Connecting different cylinders at a 90 degree angle

[ryanbourgoin]

I'm trying to 3d print an adapter from my Dewalt Planer to my 2.5" Ridgid shop vac. Additionally, I'm trying to do it at a 90 degree angle so that the shop vac hose doesn't interfere with the boards being planed. I can do a surface loft between them using the inner surface and the outer surface, but when I go to 3d print, I'm getting non-manifold errors and when I try to have them auto-fix, it is making the center of the adapter solid. Can anyone help? I have minimal experience modeling, but just got a printer, so wanted to try.

[jhackney1972]

To do a hollow Loft, you have to loft twice, once for the solid outside shape, then a second time to hollow it out.  You also needed to create a sketch to provide a center  line for the two lofts.

Model attached.

[laughingcreek]

Since your new to modeling, I would suggest NOT moving sketch items off the sketch plane as you did in the first sketch.  attached is one approach.  I suggest going thru each feature in the timeline and asking questions about things your not sure about.

[laughingcreek]

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@jhackney1972 wrote:

To do a hollow Loft, you have to loft twice, once for the solid outside shape, then a second time to hollow it out. ...

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a pitfall of this approach with lofting is that it's difficult (impossible?) to get a consistent wall thickness.

[etfrench · Accepted solution]

Surface loft with rails, then Thicken works well.  Use tangent constraints between the rail splines and the projected adaptors.

[johnsonshiue]

Hi! Here is another similar solution. Guide Rail Sweep is used instead.

Many thanks!

[ryanbourgoin]

Thank you everyone for your help. I ended up having the tolerance on the vac side a smidge too tight and had to cut the fitting off. Additionally, I decided to attach to the inner ring of the planer (it has 2 rings) because it was wasting filament to go around the bigger size. Because I messed up the original model so much, I started over taking the advice given here. My workflow was:

did all work in 1 plane as suggested

Do a canvas with a pic I took with calibers

calibrated the picture

ID of vac hose

OD of vac hose

OD or vac hose ring

rotate sketches 90 deg facing north

extrude to component, then I cut the excess

then I crated planer 

OD planer ring

ID planer ring

rotate 90 deg facing west

extrude to component

then I did a 3 point arc connecting the center points of the circles

then I did a surface loft using the outer edge of each adapter, centerline following arc

then I did an analysis to break it into half (didn't even know you could do this and it was awesome)

then I thickened

I think I got everything right, trying to print the whole thing (like 4.5 hours)

Some questions:

Why do the center points of the circles disappear? I had a hell of a time getting the arc to eventually attach, but I think it was more luck than anything else.  Also, I wasn't sure how constraints would have helped, can someone tell me how they interact? Did I miss anything in the workflow?

Again, thank you all for all of your help.

[laughingcreek]

again, highly suggest not rotating things off the sketch plane.  this time you did it in sketch 2.  keep all your sketches 2d (moving things off the plane makes it a 3d sketch).  both these sketches could have been placed on the origin planes that are at right angles to each other.  (hint: layout the center line first so the end points are on the sketch axis)

if you do a section analysis and look at these locations-

you can see the loft could be improved. in the attached I changed the center line from an arc to a spline so I could make the center line perpendicular to the loft profiles.  then I changed the end conditions of both loft profiles from "connected" to "tangent".  open the attached and you can see the result.

[ryanbourgoin]

I tried to just do a basic test following your instructions. I think I did the circles on the 90 deg angles correctly; I did the spline on the plane between green and red. However, when I went to loft, it didn't give me the option to do tangents. I'm not sure where I went wrong and there's small gap again.

[TrippyLighting]

That is because you used sketch profiles for lofting instead of surface edges.

Tangency can only be created between sketch object or between surfaces, not between sketch object and surfaces.

It would probably be easier if you created the whole design as a solid loft and shelled it or as a surface loft and then thickened it. 

[ryanbourgoin]

The solid loft using the faces and following the spline followed by cutting solid loft based on the inside edge following the spline seems to have eliminated the gaps and kept the walls consistent without thickening.