Repairing Imported Models with SOLIDWORKS Surfacing Tools

   By Ben Colley on December 27, 2022

In the manufacturing industry, it’s very often the case that companies need to work in cooperation with independent contractors and other manufacturers to develop a product. One company specializes in small motors, while another company may specialize in molded plastic… while another company works with die cast metals, etc. It’s almost a guarantee that each of these companies will use some form of 3D CAD to develop their particular products; and because the CAD market consists of a wide variety of programs, each serving different companies according to their needs, this presents a challenge to collaboration when they are ready to combine their CAD assets. Learn how to repair imported models with SOLIDWORKS surfacing tools in this in-depth case study example.

SOLIDWORKS supports a wide range of common CAD file types, such as AutoDesk, Solid Edge, Rhino, NX (etc.), and can import them directly into the SOLIDWORKS modeling environment. If a file is coming from a less common CAD program, then SOLIDWORKS can also work with neutral formats that are used industry-wide, such as STEP, IGES, and Parasolid files. There’s no escaping the fact, however, that different programming is used in each software to generate the 3D models, so when non-native CAD files are brought into SOLIDWORKS, there is often some level of repair that needs to be done, either through automated processes or manual tools. Fortunately, SOLIDWORKS is well-equipped to work with non-native files, having a variety of built-in solutions to deal with the imported geometry:

  • Import Diagnostics: When SOLIDWORKS opens a non-native CAD file, Import Diagnostics searches for problem areas in the model, and can often fix any faulty faces or gaps that are identified during the translation to SOLIDWORKS geometry.
  • FeatureWorks: SOLIDWORKS models are feature-based,­ allowing for complete parameterized control of the geometry. Imported models don’t come with any feature history, but FeatureWorks gives you the option to assign features to imported geometry to give you the same kind of parametric control over it as you would have of a native SOLIDWORKS part.
  • Surfacing Tools: Regardless of the geometry that comes into SOLIDWORKS, it will, at its most basic, be constructed of a tapestry of knitted faces. SOLIDWORKS’ robust assortment of surfacing tools gives users complete capability to repair and reconstruct imported models.

Although the full assortment of Surfacing tools is useful for imported model repair, a few tools stand out as particularly helpful when dealing with broken surfaces and gaps:

  • Delete Face
  • Filled Surface
  • Delete Hole
  • Trim/Untrim Surface
  • Intersect

SOLIDWORKS also includes a variety of analysis tools that aid in model repair, including:

  • Check Entity
  • Curvature
  • Zebra Stripes
  • Deviation Analysis.

To see these tools in action, we’ll look at a case study with an imported model of a carving knife handle.

Case Study: Imported Carving Knife Handle

Scenario: We’re working with an outside contractor to develop a mechanized carving knife. Our company uses SOLIDWORKS to model the internal mechanism, while the outside contractor uses a program called “AwesomeCAD” to model a hollow handle. AwesomeCAD is not a widely used CAD program, so the contractor exports the model to a STEP file, which we will import into our SOLIDWORKS assembly to complete the product.

Route A: Import Solids

“Plan of attack”:

  • Use Import Diagnostics to fill gaps, knit unattached surfaces, and create enclosed volumes.
  • Use Combine to subtract the inner volume from the outer volume.
  • Use Curvature, Zebra Stripes, and Deviation Analysis to identify areas with discontinuity in curvature
  • Use Delete Face (Delete and Patch) to remove faulty surfaces and fill in with surrounding faces.

We begin by importing the STEP file with a simple File > Open. The options utilized in the import affect how SOLIDWORKS will translate the imported geometry into a SOLIDWORKS model. By default, SOLIDWORKS looks at any fully enclosed surface bodies and tries to turn them into solid bodies.

