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The Ultimate Guide to Working with STEP Files, Part 2: Working with Revised STEP Files

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The Ultimate Guide to Working with STEP Files, Part 2: Working with Revised STEP Files

In Part 1: The Battle of Two Import Engines – Quality and Speed we concluded that SOLIDWORKS users should evaluate both import engines, traditional and 3D Interconnect, when a STEP file is received from a new vendor. Typically, one engine will provide better geometry or a faster import experience than the other (see Table 1). Try both engines and determine which one works better for that specific STEP file.

Most users will use the traditional engine by default. In the 10 percent of cases where they are not satisfied with the end-result, the 3D Interconnect engine can be used, and most of the time users will notice an improvement. For that small group of users with their specific type of STEP files, the 3D Interconnect works best.

A STEP file you receive from a vendor will work better with one engine than the other, depending on how that STEP file was created. For example, what was the original CAD software and what export settings were used? Usually a vendor will maintain a particular procedure for creating STEP files. Therefore, the settings for importing one STEP file from that vendor would most likely work for every STEP file from that vendor.

Table 1. Traditional Import Engine vs. 3D Interconnect.

Design Changes in a Multi-CAD World

The amount of time SOLIDWORKS users spend working with STEP files varies based on how tightly they are integrated in a supply chain with multiple CAD solutions.

Lucky users simply download a STEP file once, covert it to SOLIDWORKS, save it in the library and use it as-is for a long period at time.

Unlucky users receive multiple revisions of models as STEP files during the development phase of a design. For these users, it is critical to minimize the time spent:

  • Identifying the changes between revisions, including Geometry, Topology, Location, Orientation, Number of bodies, Face and edge IDs and Metadata.
  • Updating the geometry.
  • Updating the mates of the component in all assemblies it is used.
  • Updating the metadata and revision data in a PDM system.

Consider the following scenarios (from simple to complex):

1. Download the model of a fastener from a supplier’s website to integrate in your assembly.

  • Once the model is converted, you can use it for a long time.
  • No revisions are expected.
  • This will be a one-time download and conversion exercise (with the proper use of a library system).

2. Receive a STEP file of a complete product from a customer, for manufacturing purposes.

  • The model can be used as-is, no modifications are to be performed by the SOLIDWORKS user.
  • The customer will revise the product and send new STEP files for each revision. The SOLIDWORKS user would need to check the differences between revisions.

3. Receive a STEP file of the concept of a product from a customer for development purposes.

  • The model cannot be used as-is. The geometry would have to be modified by the SOLIDWORKS user.
  • As the development progresses, the customer will revise the product and send new STEP files for each revision. The SOLIDWORKS user would need to check the differences between revisions.
  • After receiving a revised STEP file, the SOLIDWORKS user would like to minimize the work performed in modifying the geometry. Ideally, the changes performed by the user in Revision x should be preserved in the model after the STEP file was changed in Revision x+1.

4. Receive STEP files of components to be inserted in your assembly from a supplier during the development phase of your product.

  • The component will be inserted and mated in your assemblies.
  • As the design is being iterated, the vendor will revise the model and send new STEP files for each revision. The SOLIDWORKS user would need to check the differences between revisions.
  • After receiving a revised STEP file, the SOLIDWORKS user would like to have as many existing mates preserved, so no duplicate work would be required.

This article focuses on best practices for minimizing the time needed to update the geometry of components originated from revised STEP files and preserve or re-create their mates in assemblies. We will share with you:

  • What works well.
  • Work arounds for what does not work.
  • SPR numbers to help you vote for fixing problems.

To accomplish this, we will study several case studies following the same steps, for each import engine (traditional import engine and 3D Interconnect), using SOLIDWORKS 2020 SP 4.0:

  1. Revision 0 of a model is received from a third party as a STEP file.
  2. The model is imported in SOLIDWORKS.
  3. The model is inserted and mated as a component in an assembly.
  4. All files are saved and closed.
  5. Revision 1 of the same model is received as a STEP file.
  6. We will study how easy it is to update the geometry in the component file.
  7. We will study how easily the mates are updated in the assembly.

Case Study #1A–Unibody Part File Imported Using the Traditional Import Engine

Step 1: Import the file Gear, Cam – Rev.0.STEP using the traditional import engine (Figure 1). We were notified that the originating CAD file is not CATIA, therefore we did not check the B-Rep mapping box.

Figure 1. Importing using the traditional import engine.

The result is a part file containing one solid body, which imported without topological errors, as per the Import Diagnostic tool (Figure 2).

Figure 2.

Step 2: The part contains a solid body related to the Imported1 feature (Figure 3). Notice that there are no external references attached to that feature.

Figure 3.

Step 3: Save the part as Gear, Cam.sldprt.

Step 4: Insert the part as a component in the CamShaft.sldasm.

Step 5: Apply three mates to locate the component in the assembly (Figure 4).

