How to create a joint or lip on model's shell to split it for 3D printing?

[mitchdunc]

Hey community!

I'm trying to create a 3D printed mini subwoofer box for my car. The shape is unusual since I'm filling dead space in the car. However, the model is too big for my printer. I created this shape by lofting a circle to a square using guide rails. I then shelled the object.  I learned how to do multiple slices of the body, but none have the 'lip' I'm looking for when gluing it together. I don't want to glue flat surfaces together, and I'm looking for a way to make each piece of the 'tube' interlocking prior to glueing. 

I annotated the shape I'm trying to create inside the shell of the body with red lines. I don't think I could do a revolve feature since the base is a square shape and not a circle? 

Any advice on where to look or how to achieve this will be greatly appreciated! Thanks!!!

[mitchdunc]

Desired way to slice the body in red lines. First picture is the section analysis of the cut, second picture is the entire body with the sections I'm trying to cut for printing 

[laughingcreek]

an approach, see attached model-

[etfrench]

One way to do this on organic shapes is with a sweep:

1: Create a sketch on a mid plane.  In this case I'm using one of the Origin planes, but any plane should work.

2: Draw the profile for the split body operation.  Use the Project/Intersect command to get the shell position.  Add some offset lines to extend the splitting profile far enough to split the entire body.

3: In the Surface workspace, sweep the splitting profile.

4: Thicken the surface body, I used .001" .

5: Split the main body using the body created in step 4.

p.s. You may need to create the sweep path(s) by creating a plane at the split point, then on a sketch on that plane, Project/Intersect the body.

[mitchdunc]

Hey @laughingcreek thank you so much for the quick reply. I'm trying to reproduce the steps and approach you took. I'm unable to get the line to become the profile in the sweep. I noticed the line I'm trying to create is blue and the one in your approach is black. 

Does that mean I don't have a constraint set up properly? What do I need to click to properly add the line to the sweep function? I attached the file where I'm stuck. 

Thanks so much! 

[laughingcreek · Accepted solution]

[mitchdunc]

Ahh! I see the difference now in surface vs. solid. Thank you so much again for the help! Made my day!

[mitchdunc]

I was able to originally make the cuts and separate my bodies. I re-measured again and I made the whole box about 80mm too long. I edited my offset plane from step 3 on the feature tree to 420mm. Since then I've had an issue with thickening the line closest to the speaker hole. It's giving me a generic error. Do you know why this may be @laughingcreek? 

[laughingcreek]

the surface quality from lofting in this way is usually pretty bad, particularly around transitions-

 so building anything off them can sometimes be sketchy.  the original sweep has a terrible jigger in it in one spot-

and seen from zoomed out-

when you have a comb that sticks way out like that it because you have a spot in the edge that essentially has infinite  curvature.  the effect of a sub par path created by cutting an edge into a jiggly surface is compounded by having some of the sweep profile on the "inside" of the loop.  that was just to much for the software to interpret. 

the issue can be eased by splitting the face on the inside instead, and using that for the path.  that puts more of the profile on the outside of the loop, and fusion does a better job interpreting the surface.

a file is attached.

the closer you get to the transition area, the less likely this will work.

a better long term solution would be to learn better lofting techniques that result in better surface quality.  then subsequent  actions like this will be less likely to fail.  that's for another day.

[GRSnyder]

Just as an aside, an alternate approach to creating lips on simple bodies is to split the body with a plane, then sketch the parting line directly on that plane. You can then extrude with the Intersect option to create the volume of the lip. Use Combine to remove the lip from one body and add it to the other.

This approach has its limitations, but it's usually simpler than using sweeps and surfaces.

[mitchdunc]

I was able to replicate that solution, however it still doesn't seem to split the body into two bodies (which I assume I need for printing.) Do you know any workaround for that? Or are we just reaching the limits of software interpretation?

Side note, would it be better if I lofted a similar rectangle closer to the circle hole? That way the sections I would need to cut would be more geometric and less organic.

[mitchdunc]

@laughingcreek Adding a second fillet to make the 'tail' end of the box more square did wonders. I was able to get two slices and fit it all on my slicer for printing. Thank you for all the help again! I appreciate it a ton.