Importing system options

Import system options

Using the default import options, we immediately see issues when we run Import Diagnostics. Instead of a single solid model with an internal cavity, we get a solid interior, with a broken set of surface bodies on the exterior. There’s a hole in the thumb rest, a broken-out gap on the edge of the button, and the button is not knitted to the rest of the model.

handle with broken surface bodies

Handle with broken surface bodies

Upon using the healing options in Import Diagnostics, the holes in the outside surface are filled by new faces, the disjointed surface bodies are knitted together, and we end up with two overlapping solids – the volume enclosed by the exterior surface and the volume enclosed by the interior surface. This allows us to easily create the shelled solid by use of the Combine tool. We preselect the two solids, launch the Combine tool (with the “Subtract” operation type), and end up with a single hollow solid.

Combine tool

Combine tool

Upon closer inspection of the faces that were generated by Import Diagnostics, however, we realize that our repairs aren’t done. From the Evaluate tab of the CommandManager, we make use of Curvature and Zebra Stripes to get visible cues of a discontinuity in curvature between the original curved surfaces and the new surfaces that were created to fill the gaps in the model.

curvature and zebra stripes

Curvature and zebra stripes

The discoloration at the edge of the new surface and the jagged break in the zebra stripes tell us that there is a sharp change in curvature between the original surfaces and the generated patches.

To quantify the deviation that’s occurring, we make use of Deviation Analysis, and select the edges of the larger surface that was generated on the thumb rest.

deviation analysis

Deviation analysis

A color-coded set of arrows indicates a fluctuating deviation – an upward tilt along the edge of the new face, ranging up to a 3-degree deviation from the surrounding surface.

To solve this issue, we make use of a quick and easy fix, “Delete and Patch” with the Delete Face command, from the Surfaces tab.

Delete face

Delete face command

In this case, SOLIDWORKS is able to successfully extend out the surrounding surfaces to patch the holes that are created when removing the faulty faces, and repairs are done. We have a single, solid, shelled part with no gaps or broken surfaces.

Route B: Import Surfaces

import surfaces

Import surfaces

“Plan of attack”:

  • Use Check Entity to identify gaps
  • Use Filled Surface with “Curvature” to patch hole


Use Delete Hole

  • Use Filled Surface to complete spherical button surface


Use Untrim Surfaces

  • Knit outer surfaces together into a watertight surface body
  • Use Intersect to fill in volume between the inner and outer surface bodies.

Sometimes, Import Diagnostics won’t get us as far as we’d like in the repair process, and we’d be better off repairing the model manually with surfacing tools. And if solids are not being generated the way we expect them to, then we may be better off unchecking that setting in the import options. So, in this case, we don’t try to create solids (Options) and we skip Import Diagnostics. As a result, in this case study, we end up with three surface bodies: the “watertight” (fully enclosed) inner surface body, the outer surface with some gaps, and the broken button surface.

In this model, the problem areas are easy to visually identify, but that’s not always the case. Sometimes the gaps are very small, or in hard-to-see areas. This is where the Check Entity (“Check”) command – which searches for invalid faces, invalid edges, and open surfaces – can be very useful. To find the gaps in the model, we launch the Check command from the Evaluate tab.

check entity command

Check entity command

The Check operation identifies two open surfaces – the spherical button surface and the large outer surface – and highlights the boundary surfaces where gaps are present. With these areas identified, we can see where repairs need to be made.

The intuitive fix for the large hole in the thumb rest would be Filled Surface – just patch the hole with a new face. So, we launch the Filled Surface command, select the edges of the hole, and are presented with three options for the boundary conditions:

  • Contact
  • Tangent
  • Curvature

“Contact” is chosen by default, so we try this boundary condition first.

applying boundary condition

Applying boundary condition

The hole successfully patches, but on closer inspection with Curvature Analysis, we see the same discontinuity in curvature that we encountered earlier with the Import Diagnostics fix. This is because the “Contact” boundary condition does not factor-in the curvature of adjoining faces; it only acts to generate the simplest face possible given the edges of the hole.

The “Tangent” condition would take surrounding faces into account, but only for a limited distance across the new face, similar to a fillet. This might be acceptable in this case, but the best option for coming up with a seamless patch would be “Curvature”. This accounts for the surrounding faces and extends them into the new face as far as possible, eliminating any breaks in curvature continuity.

curvature option used to repair solidworks models

Curvature option

Using this option, we see clean curvature, and a Deviation Analysis shows basically zero deviation along the edge of the new face, so this may be an acceptable fix for the end product. The manufactured part would show no sign of a break in the thumb rest.