Figure 4.

At this time, the revision 0 of the assembly is completed. In the next design iteration, it was determined that the torque needs to be increased, therefore the vendor revised the gear and a new STEP file was sent.

Since the traditional import engine does not create external references between the SOLIDWORKS file and the STEP file, many SOLIDWORKS users would simply import the revised STEP file into a new SOLIDWORKS part and overwrite the original file. That would create a lot of manual work. Luckily, there is a better solution.

Instead, we will attempt to edit the Imported1 feature and point it to the revised STEP file.

Step 6: Edit the Imported1 feature (Figure 5).

Figure 5.

Step 7: Select the Gear, Cam – Rev. 1. STEP file (Figure 6). Notice that the box Match faces and edges is checked. This setting ensures the propagation of the dependencies of the old faces and edges in the old body, such as sketches or features, to the new faces and edges in the new body.

Figure 6.

Step 8: Run the Import Diagnostic tool. Again, the result is a topologically  correct model.

Figure 7.

Step 9: Re-open the assembly CamShaft.sldasm.

Step 10: There are no errors. The IDs of the faces used as references in the mates have been preserved. This saves the user a lot of time, especially when the same part is used in multiple assemblies (Figure 8).

Figure 8.

Case Study #1B – Unibody Part File Imported Using 3D Interconnect

Step 1: Import the file Gear, Cam – Rev.0.STEP using 3D Interconnect (Figure 9).

Figure 9. Importing using 3D Interconnect.

Note: Once the Enable 3D Interconnect box is checked, the STEP file can be selected from the drop-down, to access extra settings (Figures 10 and 11).

Figure 10.

It is worth noting that with 3D Interconnect, extra settings become available regarding importing assemblies as multi-body parts (Figure 11).

Figure 11.

The result is a part file containing one solid body, which imported without topological errors, as per the Import Diagnostic tool (Figure 12).

Figure 12.

Step 2: The part contains a solid body related to a 3D Interconnect feature (Figure 13). Notice that there is an external reference attached to it. That should keep the link to the STEP file.

Figure 13.

Step 3: Save the part as Gear, Cam.sldprt.

Step 4: Insert the part as a component in the CamShaft.sldasm.

Step 5: Apply 3 mates to locate the component in the assembly (Figure 14).

Figure 14.

Step 6: Save and close all files.

At this time, the revision 0 of the assembly is completed. Like in the previous case study, in the next design iteration, it was determined that the torque needs to be increased, therefore the vendor revised the gear and a new STEP file was sent.

At this time, the SOLIDWORKS user has two options:

  • To overwrite the old STEP file with the new one.
  • To keep both files and update the link to the new STEP file.

Let’s try both.

Step 7: Replace the STEP file with the new one (same name, same location).

Step 8: Open the part file Gear, Cam.sldprt.

To our surprise, there is no indication on the part file that the STEP file was modified. Measuring key dimensions proves that the model was not updated yet (Figure 15).

Figure 15. We encountered a bug – the link to the STEP file does not work.

Problem #1:

This was unexpected. The external relation link does not seem to work as expected. The 3D Interconnect icon should have changed as per Figure 16. Then a simple Update Model command would have updated the geometry.

Figure 16.

We researched this issue and found out that SOLIDWORKS Technical Support is aware of the problem. It is recorded under “SPR 1180136: Non-native file inserted in assembly as 3D Interconnect feature does not show refresh icon (symbol) in FeatureManager Tree when its geometry is changed.”

At the time of writing this article, the status of this SPR was open. If you would like this fixed sooner, please vote on it.

Workaround #1

Step 9: Since the standard functionality is broken, let’s try the second option as a workaround: Edit the 3D Interconnect feature.

Figure 17. No indication that the link is out-of-date.

Step 10: Since the STEP file has the same name, we will simply select OK.

Figure 18.

Step 11: The model is updated, as proved by the measured diameter.

Figure 19. The part was updated.

It is time to test how robust are the existing assembly mates for a model revised using 3D Interconnect.

Step 12: Open CamShaft.sldasm assembly. All mates are failing (Figure 20).

Figure 20.

Problem #2:

We researched this issue and learned that this is a known problem. To have this fixed sooner, please vote on “SPR 1072694: 3D Interconnect – Ability to maintain the downstream features (mates) in a SW file when the linked STEP file’s geometry is updated.”

Workaround #2:

Instead of using faces and edges of the imported part as mate references, the user could create a set of reference entities inside the part to be used for mating purposes.

While those entities might lose reference when the part is updated with information from a revised STEP file, fixing them is simple and, more importantly, is only done once.

The main benefit of this workaround is that the mates will be preserved in all assemblies containing this part!

Preliminary Conclusions – Case Study 1 – Unibody Part

Conclusion #1 – Maintaining Links

The 3D Interconnect engine is supposed to eliminate the main limitation of the Traditional engine related to revisions of the STEP file, which is the absence of the link between the imported feature and the STEP file.

