Figure 1. From Left to right: traditional engine, 3D Interconnect assembly, 3D Interconnect part.
Background: Working with Imported Geometry
In today’s multi-CAD world, the interoperability between various CAD solutions becomes increasingly important. For example, large concept assemblies could be started in CATIA or NX, then broken out into functional subassemblies that are easier to finalize in SOLIDWORKS. Similarly, PCB boards can be generated by Altium and used in SOLIDWORKS assemblies as components.
Figure 2. File Types available under the File Open dialog in SOLIDWORKS.
Even though the CAD industry made huge steps forward in ensuring interoperability (for example, 3DEXPERIENCE Platform, NX Synchronous Technology, or the fact that SOLIDWORKS can open almost any native file created by other CAD systems), the STEP file is still the most used vessel for moving data from one CAD system to the other.
In real life, end-users have no access to the original author of the neutral file, so they will have to use whatever file format they get.
There are multiple articles describing preferences for the neutral file types you should demand from your customer. In real life, many end-users have no access to the original author of the neutral file, so they will have to use whatever they get. This series of articles will focus on best practices to get the most from working with STEP files. That being said, many of the tools and techniques presented could apply to working with other file formats.
SOLIDWORKS recognized this trend in the industry, and in 2018 significantly improved the functionality for importing STEP files by giving users two separate STEP importing engines incorporated into the standard version of the software.
Typical Repetitive Workflows Involving Imported STEP Files
Depending on where your company is positioned in the supply chain, your role as a SOLIDWORKS user can include one or more of these repetitive activities:
- Importing STEP files into SOLIDWORKS.
- Performing Import Diagnostic procedures.
- Healing topological errors.
- Comparing the changes in geometry between two successive revisions of a STEP file.
- Updating the SOLIDWORKS models based on the data from revised STEP files.
- Repairing assembly mates due to loss of references (face, edge or vertex ID) involving models based on new data from revised STEP files.
- Repairing drawing detailing elements (dimensions, balloons, annotations) due to loss of references (face, edge or vertex ID) involving models based on new data from revised STEP files.
This series of articles will focus on suggesting options, best practices and workarounds for maximizing the quality of the imported geometry, while reducing the manual work required by the end-user, using only the standard functionality from inside SOLIDWORKS.
- Article #1 – The Battle of Two Import Engines – Quality and Speed (Traditional versus 3D Interconnect)
- Article #2 – Strategies to Preserve the Mates and Dimensions during Revisions
- Article #3 – Comparing Geometry Changes between STEP Revisions
- Article #4 – Simplification Techniques for using Complex Imported Geometry in Large Assemblies
One thing is clear – there is a lot of confusion.
Two Importing Engines Are Better Than One
Three years have passed since SOLIDWORKS added a second import engine for STEP files, and after talking to hundreds of users who have partnered with my team for consulting and mentoring sessions, it became clear that there is a lot of confusion about three things:
- Using the optimal import engine for a specific application or workflow.
- Determining the pros and cons of each engine.
- Identifying ways to edit imported geometry created by the new engine.
This series of articles endeavours to answer these questions.
Conclusions… First
We know that many readers are jumping directly to the conclusions, so we decided to table them in the beginning. The rest of the article is supporting this information with case studies, benchmarks, best practices, tips and tricks.
Table 1. Traditional Import Engine vs 3D Interconnect.
Note about Revision Reliability: Strategies for increasing revision reliability will be covered in Article #3.
Chapter 0: Selecting the Import Engine
The default options for selecting the Import Engine (Traditional or 3D Interconnect) are located in the System Option/ Import /General (Figure 3).
Figure 3. System Settings for Imported Geometry.
If the Enable 3D Interconnect box is not checked, the Traditional Import Engine (TIE) will be used. If it is checked, the 3D Interconnect Engine (3DIE) will be used.
Since this setting applies to various file formats, it is important to see how it affects the importation of STEP files.
Notice that if the box is checked, the import options on the same page are greyed out. In this case, each type of file format would have its own options.
To access the STEP import options for 3DIE, from the File Format dropdown, select STEP/IGES/ACIS.
Figure 4.
