How to blend two cylinders for an organic/welded T-pipe shape, like in the attached image?

[FusionFan3000]

I'm trying to create my own T-pipe style object like in first attached image (created by someone else in Solidworks). The two cylinders are blended together in a very organic way.

I tried intersecting and joining two cylinders in the Design Workspace ("Solid" tab) and adding a fillet, but as expected, the result is nothing at all similar to the organic nature of the first attachment.

I'm not familiar with using the Surface or Mesh tabs, and am hoping there's a way to achieve this with a parametric design instead via the "Solid" tab instead? And if not, could someone please help me understand how to achieve this?

Any advice is appreciated!

[davebYYPCU · Accepted solution]

No idea of the ratio between the pipe diameters, so you may pick up some clues.

Much easier with Surface, solids will be difficult due to solid Loft being limited quasi "four sided" objects

The Patch in this example is 5 sided.

Might help...

[FusionFan3000]

O M G THANK YOU!!!!!!!!!! You could not have shared a more perfect set of instructions. That is super super helpful. I walked through the file and learned a lot - would never have figured that out on my own. Also the way you went about it using surfaces instead of a Form makes it very easy to design with specific dimensions in mind and go back and edit.

I'll summarize my takeaways for anyone coming back here in the future, even though the file you attached makes it way clearer:

• Rather than creating intersecting solid cylinders and trying to blend them together with fillets or lofts, you need to create surfaces of some of the key fixed elements such that you can patch their edges. The patching operation will automatically create the organic blend between them.
• Rather than working on the entire shape, it makes sense to work on just a quarter at a time until you have created half of the full structure.
• Stitch it all together so you have a single surface that represents half of the object you want. Then mirror it so you have the full body.
• Use the thicken operation to turn it into the solid body that you want.

Woohoo!

[johnsonshiue]

Hi! There are multiple ways to do it as Dave already illustrated. Here is another solution. Instead of creating a Fillet, create a Chamfer. Then delete the chamfered face. Cover the face with a Loft surface. The blend will be much closer to weld beads. Another way is to create a Chord Length Fillet (not the Constant Radius Fillet).

Many thanks!

[TrippyLighting]

Would you be able to share the model you posted images of?

The surface patches in the model @davebYYPCU posted aren't even tangent where they need to be. Tangency is a minimum requirement for a smooth transition between surfaces!

[FusionFan3000]

Dear @davebYYPCU , @johnsonshiue , and @TrippyLighting 
Thank you all for chiming in, sorry I'm coming back to this late, but it seems as TrippyLighting mentioned, there may be more to it than meets the eye.

I tried re-creating the steps from @davebYYPCU , but I think the surfaces might be having some issues, for example the circular ends generate errors if I try further modifying the body, such as extruding / push-pulling it.

For full context: A designer helped me design the original T-Pipe design as the outer plastic shell for a prototype I'm trying to design. Unfortunately, the designer...

• (A) forgot to have the protruding branch be tilted 5 degrees upward compared to the ground (e.g. XY plane). In their design, the protruding T is parallel to the ground.
• (B) I'm now working with a DFM engineer to try to turn it into something moldable, but we're struggling to modify the original design.

I don't have access to that designer anymore, so I can't ask them to fix the design, but even if they do, it seems they had a lot of artifacts which caused issues anyway.

I've attached:

• Original STEP file from designer
• F3D file of my attempt to recreate designer's STEP file using @davebYYPCU 's instructions 
• Image that shows a comparison of the original designer's file, my attempt, and a request from my DFM engineer that I am struggling to fulfill.

If you have any thoughts on how I could solve this, I would be very grateful!

P.S. @johnsonshiue the solution you mentioned seemed to have a harsher/sharper transition compared to a more natural organic one, but maybe I'm not interpreting the image you shared correctly?

[davebYYPCU · Accepted solution]

Having fixed my earlier deficiencies, 

Makes sweet work when the sketches are fully defined. (no guessing) Slightly different set up.

