load automatically on SOLIDWORKS start.

Note that disabling the add‑in does not remove or suppress the features already recognized in your models – they remain as normal SOLIDWORKS features. You simply lose access to the recognition commands until you re‑enable the add‑in.

The advantages of using SOLIDWORKS FeatureWorks

Seamless integration with SOLIDWORKS
FeatureWorks is fully integrated into the SOLIDWORKS environment. All recognition options are available from the SOLIDWORKS menu bar and PropertyManager, and recognized features appear in the FeatureManager tree like any other features. This keeps your workflow consistent and minimizes training overhead.
Reuse of existing CAD data
Instead of re‑modeling an entire part, you can import existing CAD models and convert them into editable SOLIDWORKS feature trees. This saves time and reduces the risk of introducing errors during manual remodels.
Preservation and reconstruction of design intent
Recognized features regain parametric controls and end conditions (for example, a blind or “through all” hole), allowing you to maintain or re‑introduce design intent that was lost during translation. Downstream changes become much safer and more controlled.
Improved collaboration
FeatureWorks simplifies working with suppliers, customers, and colleagues using other CAD systems or different SOLIDWORKS versions. Neutral files can be exchanged, recognized into features, and modified without recreating the design from scratch.
Flexible level of use
You do not have to recognize an entire part. You can use FeatureWorks selectively to recognize only those features you care about – for example, holes and fillets in a vendor part – while leaving the rest as imported geometry.

Bottom line

SOLIDWORKS FeatureWorks is a valuable tool whenever you need to turn imported “dumb” solids into editable, parametric models. By understanding its Automatic and Interactive modes, using step‑by‑step recognition, and applying a sensible strategy (clean geometry, recognize in stages, and avoid mesh-only data), you can recover design intent from neutral CAD files and get back to working in the familiar SOLIDWORKS feature‑based workflow.

Used intelligently, FeatureWorks can significantly reduce re‑modeling effort, improve collaboration across CAD systems and SOLIDWORKS versions, and give you far more control over imported geometry than simple direct editing alone.