Regardless of what CAD software you work with, at some point you will be confronted with the need to import a STEP file. SOLIDWORKS 2024 offers some much-needed improvements in the process for STEP files.
STEP stands for Standard for the Exchange of Product Data and is also known as ISO 10303. As a common file format used for 3D modeling and printing, these files are an ISO standard exchange format. This means that STEP files can read and save the complete body of a 3D model — not just the basic geometries — which is necessary for high levels of accuracy.
All the 3D model data is saved as text that various CAD systems can interpret. STEP files make it easy to create, share and edit 3D models across many different programs and software in a standardized format.
Let’s open a STEP file to view the text. It can be informative.
You can see that the file was originally created in Creo and which version of Creo was used. You also see the author of the file. The remainder of the file are basically directions on how to re-create the geometry of the Creo file.
STEP files are considered neutral or agnostic as they can be read by any CAD software. Many companies will require that you save files as a STEP file and upload it into their PDM system, so that they can be sent to vendors or in the event the CAD software the company uses is changed.
The first step before importing any STEP file is to review your Options Import settings.
There are two places where you control the behavior of the import. One is in the General File Format:
If 3D Interconnect link is enabled, you can:
- Insert proprietary CAD data directly into a SOLIDWORKS assembly without converting it to a SOLIDWORKS file.
- Open the proprietary 3D CAD format in the SOLIDWORKS software with its associative link to the original part.
- Update changes in the SOLIDWORKS file if you update the proprietary CAD data in its authoring application by maintaining all downstream features created in SOLIDWORKS.
- Break the link of the inserted part file with the original part file.
This is useful if you are using SOLIDWORKS integrated with a PDM system because you won’t be cluttering up your PDM with linked STEP files, only with the converted file.
If you enable Feature and Component level, SOLIDWORKS will display the component links and feature links with an arrow symbol on each component and feature in the Feature Manager design tree after import. This allows for easier editing. If this is disabled, then the STEP file will come in as a single item with no expandable features or components.
Select STEP/IGES/ACIS from the drop-down list.
I did a quick poll on LinkedIn to see whether users prefer importing as parts or as a multi-body part, and the answers were interesting.
I prefer to import as parts because it makes it easier to organize a large imported assembly, but many users said they preferred to import as a multiple body part as it makes editing easier.
I will show you an example using the same STEP file so you can determine which method you would prefer and how the results differ.
If you enable Automatically run Import Diagnostics (Healing), SOLIDWORKS will automatically try to repair any gaps or missing faces.
I normally disable this because I want to inspect the imported file first, and depending on the imported file, the diagnostics can take some time. So, you might sit there for a significant amount of time while SOLIDWORKS attempts to make repairs. Several times, I have imported a STEP file, waited several minutes for the Import Diagnostics to go through and then, after looking at the STEP file, decided I didn’t like the file at all and opted to use something else.
When you open a STEP file, you have a second opportunity to check the Options in case you forgot earlier or if you want to change the settings for that specific import.
I imported this STEP file using the create feature and component level enabled, as well as import multiple bodies as parts. This is a single part, so SOLIDWORKS created a single body and a single part.
Note that the STEP file is retained as a link.
I enabled “Import assembly as multiple body part” for this file.
This created 37 solid bodies in a single part file.
Let’s say I wanted to move this bracket’s location.
I would need to locate which of the 37 solid bodies define the bracket in the Feature Manager.
Once I have located it, I will rename it in the Feature Manager so I can locate it easily.
With the desired body selected, go to Insert > Features > Move/Copy.
Input the desired value in the correct direction and green check.
To delete a body, locate it in the Feature Manager.
With the desired body selected, go to Insert > Features > Delete/Keep.
Going through the feature tree, these three solid bodies represent the hardware at the bottom of the structure:
It would be nice if I could combine them into a single body, but SOLIDWORKS gives me an error when I attempt a Combine.
I also can’t create a folder to organize the bodies because it is a single part file.
I imported the same file using the Import multiple bodies as parts option, so you can see the difference. SOLIDWORKS automatically organized files into sub-assemblies and parts.
SOLIDWORKS also was able to identify each part and assembly from the STEP file and rename the files so they are easier to identify.
Each sub-assembly/part is automatically fixed in place.
To move the plate, it is easier to identify in the browser.
Simply right click and change to Float, then you can then drag it to desired location.
If I want to modify the plate, I can open it up as a separate file and use Feature recognition to make it more editable.
Be sure to look at the FeatureWorks options before you proceed to define how you want the operation to proceed.
You can opt to overwrite the file you are translating or create a new file.
You can add dimensions and constraints to the sketches that are created.
You can have any holes reproduced using the Hole Wizard.
I identify the part as a sheet metal part and select the front face as the fixed face to act as the base feature.
Even though I told SOLIDWORKS it was a sheet metal part, SOLIDWORKS translated a Boss-Extrude as the primary feature.
SOLIDWORKS also added an unnecessary plane.
I deleted the unnecessary plane and moved the sketch for the Boss-Extrude to the Front Plane. I assigned 1060 Alloy as the material.
To use the new feature-based part, I need to use the Replace command inside the assembly.
The hardware that I couldn’t combine when it was imported as a multi-body part is now a single part and is identified with the correct McMaster part number.
Here’s another example of a workflow using an imported STEP file.
I am working inside an assembly and want to bring in a STEP file. I can use Insert Components because I have 3D Interconnect enabled.
Enable Float for the inserted part in order to have the freedom to assign my own mates.
Select Browse to locate the desired STEP file.
The STEP file is imported and appears in the Open documents list. I select it and insert it into the assembly.
It comes in as a solid body inside a part file. Open the part file.
Before I can use FeatureWorks, I have to break the link to the STEP file.
Highlight the part, right click and select Break Link.
Once you break the link, you can’t undo the change. However, you still have the original STEP file, so you can always start over, if needed.
Now that the link is broken, FeatureWorks is available so you can translate the features.
That said, FeatureWorks does not always do a great job recognizing and translating features. About half the time, I end up re-creating the part from scratch or using the Move/Copy/Delete Body tools to get the part where I want it to be.
Most vendors have a STEP file of their products available as free downloads.
I also will search on Traceparts, 3DContentCentral and GrabCAD when I am looking for parts. These are great resources and worthy of bookmarks in your favorite browser.
You must have a SOLIDWORKS Professional, SOLIDWORKS Premium or SOLIDWORKS Office to use Task Scheduler.
If you have multiple STEP files, you can use the Task Scheduler to batch process them.
Task Scheduler displays the progress as it creates the files.
About the Author
Elise Moss is a mechanical design engineer, currently working in Silicon Valley. She has been using SOLIDWORKS since 1998 and uses it daily in her current work. She holds a BSME from San Jose State University. She has written articles for Autodesk’s Toplines magazine, AUGI’s PaperSpace, DigitalCAD.com and TenLinks.com. She has taught CAD classes at Laney College, DeAnza College, Silicon Valley College and for Autodesk resellers. Laney College has recently named her as Professor Emeritus. Autodesk has named her as a Faculty of Distinction for the curriculum she has developed for Autodesk products. She is a Certified Autodesk Instructor as well as a Certified SOLIDWORKS Educator.