Fusion
@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)...
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.
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
@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?
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.
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.
Selecting this chain, it breaks at the white dot on the left, and black dot on the right.
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.
"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
