In the electronics industry, engineers regularly rely on STEP files to share 3D data between customers and external suppliers of components like cables, battery packs, machined parts, and more.
While these neutral files are great for collaboration, engineers who primarily use SolidWorks experience difficulties when trying to examine an individual part in a STEP file with multiple components or need to alter a design that has been sent to them in the STEP file format. Instead of clean, editable features, you’re often left with “dumb solids” or complex surface bodies that can be difficult to modify and integrate into larger assemblies.
Converting these STEP files into workable SolidWorks models is simple, but also vital for the engineer to learn when dealing with these STEP files daily. Whether you’re comparing the geometry and overall dimensions of components on a PCB or taking apart the STEP file of a keyboard to inspect each key, knowing how to get these clean, parametric models makes all the difference.
In this post, we’ll walk through the steps on how to properly import a STEP file into SolidWorks, what all the settings in the import and export menus mean, and then how to properly export the model back to a STEP file to send back to the customer or supplier.
Why Would Engineers Need to Know This?
STEP files are one of the most common formats used for sharing mechanical data across different CAD platforms. Whether the file comes from a connector manufacturer, a cable supplier, or a customer design team, it is almost always provided as a neutral format to communicate the scope of the design.
The challenge is that STEP files don’t keep the original “recipe” of how the model was built, which makes them harder to edit or adjust later if needed. When opened in SolidWorks, they typically appear as imported bodies without sketches, dimensions, or feature trees.
This creates several issues:
- Difficult to modify geometry such as holes, fillets, or cutouts.
- Challenges when checking interference, fit, or alignment.
- Extra time required to recreate features manually.
- Difficulty when separating parts from a complete assembly.
For engineers working with custom components like overmolded cables, battery packs, machined enclosures, or any complicated assembly, being able to convert these files into usable SolidWorks parts speeds up and simplifies the design review process.
Steps
1. Opening Up Through SolidWorks
The first step is importing the STEP file correctly. Open SolidWorks and go to File → Open, then select the appropriate STEP file from the pop-up window.
Before opening the file, click on the Options button.
This can also be performed through SolidWorks at any point by selecting “Options” from the drop-down menu of the gear icon in the top toolbar.
Select the “Import” option from the left-hand column, then make sure the file format dropdown is set to STEP/IGES/ACIS so that the correct settings are seen.
Inside the import options, you can choose how SolidWorks handles the geometry. If the STEP file contains multiple components, importing it as an assembly is usually the best option. This allows each component to be handled individually, making it easier to isolate and convert specific parts.
With the correct menu and file type selected, the next step is to understand what each of these import settings actually does and how they impact the quality and usability of your model.
2. Definitions of Import Settings
Understanding the import settings is key to getting a usable model. Several options directly affect how editable the part will be.
These settings are as follows:
Entities to Import
- Solids and Surfaces - Whenever possible, import as a solid body. Surface bodies are more difficult to work with and often require additional steps to knit or repair before they can be used.
- Try Forming Solid(s) - This option attempts to automatically convert surfaces into solid bodies. It is useful for improving model usability, especially when working with complex geometry.
- Do Not Knit - This prevents SolidWorks from trying to combine surfaces into solids.
- Free Curves and Points as Sketch – Imports any standalone curves, edges, or points as 2D/3D sketches.
- Reference Planes – Imports any planes that were defined in the original CAD model.
- User Define Attributes – Imports metadata attached to the model (like part numbers, material info, or custom properties).
- Assembly Structure Mapping
- Default - Imports the model exactly how it was structured in the original file.
- Import Multiple Bodies as Parts - If the STEP file contains multiple solid bodies, SolidWorks converts each body into its own individual part within the assembly.
- Import Assembly as Multiple Body Part - Brings the entire assembly in as one single part file with multiple solid bodies inside.
- Automatically Run Import Diagnostics - This tool checks for gaps, missing faces, or geometry errors. Running diagnostics immediately after import helps clean up the model and ensures it behaves properly in later operations.
