Convert STEP to SLDPRT
SolidWorks opens STEP files directly, and Save As gives you the .sldprt. What you get is the exact shape as a single imported body, with no feature tree behind it — and one setting, 3D Interconnect, decides whether the new part stands on its own or stays tied to the STEP file it came from.
We cannot write .sldprt files. The format is closed, so only SolidWorks saves one, and no converter outside SolidWorks produces a real part file. We do read STEP, so if the aim is a mesh for printing or a model to look at, that part runs here.
Opening a STEP file in SolidWorks and saving a part
Written for SolidWorks 2022 and later.
Open the STEP file
File → Open → file type: STEP AP203/214/242 (*.step;*.stp)
Choose the file. SolidWorks reads all three application protocols, and .stp and .step are the same format under two names.
Decide whether to keep the link
Tools → Options → System Options → Import → Enable 3D Interconnect
With 3D Interconnect on, which is the default in recent versions, SolidWorks does not translate the STEP file so much as reference it. The part updates if the STEP file changes, and it breaks if the STEP file is moved or deleted.
For a file you were sent once and want to own, this link is a liability. Either switch the option off before opening, or keep it on and break the link in step four.
Let it open, and read the tree
FeatureManager → Imported1 (or the STEP file’s name, with a link arrow)
A single part arrives as one imported feature. An assembly arrives as a SolidWorks assembly with a part for each component, which is the case covered further down.
Break the link, if there is one
Right-click the imported feature → Break Link
The geometry is copied into the part and the tie to the STEP file is cut. After this the .sldprt is self-contained and can be sent anywhere without the original beside it.
Run the import check
Right-click the imported feature → Import Diagnostics…
SolidWorks lists any faulty faces and any gaps between faces. Attempt to Heal All repairs most of them. A STEP file from another CAD system often has a few, and they are much cheaper to fix now than when a fillet fails later.
If the tree shows a surface body instead of a solid body, there is a gap somewhere and the shell did not close. Import Diagnostics is what finds and closes it.
Save as a part
File → Save As → Save as type: SOLIDWORKS Part (*.prt;*.sldprt)
That is the .sldprt. It holds the exact geometry from the STEP file as one body, ready to be modified with new features on top.
What you get: the shape, without the history
A STEP file carries finished geometry. Every cylinder is a true cylinder, every fillet a real blend surface, and the part measures exactly as it did in the program that made it. That is a great deal more than a mesh gives you, and it is why STEP is the format to ask for.
What it does not carry is how the shape was built. The original author’s sketches, extrudes, patterns and dimensions belong to their CAD program’s own history, and STEP was never meant to move them. So the FeatureManager shows one entry, and there is no dimension to double-click.
You can still do nearly everything. New features go on top of the imported body: cut it, add bosses, drill holes, fillet edges. Direct editing covers a lot of the rest — Move Face shifts or offsets faces of the imported body, and Delete Face removes a fillet or fills a hole. For a part that needs one hole moved, that is quicker than having the history would have been.
Getting features back with FeatureWorks
FeatureWorks is the SolidWorks tool that looks at an imported body and tries to work out which features would have produced it. It is under Insert, FeatureWorks, Recognize Features, and it comes with SolidWorks Professional and Premium rather than Standard.
It recognises the regular things well: extrudes, revolves, holes, simple fillets and chamfers, linear and circular patterns. On a bracket or a turned part, automatic recognition can rebuild most of the tree, and the result has real dimensions you can change.
It does poorly on anything organic or heavily blended. When automatic recognition stalls, the interactive mode lets you point at faces and say what they are, which gets further but takes patience.
The honest summary is that FeatureWorks is worth five minutes on a prismatic part and not worth an afternoon on a casting. For a complex part, modelling new features on top of the imported body is usually the faster road.
STEP assemblies
A STEP file can hold an entire assembly: every component, its geometry, its name and its position. SolidWorks opens that as an assembly document with a part for each component.
With 3D Interconnect on, those parts exist only as references into the STEP file until you break the link or save them out. To get a normal set of files, right-click the top of the tree, choose Break Link or Dissolve Feature, and then save the assembly. SolidWorks writes the .sldasm and one .sldprt per component into the folder you pick.
Positions come through as fixed locations rather than mates. The parts sit where they should, and nothing holds them together in the SolidWorks sense, so the first thing dragged will move alone. Add mates where you need motion, or leave everything fixed if the assembly is only a reference.
If you do not have SolidWorks
Then there is no route to a .sldprt, and it is worth asking whether you need one. Whoever asked for "the SolidWorks file" usually wants something SolidWorks can open, and a STEP file is exactly that. Sending the STEP is not a lesser answer; it is what the format is for.
If what you need is to use the model yourself — to print it, look at it, or measure it — the STEP file is already enough. It converts to STL, 3MF, OBJ or GLB on this site, in your browser, with a setting for how finely the curved surfaces are meshed.
And if you are starting from a mesh rather than a STEP file, the conversion to STEP runs here too. SolidWorks opens the result as a faceted solid, which is a different and more limited thing than a real STEP import, and the page for that conversion says exactly how.
Where we can actually help
We read STEP in the browser with a real CAD kernel, so everything that is not SolidWorks-specific runs here: a mesh for printing, a GLB to show somebody, or a STEP solid made from a mesh for SolidWorks to open.
Questions
- How do I convert a STEP file to SLDPRT?
- Open the STEP file in SolidWorks with File, Open, then use File, Save As and choose SOLIDWORKS Part. If 3D Interconnect is on, right-click the imported feature and choose Break Link first so the part is self-contained.
- Is there an online STEP to SLDPRT converter?
- Not a genuine one. Only SolidWorks writes .sldprt files. Anyone with SolidWorks can open your STEP file directly, so sending the STEP file is normally all that is needed.
- Why is there no feature tree after importing?
- STEP stores the finished shape, not the steps that built it. You get one imported body with exact geometry. FeatureWorks can recognise simple features on it, and new features can always be added on top.
- My STEP file opened as surfaces, not a solid.
- There are gaps between faces, so the shell did not close. Right-click the imported feature, open Import Diagnostics, and use Attempt to Heal All. Once the gaps close, SolidWorks knits the faces into a solid.
- What is 3D Interconnect and should I turn it off?
- It makes SolidWorks reference the STEP file instead of translating it, so the part updates when the file changes. Leave it on for files that will be revised; break the link or turn it off for a file you want to keep as an independent part.
Where to go next
Related guides
Tools that do part of this here
About these formats
Checked against current software versions on 2026-10-09