However, an even better option exists for repairing this particular type of gap. Instead of patching the hole with a new face and trying to blend curvature, we can remove the problem area altogether with Delete Hole. We select Delete Hole from the Surfaces tab of the CommandManager, select a boundary edge of the hole, and execute.

repair solidworks with delete hole command

Delete hole command

Just like the Delete and Patch operation we used earlier, Delete Hole extends out the existing faces to fill the gap as if it were never there. This means there will be no break in curvature continuity, and no extra faces to complicate the model. This is the best fix for this case.

Looking to the broken button surface, we’re presented with a slightly different challenge. Instead of an enclosed hole, we have a break-out on the edge. There are a couple ways we could fix this break:

Repair Option A) We could repair the break using a Filled Surface operation. This would be done by sketching-in an arc to complete the circular edge around the base and using the sketched entity as a boundary in the Filled Surface.

Repair Option B) The better option for this application is the Untrim Surface command on the Surfaces tab. We select this option and start picking edges from the broken-out section. As selections are made, SOLIDWORKS looks for a solution with the cleanest face and boundary, extending the surface into the broken-out section, similar to Delete Hole.

 untrim surface

Untrim surface command

Built into the Untrim Surface command is an option to extend the face out from the edges by some percentage. If we leave the extension at 0%, a simple patch will be created, and the bottom edge of the surface body will be segmented between the original surface edge and the patched edge that was just created. This may be acceptable, but if you prefer to have a continuous, unsegmented circular edge all the way across the bottom of the surface, then it would be a good option to extend the surface out by some amount, then trim away the excess with a sketched circle. So, we create a plane that’s coincident to the bottom edge, sketch a circle on the plane that is coradial to the existing edge, Untrim the surface while specifying some percentage of extension, and use Trim Surface to cut away the extra material. The result is a perfectly curvature-continuous semi-sphere with an unbroken circular boundary.

trim surface

Trim surface command

At this point, all that remains is to knit the button surface to the rest of the outer surface body and fill in the volume between the inner and outer surfaces with material. Starting with Knit Surface, we select the outer body and button surface to knit together and leave the option to Create Solid unchecked.

 knit surface

Knit surface command

We now have two watertight surfaces and can create a solid by filling in the volume between the inner and outer surfaces using the Intersect command (located in the Features tab of the CommandManager). We launch Intersect, select the two surface bodies, and pick “Create Internal Regions” from the Intersect options.

intersect Command

Intersect command

The result is a solid body. A section view reveals that material now fills the volume between the inner and outer surfaces. We can now use this model to full effect in our product assembly.

Conclusion – Repairing Imported Models

repairing imported models

Repairing imported models

As we have seen, SOLIDWORKS gives us plenty of tools to take care of repairs on imported models, from automated diagnostic and repair tools to analysis and surface modeling tools. There’s no one-size-fits-all approach to fixing models, as each one will come with its own set of unique geometrical challenges. In some cases, more extensive reconstruction and a broader range of surfacing tools will be needed. But the handful of tools we’ve covered in this case study is a great place to start with simple repair jobs, and you’ll greatly benefit from keeping them on your radar.

Related Products

Browse the TriMech web store for SOLIDWORKS software to design, analyze and manufacture your products on your desktop.

Ben Colley

Related Content

3D Model Powerpoint Solidworks

Bring your SOLIDWORKS Models to Life in a PowerPoint Presentation

Next time you want to showcase your 3D SOLIDWORKS CAD Model in a PowerPoint presentation,…

Learn More...

How to create a piping route with SOLIDWORKS

Today we’re going to review how we can create a piping route for this current…

Learn More...

Quick Imported Simplification using SOLIDWORKS Import Diagnostics

If you work with big STEP or IGES files, you know how critical it is…

Learn More...