- Create Analytic Faces - Converts complex surfaces into simpler, mathematically defined shapes (planes, cylinders, cones, etc.).
- Feature Recognition - One of the most powerful tools in SolidWorks is FeatureWorks. After importing a STEP file, you can use Feature Recognition to identify features such as holes, fillets, and extrusions. While it does not always recreate a perfect feature tree, it can significantly improve editability.
- Unit of Import
- File Specified Unit – Uses the units already defined in the STEP file.
- Document Template Specified Unit - Forces the model to use your current SolidWorks document units.
Options
By taking the time to adjust these settings, you can often avoid hours of manual cleanup later in the process.
3. Converting to a Workable SLDPRT File
Once the STEP file is imported and cleaned up, the next step is making it usable.
If the file was imported with multiple bodies as parts, you can review the full assembly and isolate recognized parts, but you will not be able to edit them in a standalone file. It helps when you need to identify certain parts or sub-assemblies within a larger assembly.
If the file was imported as a multiple body part, you can isolate the specific body or part you want to review or revise and save it as a separate SLDPRT file. To do this, you will need to find the correct solid body of the model, which can be found in the part tree of the model under the Solid Bodies folder. From here, right-click on the appropriate Solid model, then select “Insert into New Part...” to open this part in a new SolidWorks window.
From here, you can begin refining the model:
- Use Feature Recognition to identify editable features
- Add reference planes, sketches, and dimensions as needed
- Rebuild critical geometry if required for full parametric control
Once your model has been refined into a clean, usable SLDPRT file, it’s often necessary to share it with suppliers or other teams. The next step is understanding how to properly export your SolidWorks model back into a STEP file while preserving the key geometry and data.
4. Exporting a SLDPRT File Back to a STEP File
Once modifications are complete, it is time to export the SolidWorks file back to a STEP format.
Go to File → Save As, then you can choose between different STEP standards such as AP203 or AP214. AP214 is typically preferred because it supports additional data such as colors and layers.
Several options directly affect how editable the part will be once the end user opens the file back up.
These settings are as follows:
Output As
- Solid vs Surface - Whenever possible, import as a solid body. Surface bodies are more difficult to work with and often require additional steps to knit or repair before they can be used.
- Wireframe – Exports only edges and curves—no solid geometry.
- Set STEP Configuration Data – Exports configuration-specific data (like different part configurations).
- Export Face/Edge Properties – Preserves additional geometric details like face and edge IDs.
- Export Appearances – Includes colors, textures, and visual properties.
- Export 3D Curve Features – Exports 3D curves (like routing paths or complex curves).
- Split Periodic Faces – Breaks up continuous curved faces (like cylinders) into smaller segments.
- Export Assembly Components as Separate STEP Files – Exports each component as its own STEP file instead of one combined file.
Once exported, it is good practice to re-open the STEP file and verify that the geometry translated correctly.
Summary
Working with STEP files is unavoidable in modern engineering workflows, especially when collaborating across multiple suppliers and design teams. While these files are not inherently editable, SolidWorks provides several tools that allow engineers to convert them into functional models with a reasonable level of control.
By understanding import settings, using feature recognition tools, and applying proper cleanup techniques, engineers can significantly improve efficiency and reduce design friction. With practice, converting STEP files into workable SolidWorks parts becomes a quick and reliable part of the design process.
Key Takeaways
- STEP files are widely used for sharing 3D data but do not retain parametric features, making them difficult to edit directly in SolidWorks.
- Proper import settings, especially selecting solid bodies and running diagnostics, can significantly improve model usability.
- Feature recognition tools can help rebuild editable features, reducing the need for complete model recreation.
- Converting assemblies into individual SLDPRT files allows for better control and easier integration into larger designs.
- Always verify exported STEP files to ensure geometry integrity and compatibility with customers or suppliers.