The result is a second options page dedicated to importing STEP files (Figure 5).
Figure 5.
Right away it becomes clear that by using 3DIE, a new Assembly Structure Mapping option becomes available, i.e. Import Assembly as multiple body part.
With 3DIE, the user can choose to:
- Import the model using the structure from inside the STEP file; an assembly will import as an assembly, and a multibody part will import as a multibody part.
- Import a multibody part as an assembly.
- Import an assembly as a multibody part.
To select the Traditional Import Engine (TIE), simply uncheck the Enable 3D Interconnect box (Figure 6).
Figure 6. Selecting the Traditional Import Engine (TIE).
Notice that in this case, the options for determining the Assembly Structure are limited. The only relevant checkbox is Import multiple bodies as parts.
With TIE, the user can choose to:
- Import the model using the structure from inside the STEP file; an assembly will import as an assembly, and a multibody part will import as a multibody part.
- Import a multibody part as an assembly.
With the Traditional Import Engine, a multibody part can be imported as an assembly, but there is no option for directly importing an assembly as a multibody part.
Good to know: The Import System Settings are not “really” set in stone. They are just the last settings used in an import operation. So, let’s not call these “default settings” so much as “the last used settings.”
The system setting can be overwritten during the File Open operation. If a STEP file is selected, the user can customize the Import settings as needed.
Once the STEP file import has started, the settings used last time overwrite the system setting.
Figure 7.
Figure 8.
Chapter 1: Import Quality
After performing multiple tests for comparing the quality of the topology and geometry imported from STEP files with TIE versus 3DIE, the conclusion is simple: each engine produces a different result. In some cases, the model obtained from TIE is superior to the one created by the 3DIE, other times the opposite is true.
Case Study #1 – Complex Assembly
In Figure 9, we imported the same STEP file containing an assembly using:
- TIE for the model on the left.
- 3DIE with the assembly option for the model in the center.
- 3DIE with the multibody part option for the model on the right.
Figure 9. From Left to right: Traditional Engine, 3D Interconnect Assembly, 3D Interconnect Part.
In this specific case, the model on the left exhibits more surface artifacts than the model in the center. The one on the right does not seem to have any visible problems.
It is worth mentioning that even though a model created by 3DIE might have topological errors, they will not be listed in the FeatureManager tree like they are for the TIE.
Case Study #2 – Unibody Part
We imported this STEP file using both engines.
With the TIE, the Import Diagnostic tool discovered (Figure 10):
- Two faces having General Geometry Problems.
- One Self-intersecting face.
Figure 10. Topological Errors using TIE.
Usually the Import Diagnostic tool can heal General Geometry Problems, and that was also true in this case study.
There is no automatic healing solution for Self-intersecting faces, so we had to delete the face and remodel it.
With 3DIE the number of faces reporting topological errors was larger (Figure 11).
- Four faces with the warning Vertex is not on curve.
- Five faces with the warning Unsimplified geometry.
Figure 11.
It is very important to know that topological errors for models imported using 3DIE cannot be fixed by the Import Diagnostic tool unless the 3D Interconnect features are dissolved, which means the link to the STEP file is broken.
Figure 12. Dissolving a 3D Interconnect Feature.
Figure 13. The link breakage is permanent.
After breaking the link, the Import Diagnostic tool was able to automatically heal all nine problems.
Figure 14. All fixed.
Another clue that each engine produces a different model is the difference in Volume and Surface Area between the two models. The differences are small, but not insignificant.
Figure 15. TIE (left), and 3DIE (right).
Case Study #3 – Complex Multibody Part (211 Solid Bodies, 4339 Surface Bodies in original STEP file)
The difference in model quality was astonishing (see Figure 16).
Figure 16.
Figure 17.
- TIE missed 135 more faces than the 3DIE.
- 3DIE was very successful in knitting 4130 more surface bodies than TIE and converting them to solid bodies.
Other cases were even more extreme. Below there are several behaviors we observed in practice, each covering a different STEP file:
- SOLIDWORKS would crash when using TIE, but would create a model when using 3DIE, for the same STEP file.
