Having trouble with simple pipe elbow connector modeling

[chrisQX8DX]

so i'm almost ashamed to ask this here since it seems such a simple thing to model ... in my defence: i have a massive cold at the moment so i think my brain is on strike and refuses to solve this simple model. 😫

it's an adapter for a hose on my CNC, going from one inner diameter to another, these two parts are modeled and have been printed and test fitted so now for the final part i need to get the 90° elbow that connects the two, sth like this:

i just can't figure it out, i first though i could just loft the end profiles or loft the edges as a surface and then thicken it. then tried sweep, revolve, whatever i do the solution eludes me ...

there's gotta be a simple way to do this ???

[kacper.suchomski]

Hi

You can use G2 tangency instead of guide path.

[chrisQX8DX]

hey thx so much for the quick reply, that works but doesn't create a perfect 90° angle but is squeezed in the middle:

[davebYYPCU · Accepted solution]

You should never use Move Tool as you did - moving a body off file origin / Sketch.

You are correct, Surface Loft and Thicken > Join, will give the best efficient result.  Solid Loft cannot do tubing.

A Spline for the centre line Rail - you lose control of the Loft.

Reconstruct sketch 3, with the inside fillet to your desired radius.  (Max about 8mm) Larger will shorten the straight rail lines.

When sorted, use Surface Loft, select the body outside edges, select both Rails, and set Tangency to those bodies, will bring the top view shape into a smooth transition

Might help...

[jhackney1972]

According to your screen capture, you would like to loft the inside diameters of each ring.  The error you are incurring is due to the incorrect path which causes the loft to intersect itself.  The path needs to be generated with an Arc and a Line.  I have attached two models. one as you show in your screen capture and one with the outside used as the body size.  The one using the diameter you show does not have an inside diameter because you did not specify it.  The one using the outside profile does as I used the ID of each end to loft the inside cut.  One other thing you need to know, you cannot Loft a hollow object.  You must create two Lofts, one for the outside solid and one for the inside cut.

[TheCADWhisperer]

@chrisQX8DX 

See my guess attached.

[pkomatlapalli]

Hello @chrisQX8DX ,

It looks like you have received a lot of advice on this thread. Did any of the replies by @davebYYPCU  and @TheCADWhisperer  answer your question? 

If you are still needing more help, please share an update here. The community will be happy to jump in and suggest more steps to help you get where you need to be.

Best,

Pavan Kumar| Community Manager