Combine Objects from STL

[Anonymous]

I have two STL files that represent 1 objecct but are two pieces for 3D printing since the single piece is large.  I want to open both STL files and combine them into a single body/component.  I've tried everything I can think of from "Uploading" the STL file to importing it and it seems because these are mesh bodies I can't combine them.

Any thoughts?  I an a TOTAL noob at this. 🙂

Paul

[ToddHarris7556]

While there may well be a workflow to accomplish this in Fusion, it's possible that Meshmixer might be a more appropriate tool - this is one of MM's core strengths.  

[Anonymous]

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@ToddHarris7556 wrote:

While there may well be a workflow to accomplish this in Fusion, it's possible that Meshmixer might be a more appropriate tool - this is one of MM's core strengths.  

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Cool, I'll give it a try.

[ToddHarris7556]

OK, I noodled around with this for a bit. I'm no STL expert, but here are a couple of thoughts:

1) I would have thought that Meshmixer and/or  Recap could be used to convert/merge/remesh these files into something more usable, but I really didn't have any luck. 

2) Recap can be used to export to OBJ/Quads, but you lose a bunch of detail, and I'm not sure how usable it really is. 

3) Just FYI... the two STL files don't actually match up - the bottom ledge is different. 

4) I actually had the best luck following THIS workflow.... essentially just remodeling the geometry in Fusion. This is really a pretty simple shape, so it goes (relatively) quickly. Basic steps are:

• import the STL.
• create mesh sections (slices). These still aren't actually useful, but can be referenced.
• use 'Fit curve to section' to manually drop sketch entities onto the sections. 
• The tools are maybe a bit clunky, (seems like you need to restart the fit curve command pretty much for every entity you place) but they do work. There were a couple of corners that took a little bit of fudging to get a closed profile, but in general, it worked pretty well.
• a handful of sections seemed like it was enough to make the three extrudes required. I then mirrored the body to create the other half. 
• For kicks, I pulled the other (right) STL in for comparison. You can turn it on or off to see the discrepancy. 

Revised part attached. Hope this helped. I wasn't quite sure, so I wanted to dig in and learn this workflow anyway. 

[ToddHarris7556]

Well, you learn something new every day. If you're lucky, maybe a couple of new things 🙂

I just found THIS workflow, that really worked liked a charm. I'm not sure how much is going on behind the scenes, but it appears to be pretty quick & accurate. In a nutshell:

1. import STL
2. In the PATCH workspace, Modify>Mesh>Mesh to BRep.
3. still in PATCH, use Modify>Merge, select chain, and click on planar face to clean up all the triangles. 

It looks like it results in perfectly usable solid bodies in about a dozen clicks. 

[TrippyLighting]

You don't even have to merge faces. You can simple select a triangular face that is coplanar with another face and hit the delete key. Fusion will auto heal that surface and maybe auto heal adjacent faces that are coplanar.

But, here's the catch - there3 always is a catch - if the faces are not complainer and there is slight curvature to the shape Fusion might still auto-heal the surface but it will change the curvature of the surface. That is sometimes not desirable so look out for that.

Fusion 360 uses some internal tolerance to be able to do this, but it does no reveal that tolerance to the user or provide any feedback that tells the user what it is doing. That's the danger.

[ToddHarris7556]

I did run into that, Peter, thanks!

I started off deleting faces, but then, as you say.... one misstep, and suddenly you've turned the body into a surface body with a hole in it. My gut says that it's safer to let Fusion figure out whether it's coplanar  or not. The merge face/chain option seems to do that. 

When it comes to smoothing filleted corners, I'm still not sure I understand the algorithm - I'm not sure if it's more dangerous to start merging long arc faces, or just leave well enough alone. In any event.... they both seem like a perfectly usable workflows. 

Slice/fit/sketch and remodel if really clean geometry is needed.

Convert/merge/heal to simply get a usable solid. 

[TrippyLighting]

How did you get the fillets to merge as cleanly as you have in the model you attached to a previous post ?

[ToddHarris7556]

That was modeled from scratch using the mesh section/fit curve workflow. It's little more work, but gives cleaner geometry. One section/sketch gets the basic body shape, then one orthogonal slice gives you top and bottom construction planes to use as extrusion boundaries. Repeat that again for each of the two ledger rails. (And I realized after that I missed the top end of the side rail being angled)

In any event.... 3 sketches, a few construction planes and 3 extrudes.

I'm not sure I can think of a use for the mesh section alone, unless it was going to be followed by a 'fit curve' step, so I would think this is a great opportunity for optimization down the road. 1-click editable mesh sections.

[TrippyLighting]

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@ToddHarris7556 wrote:

That was modeled from scratch using the mesh section/fit curve workflow. It's little more work, but gives cleaner geometry.

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Aha! I thought there was some black magic beyond my grasp involved 😉

[ToddHarris7556]

So the black magic aspect that *I'm* trying to figure out is : is there a practical difference between the two workflows?

My gut says that the remodeled geometry is cleaner/more robust/more stable vs the cleaned-up/merged mesh, but a) I wonder if that's really true and b) to what extent? i.e. when is it worth the extra effort to remodel?