As we discovered in our study, currently there is a regression in the software (SOLIDWORKS 2020 SP4.0) that impacts this functionality. We provided a good workaround and also included the SPR number related to the problem. SOLIDWORKS users who are interested in having this problem fixed sooner, are encouraged to vote on the SPR.

Conclusion #2 – Maintaining Existing Mates

To our surprise, the Traditional Engine out performed 3D Interconnect in this area. We provided the SPR number related to the problem and encourage all users to vote on it.

Case Study #2A – Multibody Part File Imported Using theTraditional Import Engine

We are partnering with a customer in manufacturing a Movable Stair product. We expect the customer to send us multiple STEP files, one for each revision of the design.

For this case study we will focus only on geometry preservation, since we already know how mate preservation would happen with both engines (see Case Study #1).

Step 1:Import the file Stair_Fram_Rev0.STEP using the traditional import engine (Figure 21).

Figure 21.

The result is a part file containing 18 solid bodies. The Import Diagnostic tool did not identify any topological errors.

Figure 22.

Step 2: Save the part as Stair_Frame.SLDPRT.

We were informed by the customer that the design was revised. Two extra members were added to the weldment (Figure 23).

Figure 23.

Step 3: Edit one of the imported features, to read the revised STEP file.

Figure 24.

The result is unexpected. Instead of now having 20 solid bodies, we still have only 18—but one of them was replaced with a duplicate of another.

Figure 25.

Problem #3:

This is clearly not working as expected. We researched the problem and realized that SOLIDWORKS Technical Support was aware of it. They recorded it under “SPR 1187494 STEP – Export and Import – weldment part – changing the dimension of the structural member, the order of body will change once re-imported.”

Workaround #3:

Perform a manual replace of Imported Geometry as described in the following steps.

For users who work in a PDM system, it is important not to replace files, but rather to work with versions of the same file. This workaround was created for such users.

Step 4: Reload the file to undo step 3.

Step 5: Select all Imported features and move them to a new folder.

Figure 26.

Step 6: Name the folder “Rev. 0.”

Figure 27.

Step 7: From the Insert menu, select Features and Imported.

Figure 28.

Step 8: Select the new STEP file.

Figure 29.

Step 9: Select all new Imported features and move them to a new folder.

Step 10: Name the folder “Rev. 1.”

Step 11: Suppress the Rev.0 folder.

Figure 30.

The beauty of this workaround is that both revisions can be kept in the file. Configurations can be created. Some users would go even further and delete all the new duplicate features, leaving the old bodies untouched, so the mates would be preserved.

We will also use this technique as the basis for one of the solutions in the Comparison section of Article #3 in this series.

Case Study #2A – Multibody Part File Imported Using 3D Interconnect

Step 1: Import the file Stair_Fram_Rev0.STEP using 3D Interconnect (Figure 31).

Figure 31.

The result is a part file containing 18 solid bodies. The Import Diagnostic tool did not identify any topological errors.

Figure 32.

We were informed by the customer that the design was revised. Two extra members were added to the weldment (Figure 23).

Step 2: Edit the 3D Interconnect feature to point to the new STEP file.

Figure 33.

Figure 34.

The model updates correctly, as expected.

Figure 35.

Conclusion

Updating geometry correctly when STEP files are revised is a critical functionality for SOLIDWORKS users. In an ideal world, there will be two major expectations:

  1. The geometry will update correctly.
  2. The existing entities’ IDs will be preserved (face and edge IDs).

Currently the findings are mixed. For uni-body parts, the traditional import engine seems to be superior to 3D Interconnect. For multi-body parts, 3D Interconnect works better for the first condition (Table 2).

  Traditional Engine3D Interconnect Engine
 Link to STEP fileNoYes (1)
Unibody PartGeometry AccuracyYesYes
 Entity ID PreservationYesNo (2)
 Link to STEP fileNoYes (1)
Multibody PartGeometry AccuracyNo (3)Yes
 Entity ID PreservationNoNo (2)

Table 2.

  1. Current regression. Vote on SPR 1180136: Non-native file inserted in assembly as 3D Interconnect feature does not show refresh icon (symbol) in FeatureManager Tree when its geometry is changed.
  2. Current limitation. Vote onSPR 1072694: 3D Interconnect – Ability to maintain the downstream features (mates) in a SW file when the linked STEP file’s geometry is updated.
  3. Current regression. Vote on SPR# 1187494 STEP – Export and Import – weldment part – changing the dimension of the structural member, the order of body will change once re-imported.

The good news is that we have good workarounds for all these problems. Try them and let us know how well they work for you.

 

To be continued in:

Article #3 – Comparing Geometry Changes between STEP Revisions

Article #4 – Simplification Techniques for using Complex Imported Geometry in Large Assemblies

 

About the Author

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.

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