I did encounter problems with the sketch 4 rail, and near coincident with Combine, so went with Boundary Fill.

Check and let me know if I have missed anything.

Might help...

[FusionFan3000]

Thank you so much!!!!! It's perfect and easy to follow in your file!

Am I understanding correctly that the key difference this time is that we only used the edges of surfaces and bodies (as opposed to sketch lines) for the surface patch, which allowed us to set each edge as "Tangent" in the Surface Patch "edit feature" menu?

Follow up question if you don't mind:
If I try to adjust the curvature of the arc at the top with a fit point spline (image below))

or if I try to change the angle of the protruding branch from a slight tilt to completely perpendicular (image below)

...then, the final Mirror function breaks down with a compute failed error (even if I manually regenerate the surfaces and surface patches and boundary fill operations).

I don't quite understand why that would be happening?

[davebYYPCU]

Few hours before I can get to the files.

Yes, 100%, the Tangent / Curvature settings are only available from body edge selected, sketches are not a trigger.

The red icon, I’ll presume the body to mirror had internal references that are now lost, I presume a Delete / Replace will fix it, (could be wrong) but will confirm later.

Fusion will behave more predictable with an adjustable fillet, instead of the spline.  This is more a design intent decision - change the highlighted Tee angle, and allow Fusion to adjust the fillet radius, by making the radius driven.  Otherwise the pivot position for the Tee intersection, would need to be the centre point of this Fillet.  Thoughts?

For now….

[FusionFan3000]

Oh ok I think that makes sense. I was using a fit point spline because its bezier handles allow one to play around with the exact curve a bit (allowing me to try to match the original T-pipe), but having that radius be driven is probably more reliable (like in your latest file) even if it comes at the cost of not having the bezier handles. Regarding the mirror, I'll try to recreate all the operations from scratch and see if that fixes it. I had so far only attempted to edit and re-do the patch and boundary fill operation.

[davebYYPCU]

No joy, now that there is a spline curve in the model, most if not all my attempts to repair your broken files, have been unsuccessful.

You are right, to reengineer that original, needs the spline, as an arc will not fit.

@johnsonshiue or @jeff_strater can ask the developers to investigate the broken Mirrors, and some of my testing breaks the Boundary Fill.

Might help...

[FusionFan3000]

Thank you for taking a look! Not sure if there's a downside to doing it this way, but instead of doing a boundary fill to create a solid body which represents half of the model, and then doing a mirror operation....

I instead mirrored the surfaces and stitched them, then boundary filled the final result. It seems to work!

[davebYYPCU]

Ok, always a number of ways to get there, however the routines that are failing need reporting.

Might help…

[FusionFan3000]

Ok makes sense. Thank you so much again for your help, I really really appreciate it - you've lifted a huge burden that was causing a lot of stress and also taught me a bunch in the process. I def owe you a beer 🍻

[johnsonshiue]

Hi! I took a quick look at the model. The Mirror Bodies failure is probably due to inconsistent edge tolerances. Boundary Patch Surfaces have relatively loose tolerance (0.01mm). Trying to join the BP surface bodies with cylinders (tight tolerance) may not yield an ideal result. Instead, I create the Mirror first and then stitch them all together.

Many thanks!

[davebYYPCU]

Both files in message 8 do not create or update the mirror, please report failures.

Workaround has Been figured out, but not a fix to a simple problem.

[johnsonshiue]

Hi! I will forward it to the project team for further investigation. Though the issue may looks simple, the underlying cause may not be as trivial to address as it seems.

Many thanks!

[guilherme_sergio]

Hello!
Thanks for highlighting this for us.

The join operation deletes the shared faces to create a single solid body. This looks to be problematic in the attached model.
As mentioned before, manually deleting what would be the shared face and mirroring the resultant surface body achieves the desired result - the join operation happily succeeds.
It does look to be a tolerance issue.

We have opened a task for the failed join operation in the mirror and will investigate further.


Many thanks,