First Season’s greetings to all!
I want to expand my F360 modeling abilities. I am pretty good with the conventional modeling side but would like to expand my knowledge of mesh and more free-form modeling.
Last year on January 1 I jumped down the Primo world and this year I bought an Ender 3 v2 that I am loving. I love the availability of all the ideas on Thingiverse but really would like to be able to import into F360 to modify. I only have the non-commercial license and am a little confused about the process. I would also love to import some of Ryan’s primo models to practice the modeling of shapes.
Biggest hurdle is the conversion all of the holes are not converting very well. I can clean up the flat surfaces nice but circular faces are just prismatic.
Ironically, I have no interest in printing Primo parts as I could not be happier with the parts I bought from V1, and my 3D printing skills are at best sad. I can print 2 baby Christmas Yoda’s then the next print is a train wreck. so would not tackle a complex 17 hour print.
I don’t have an answer to the specific question you are asking here. I’ve watched several videos about importing and cleaning up STL files into Fusion 360, and the process has always seemed tedious, and the final result not super clean. But I do regularly use STL files as the basis for something I’m modeling in Fusion 360.
Dating back to the MPCNC Burly, I’ve recreated and modified about a dozen of Ryans parts. I bring the part into Fusion 360, and then use Fusion’s Mesh Section feature to take reference slices through the mesh. Recently the Mesh Sections tool has been moved to the Mesh/Create menu. Some of these Mesh Sections will be used to creating drawings for extrusion. Other are used as information on the placement of features.
A Mesh Section is just reference drawing. If you want to use the curves directly (like in an extrude) you have to recreate them in a sketch. The Sketch/Fit Curves to Mesh tool is designed to trace the curves of a Mesh Section. This tool is a bit complex and will take some ramp-up time. And don’t feel like you have to stick to the results from the tool. What is created is just arcs, curves, and lines, and can be edited or replaced or constrained like any other sketch geometry. As example, a drawing created using the “Fit Curves to Mesh” can capture fillets and chamfers on the STL. Typically, I’ll delete this geometry to create a sharp corner, then add the chamfer or fillet back in using the Solid/Modify tools.
I have sometimes worked with STL files directly (rather than use them as a reference). I first reduce the number of triangles as far as I can without losing functionality. Then I convert the result to a B-Rep (solid), and use Solid workspace tools to modify the converted object. As for the “prismatic” holes, you can model them away. In a sketch starting on the top surface, create circles centered on the hole, with one circle inside the hole and one outside. Using this sketch, extruded a walled cylinder to the bottom of the hole and Join it to the object. Then offset the inner face the cylinder to get your hole to the correct dimensions. Sometimes when I do things like this, I end up with artifacts (like the hole is skimmed over). I’ve always been able to just select the artifact and hit delete.
Great idea. I like this. I did experiment with the “Mesh Section” and see some potential but got a little stuck trying to use the geometry in the mesh section as you pointed out.
I watched some videos when they updated the Mesh workspace. The “prismatic” conversion option looks like magic when converting STL files to solids, but unfortunately it is only available in the paid version. Sigh.
