Converting .3dm into a Soildworks compatible file type?

I have been recently doing some work for a client who is wanting to take my Rhino .3dm file into Solidworks and continue the development of the CAD.

I have searched on the boards to try and find the answer but I haven’t found a definitive answer, I know that Solidworks supports multiple file types for importing, I’m just not too sure which is best. The Rhino file is mainly Polysurfaces with 1 or 2 mesh objects. It isn’t the end of the world if the mesh objects aren’t supported by the file type which best supports polysurfaces.

Any insights would be much appreciated. At the moment I am thinking .IGES is the best option?


IGES seems to work best for us. SW can actually import 3DM files as well. Why not do all files you can think off and send over? Next time you will know what worked. As a client it’s pretty annoying having to get back to the designer and tell them the file didn’t import.

When you save out as an IGES file in Rhino you can select what IGES type you want and can choose Solidworks Solids as your type.

In Solidworks 2012 (and maybe older editions) you can actually run a feature recognition once you import the file and it can often recognize basic features like extrudes, revolves, chamfers, fillets, etc. and it will rebuild a feature tree so that you can readjust in SW. It works pretty great with some models.

Your application sounds pretty straightforward but this is actually a complex topic. Translation of mesh formats to Solidworks is a constant battle and some cases are easier than others.

Getting your Rhino surfaces into Solidworks won’t be difficult, try Parasolid/STEP/IGES.

The mesh parts are tough but not impossible. Here are some options:

  1. SW STL import - Export your mesh as an STL file. In SW, choose File → Open then for file type, select STL. Click Options, and then check the button for “Surfaces.” This will attempt to convert your mesh to surfaces on import. There is a cap on the # of polygons it can handle.
  2. DXF import - Export an STL. Download freeware called MeshLab and open the file, then save as DXF. Import into SW and choose the option to open as a 3D file.
  3. Rhino MeshToNurb command - In Rhino you can convert a mesh to a series of surfaces. This is a heavy-handed solution, as it simply places one surface per polygon. But it can be useful to export this massive polysurface and then use it as a reference to rebuild a more elegant surface.
  4. Other plugins - If you find yourself doing mesh imports often, it might be worth getting the ScanTo3D module from SW, or a 3rd party plugin such as Power Surfacing or T-Splines. All of these plugins have ways to convert meshes to surfaces.

Solidworks will open and Rhino4 .3DM file – it doesn’t want to open Rhino5 files. So, save as RH4 and you should be good to go.

Thank you for the responses, I have sent a igs and a Rhino 4 3dm.