- A model would be created using TIE, while no geometry would appear using 3DIE.
- Components in an Assembly file would be moved from their position using 3DIE. They would appear in the correct location and orientation using TIE.
- More topological errors would appear in a model imported with TIE.
- More topological errors would appear in a model imported with 3DIE.
After multiple case studies, the only recommendation we can offer is to test using both engines when encountering problems. See which model has the best geometry and topology, and discard the other one.
Chapter 2: Import Speed
Two of the main complaints we heard from SOLIDWORKS users, especially from the ones who need to import complex STEP files in the automotive industry, are:
- SOLIDWORKS crashes after spending hours trying to import a complex STEP file.
- SOLIDWORKS takes a long time (hours) to import a complex STEP file.
The main reason for crashes is an insufficient amount of RAM in the workstation used for the import process. The whole data is stored only in the RAM during the process. No files are saved on the drive, even if the STEP file contains a huge assembly with many components that have many bodies.
In extreme cases, users who had 32 GB RAM installed experienced crashes. When opening the same STEP file on a workstation with 64 GB RAM, the import succeeded.
We recommend 64 GB RAM or more for importing large STEP files.
We performed multiple benchmarks timing the opening of various types of STEP files using both engines.
Case Study #4
Simple Part (Unibody)
Figure 18. Unibody Part – Import Speed.
Case Study #5
100% Solid Multibody Part (348 Solid Bodies, 0 Surface Bodies)
Figure 19. Solid Multibody Part – Import Speed.
Case Study #6
Complex Multibody Part (211 Solid Bodies, 4339 Surface Bodies)
Figure 20. Complex Multibody Part – Import Speed
Case Study #6
Simple Assembly (397 Components, 348 Solid Bodies, 0 Surface Bodies)
Figure 21. Simple Assembly – Import Speed.
Case Study #7
Complex Assembly (20 Components, 1224 Solid Bodies, 18975 Surface Bodies)
Figure 22. Complex Assembly – Import Speed.
Note that for Case study #7, we also took advantage of the 3D Interconnect functionality for importing assemblies as multibody parts. The opening time in this mode was 4,019 seconds.
This number is astonishingly low, considering how complex and time consuming the process is for saving an assembly originating from a STEP file as a multibody part:
- Open the assembly from STEP.
- Save the assembly file (extremely time consuming, especially for TIE).
- Save the assembly file as a multibody part.
Conclusion for Part 1: The Battle of Two Import Engines – Quality and Speed (Traditional versus 3D Interconnect)
All these case studies made clear that two engines are better than one. If the geometry obtained from using TIE is unacceptable, try 3DIE—and vice versa.
For import speed, 3DIE seems to have the edge over TIE, but that would need to be placed in the context of revision workflows of the models. As you will see in the next articles in this series, the import speed is not everything, considering that most of the time it is only done once.
The resulting model, however, will be opened tens or hundreds of times as a component of a larger assembly. Without optimizing the imported geometry, the overall productivity when working with such assemblies would be impacted.
It is imperative that users have a clear vision about how the imported geometry will be used in their workflows and optimize it accordingly.
This will be one of the main topics to be covered in the following articles. Stay tuned.
To be continued in:
Article #2 – Strategies to Preserve the Mates and Dimensions during Revisions
Article #3 – Comparing Geometry Changes between STEP Revisions
Article #4 – Simplification Techniques for using Complex Imported Geometry in Large Assemblies
Learn more about SOLIDWORKS in the whitepaper Design Through Analysis: Simulation-Driven Product Development Pays Business Dividends in Transition to Smart Manufacturing.
As an Elite AE and Senior Training and Process Consultant, working for Javelin Technologies, Alin Vargatu is a problem hunter and solver, and an avid contributor to the SOLIDWORKS Community. He has presented 25 times at SOLIDWORKS World, once at SLUGME and tens of times at SWUG meetings organized by four different user groups in Canada and one in the United States. Alin is also very active on SOLIDWORKS forums, especially on the Surfacing, Mold Design, Sheet Metal, Assembly Modeling and Weldments sub-fora. His blog and YouTube channel are well known in the SOLIDWORKS Community.