Community
Fusion Support
Report issues, bugs, and or unexpected behaviors you’re seeing. Share Fusion (formerly Fusion 360) issues here and get support from the community as well as the Fusion team.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Changing wall thickness of curved tube

8 REPLIES 8
Reply
Message 1 of 9
john3KBSE
251 Views, 8 Replies

Changing wall thickness of curved tube

Hi, I've drawn a curved pipe as shown on attached file.

 

The internal diameter is fixed but I need to increase the wall thickness from 1.95mm to 3mm.

 

Due to curvature constraints I can't use PressPull as it leads to bad geometry. Likewise with using thicken when converted to t spline.

 

Ideally the walls of the body need to self-intersect (overlap?) at the exterior concave curves.

 

I'm fairly new to fusion 360, so please forgive me it this is not very well explained!

 

Thanks in advance for any help

 

John

 

 

8 REPLIES 8
Message 2 of 9
TheCADWhisperer
in reply to: john3KBSE


@john3KBSE wrote:

I'm fairly new to fusion 360, so please forgive me it this is not very well explained!


Are there any unresolved issues highlighted in your Timeline?

Are all of the sketches fully defined?

Why are there multiple bodies?

 

I am going to suggest starting over from scratch.

You only need one sketch.

No splines.

No repeated dimensions.

No user created workplanes.

One body.

 

Ask questions early and often.

Use the Origin as an absolute datum.

Do you have a picture of something similar that already exists in the real world?

 

Start a fully defines sketch (see Attached)...

TheCADWhisperer_0-1691930748474.png

 

Message 3 of 9
jeff_strater
in reply to: john3KBSE

Here is one way - I did not use your design, I just created a new one to illustrate the concept.  I did this with 2 Lofts, using a Centerline Rail to affect the shape.  The outer wall goes from 100mm to 150mm, while the inner diameter stays at 75mm.

Screenshot 2023-08-14 at 8.09.52 AM.png

 

model is attached, FYI.

 

BTW, if you are interested, there is a lot you probably could have done differently in your design.  There are lots of warnings, which should not be ignored, and lots of Move Body/Split combinations that likely could have been done in other, more efficient ways.

 


Jeff Strater
Engineering Director
Message 4 of 9
davebYYPCU
in reply to: jeff_strater

Interesting, 

one loft, and a pipe cut is jumping out at me. (Less sketching)

 

Might help....

 

Message 5 of 9
john3KBSE
in reply to: john3KBSE

Hi Guys, Thanks for getting back to me.

I fully take on board your remarks! This is my first foray into fusion360 so please forgive the messy, scattergun approach - certainly not the most efficient.

The reason there are so many bodies is that when lofting along different sequential centre lines I can never get the chain selection to produce a body without an error. Clearly something I'm doing wrong as I understand that one body modelled along a continuous centre line would be ideal.

I'll take on your suggestions in a new simplified document and see how I get on.

Jeff - the issue with having a wider outside dimension is that the requisite curves are too sharp so the body self-intersects creating and error message. Maybe I need to convert to a t spline and manually thicken certain areas of the surface?

Dave - Could you explain how a pipe cut would work?

 

Message 6 of 9
TheCADWhisperer
in reply to: john3KBSE


@john3KBSE wrote:

...the issue with having a wider outside dimension is that the requisite curves are too sharp so the body self-intersects creating and error message... ...certain areas of the surface?


@john3KBSE 

From your problem description I suspect that you will need to use Surface Modeling tools and then Stitch.

I suspect that you can stay away from Splines and Loft.  My attempt would be with Lines, Arcs, Sweep (surfaces) and Trim, Stitch and Shell.

TheCADWhisperer_0-1692030253775.png

 

Message 7 of 9
davebYYPCU
in reply to: john3KBSE

Ideally the walls of the body need to self-intersect (overlap?) at the exterior concave curves.

 

Well, that is not a normal request and Sweep, Pipe and other tools prohibit this type of overlap.  You would have to make separate bodies and combine join them at the intersections in this case.

 

Your main problem is that the centre line is not Chaining.

 

You should be able to double click on any part of the chain, and Fusion will select the whole thing.

 

nochaindb.PNG

 

Selecting this chain, it breaks at the white dot on the left, and black dot on the right.

 

nochaindb1.PNG

 

Click Drag those curves and the chain is not connected, even though it appears to be.  Loft is so finicky, and even if the chain was fully connected, there are no tangent constraints, and therefore Fusion will then complain, not Smooth.

 

Fully defined and constrained sketching, turns black, and its fully parametric, with dimension changes. As depicted from the whisperer.

One track per sketch will reduce the sketch chaining calculations as well.

 

Might explain some of the process you need to implement.

Message 8 of 9
jeff_strater
in reply to: john3KBSE

"Jeff - the issue with having a wider outside dimension is that the requisite curves are too sharp so the body self-intersects creating and error message. "

 

As discussed here, that will cause problems.  Fusion does not allow self-intersecting geometry.  How will this object be manufactured?

 

"Maybe I need to convert to a t spline and manually thicken certain areas of the surface?"

 

You will still have the self-intersecting problem with this method, and manually thickening would be frustrating, inaccurate, and time-consuming.


Jeff Strater
Engineering Director
Message 9 of 9
TheCADWhisperer
in reply to: john3KBSE

@john3KBSE 
After a bit of thought, I’ll guess that the internal hole is tangent continuous smooth.

In that case Sweep the “hole” as a solid body and then Shell to the outside (or Offset if surface modeling ends up being required).

All starts with a logical tangent continuous path.  Lines and arcs.

 

I suspect this ends up being a relatively simple problem once the Path is defined.

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums