15 cose da sapere prima di importare file CAD in Onshape

Importing into Onshape is honestly pretty painless once a few things click. Most files don't land perfectly on the first try, and that's completely normal – what matters is knowing the fix.

Sometimes that means picking the right format before the import even happens. Sometimes it means knowing exactly which command turns a part with no flat pattern, no features, or a gap in the middle of a sketch into something usable in no time at all.

Here's the full rundown, grouped by what's actually happening at each stage:

• Formats and File Types
• Assiemi
• Lamiera
• Sketches
• Direct Editing
• Beyond the Basics

Formats and File Types

1. Native Files Work Just Fine

There's no need to convert anything before importing. Onshape reads SOLIDWORKS, Inventor, Pro/E, Creo, NX, and CATIA files directly, so the file can just be dropped in as-is.

CATIA parts are a nice example of why that matters – opening them elsewhere, in SOLIDWORKS for instance, reportedly calls for an extra purchase, while Onshape handles them right out of the gate.

2. Parasolid is a Great Fallback

When native isn't available, Parasolid (.x_t) is the next best thing. It's the modeling kernel behind Onshape itself, and it also powers NX, Solid Edge, SOLIDWORKS, and Shapr3D, so there's a good chance whatever system is being left behind can produce one.

It's a smart move for another reason too: Parasolid files tend to come in smaller than a native archive, which is handy if a project is nudging up against the size limit.

3. For Generic Formats, STEP is It

Between IGES and STEP, STEP is generally the better choice. It's the newer of the two, and newer tends to translate more cleanly.

Creo is a fun exception worth remembering: based on some digging through Onshape's internal notes and the STEP documentation, Creo data often comes in cleaner as STEP AP242 than through its own native format. If a native Creo import isn't cooperating, that's the first thing worth trying.

4. The Size Limit is 4 GB

If an import is bumping up against that ceiling, a few options work well: strip the drawings and simulation results out of the Pack and Go before zipping it, bring the assembly in subassembly by subassembly instead of all at once, or export to Parasolid instead, since it tends to produce a noticeably smaller file.

Assiemi

5. Pack and Go is the Whole Game for SOLIDWORKS Assemblies

Exporting a SOLIDWORKS assembly part by part is a lot of unnecessary work, and it's an easy way to lose a reference along the way. Pack and Go solves that in one move – it bundles everything into a single zip that imports cleanly, with every reference intact. Inventor has its own version of the same idea in its zip archive.

6. Leave the Drawings Out of the Export

When prepping that Pack and Go, it's worth skipping the drawings. They'll almost certainly get recreated directly inside Onshape anyway, so leaving them out keeps the file lean and comfortably under that 4 GB mark.

7. Reorienting a Part is Quick

A model that comes in facing the wrong way is nothing to worry about. Inside a Part Studio, the fix is Transform to Rotate – and if there's no obvious edge to use as an axis, dropping in a mate connector works just as well.

Inside an assembly, it's even easier: just select the part, grab the triad, and rotate it into place, especially handy with constrained orbit turned on. And if the source system uses Z-up instead of Y-up, there's an option at import time that flips that automatically.

8. Decide What the BOM Should Say

Once an assembly lands, two tools shape how it shows up in the bill of materials.

Dissolve Subassemblies flattens the hierarchy so every component gets its own line, without breaking any mates already in place.

Composite Part does the opposite – it rolls a subassembly into a single BOM line while keeping the motion intact, a great fit for a purchased assembly nobody's planning to manufacture.

Sheet Metal

9. Reach for Thicken

Imported sheet metal almost never comes in with a flat pattern ready to go, and getting one means reaching for the sheet metal model tool. The command that actually does the job is Thicken, not Convert, even though Convert looks like the obvious pick.

One extra setting makes all the difference: turning on tangent propagation, along with Include Bends, lets the operation follow the bends all the way around the part instead of stopping at the first face. Get those right and a full flat pattern shows up in well under a minute – from there it's a quick right-click to export a DXF and send it off to the laser or waterjet.

Sketches

10. DXF Import Happens Inside a Sketch

It's easy to look for a DXF import in the main import menu and come up empty, since it actually lives inside a sketch. The move is to start a sketch, choose a plane, and select Insert DXF or DWG from there.

11. The First Dimension on a DXF Scales

DXF files come in unitless, the same challenge as an STL. The fix is simple: add one known dimension right after the sketch lands, and the entire sketch scales to match it.

That trick only applies to the very first dimension – everything added after behaves normally, so it's worth setting the scale before making any other changes.

12. Use the Sketch Diagnostic Tool

Converting a bitmap logo to a vector in Inkscape or Illustrator, in order to emboss or deboss it onto a part, can sometimes leave small gaps in the profile. The giveaway is an extrude that grabs the outer shape of a letter but skips the interior – the middle of an O, the counter of an A.

The sketch diagnostic tool's profile inspector tracks down every loose end and zooms right to it. Some close with a quick drag of an endpoint, and for messier ones, deleting the segment and drawing a fresh line that snaps into place is often the faster fix.

Direct Editing

13. A Missing Feature Tree Isn't a Dead End

Every so often, a part imports clean with an empty feature list, and that's no problem at all – direct editing works straight on the geometry, no history required.

Move Face is the one to reach for most often: box-select the faces of a boss or rib, switch from the default Offset to Translate or Rotate, and slide things into place. Delete Face clears out fillets and other features cleanly, as long as Heal is selected – Heal sharpens the corner back into a clean edge, ready for a new fillet, while leaving it open turns a solid into a surface. Modify Fillet rounds out the toolkit for adjusting radii in place.

A couple of quick habits pair nicely with all of this: pressing Y hides planes fast when they're cluttering the view, and the search bar is more forgiving than it looks – typing "rotate," for instance, still points straight to Transform.

Beyond the Basics

14. Use Kestrel for Bulk Migration

For migrating an entire SOLIDWORKS library rather than a handful of files at a time, Kestrel is a free desktop app in the Onshape App Store, built with partner SmartBench Software. It migrates data in bulk, prevents duplicates, preserves metadata, and brings drawings over as PDFs.

For a big legacy library, it's a genuine time-saver. For a handful of active parts, the manual route above is still the quicker path.

15. The Learning Center Has a Lot More

For anyone who wants to go deeper, the Onshape Learning Center is free and worth bookmarking: self-paced courses cover both importing/exporting data and direct editing, there's an article specifically on bulk importation, and the tech tips section is a great rabbit hole for anything not covered here.

Some Useful Tech Tips

• Suggerimento tecnico: come importare ed esportare con Onshape
• Suggerimento tecnico: come importare e modificare la geometria CAD 3D in Onshape
• Tech Tip: Which Onshape Import Option to Use and When?
• Tech Tip: Importing Standard File Formats into Onshape
• Tech Tip: Importing Assemblies
• Tech Tip: 3 Ways to Import CAD Data into Onshape
• Tech Tip: Importing and Exporting DXF Files
• Tech Tip: How to Use the Group and Fix Tools When Importing Models Into Onshape
• Tech Tip: How to Start a Sketch with an Imported Image
• Suggerimento tecnico: configurare la geometria importata in Onshape
• Suggerimento tecnico: importare metadati tramite la distinta base di Onshape
• Tech Tip: How to Repair Imported Models in Onshape
• Tech Tip: Updating Imported Geometry
• Tech Tip: Shift-Select When Importing Files
• Tech Tip: How to Maintain References on Updated Imports