Quick Imported Simplification using SOLIDWORKS Import Diagnostics

By Alin Vargatu on

If you work with big STEP or IGES files, you know how critical it is to simplify the imported geometry in SOLIDWORKS before inserting it in large assemblies or referring it in drawings.

SOLIDWORKS has many tools and techniques for achieving this goal, which we will cover in future blog articles, but today let’s focus on a very simple technique using a very little known tool: Import Diagnostics.

Many of you have probably used it to troubleshoot and fix (with various degrees of success) topological errors in the imported features.

Have you ever considered its amazing functionality for direct editing a model?

Let’s compare the two models shown in Figure 1.

Comparing two models
Figure 1

The one on the left has just been imported from a STEP file. It contains complex internal details that are irrelevant for the user who will insert it in a large assembly.

What if you could quickly separate the internal faces from the rest of the part and quickly fill everything with solid material to obtain the part on the right side?

Moreover, what if this process could avoid producing extra features in the tree? It would be like directly editing the STEP file!

The technique is very simple and involves the Direct Editing tool.

STEP 1 – Start the Import Diagnostic tool

One way to do that is shown in Figure 2.

import diagnostic tool

Figure 2

STEP 2 – Heal any topological errors (optional)

If import errors are reported, you can attempt to heal them now. In future articles we will focus in detail on the best practices for fixing import errors.

repair face tool
Figure 3

STEP 3 – “Crop” the faces that separate the “outside” from the “inside”

Consider holding this model in your hands and using a pair of scissors to separate the “inside” from the “outside”. We can do that using the SOLIDWORKS Import Diagnostics tool by deleting faces connecting the “inside” from the “outside”.

When selecting these faces, consider saving “functional” faces and edges that could be used for mating other components at the assembly level.

delete face

Figure 4

Do not be afraid of the gaps that are reported after the faces are deleted. It simply shows that the original solid body has been converted to surface bodies (the “solidness” flew out through the gaps).

fill cavities

Figure 5

STEP 4 – Click “OK” to exit the Import Diagnostic Tool

The result is shown in Figure 6. The “inside” and “outside” are now two separate surface bodies, and, more importantly, two separate imported features.

separate surface bodies
Figure 6

STEP 5 – Delete the “inside” imported feature

The result is shown in Figure 6. The “inside” and “outside” are now two separate surface bodies, and, more importantly, two separate imported features.

delete the inside imported feature
Figure 7

The result is a “hollow” surface body containing the faces we want to preserve.

hollow surface body
Figure 8

STEP 6 – Run Import Diagnostics to close the gaps

To close the gaps without adding any unnecessary features in the tree, run Import Diagnostics again and Heal all Gaps.

import diagnostics: gaps between faces
Figure 9

STEP 7 – Heal all topological errors

If there are any errors reported by Import Diagnostics, heal them.

import diagnostics: heal all faces
Figure 10

STEP 8 – Exit Import Diagnostics – Job Done!

Congratulations! You have just simplified a complex part in 1 minute!

exit import diagnostic

3DEXPERIENCE World Presentation:

If you plan to attend the 3DEXPERIENCE World 2023, join us on in studying more use cases like this for the SOLIDWORKS Import Diagnostics tool.


About the Author

As an Elite AE and Senior Training and Process Consultant, working for TriMech Solutions, Alin Vargatu is a Problem Hunter and Solver.

He has presented 38 times at 3DEXPERIENCE World and SOLIDWORKS World, twice at SLUGME and tens of times at SWUG meetings in Canada and the United States. His blog and YouTube channel are well known in the SOLIDWORKS Community.

In recognition for his activity in the SOLIDWORKS Community, at 3DEXPERIENCE World 2021, the SWUGN (SOLIDWORKS User Group Network) awarded the SOLIDWORKS AE of the Year title to Alin Vargatu.