topic Re: Failing loft in Fusion Design, Validate & Document Forum

Failing loft

arnou-verfaillie — Mon, 05 Jul 2021 12:09:07 GMT

Hello

I have been struggling with a loft I want to create. Been searching and googling but have not yet found any solution.

I want to connect to profile on the bottom part to the edge of the top part, so the shape flows nicely. Sometimes the loft will not succeed (is this because of the touching points at the right?) and sometimes the loft will succeed, but I get all kinds of weird shapes and bodies that don't even connect with each other.

What am I missing here, what can I do to make this part? Have also tried sweeping and the splitting bodies and faces, just to match things up, but not with the result I want.

Thanks in advance!

Re: Failing loft

TheCADWhisperer — Mon, 05 Jul 2021 12:23:10 GMT

Sketch1 is pretty "rough".

I think I would start by rotating my Canvas, not the sketch.

I got lost after that...

Re: Failing loft

arnou-verfaillie — Mon, 05 Jul 2021 12:28:35 GMT

I know it's a bit rough, the canvas was not executed that well, but you think that would solve my lofting problem?
Will definitely give it a try.

Re: Failing loft

davebYYPCU — Mon, 05 Jul 2021 12:37:42 GMT

You have way too many spline points. Will create surface irregularities for you.

Make half and mirror the half body.

Might help....

Re: Failing loft

arnou-verfaillie — Mon, 05 Jul 2021 13:29:49 GMT

Both of these suggestions helped a lot, straightening the canvas was easier to work with.

I also used less spline points and only drew half of them and mirrored them. The loft actually worked now.

I do have one other issue, parts of the loft seem hollow. I want to split the body into 3 smalles ones (for 3D printing) and when I split them, the loft itself seems hollow, which probably will mess up my print. Any idea what could cause this?

Re: Failing loft

davebYYPCU — Mon, 05 Jul 2021 13:56:16 GMT

There are 2 Loft commands,

hollow from the orange icon in Surface area,

and solid from the blue icon in the Solid area.

Might help....

Re: Failing loft

arnou-verfaillie — Tue, 06 Jul 2021 09:23:26 GMT

I used the blue icon from the SOLID area?

EDIT: I did use the blue lofting feature. Tried it as a new body instead of joining now and I got a new body with this orange (hollow?) icon next to it.

Re: Failing loft

davebYYPCU — Tue, 06 Jul 2021 10:02:53 GMT

Bodies 22 and 23 are solids, body 27 is surface.

Might help....

Re: Failing loft

arnou-verfaillie — Tue, 06 Jul 2021 10:14:16 GMT

Yeah, but how? I used the solid loft feature, then how is this a surface?

Can this be changed afterwards, I've never had this issue before? Haven't used loft much either

Re: Failing loft

davebYYPCU — Tue, 06 Jul 2021 10:40:14 GMT

Checked the file just now.....

Very interesting, @jeff_strater will raise an eyebrow!

(Solid loft has not completed correctly, profile faces are (missing - unstitched))

Yes can be fixed with Boundary fill,

First edit the solid Loft to New Body.

Use Boundary fill, select top, bottom and loft bodies, select middle tick box, and set New Body, keep tools.

Might help....

Re: Failing loft

TrippyLighting — Tue, 06 Jul 2021 11:25:49 GMT

@davebYYPCU wrote:

Very interesting, @jeff_strater will raise an eyebrow!

(Solid loft has not completed correctly, profile faces are (missing - unstitched))

What raises my eye brow is the design methodology in general. Wat people generally tent to forget is that the loft tool cannot read minds 😉 As such it needs to have precise inputs to complete it's mission. Those are missing.

Something that should have been pointed out to the OP already before lofting is even discussed is that it is a bad idea to mirror fit point splines. There is another recent thread discussing this behavior of fit point splines in Fusion 360.

Then the sketch is not symmetric about the design/sketch origin. That also is a no-no. If something is to be symmetric, then having it centered around the design and sketch origin is good practice.

Re: Failing loft

arnou-verfaillie — Tue, 06 Jul 2021 12:25:19 GMT

Ok, so fit point splines might not be the best solution (it's the 2nd time I'm designing something from a 2D scan). I'll try it again with the control point spline.

You say I'm missing precise inputs, what exactly am I missing here?

Also what exactly is raising your eye brow on my methodolgy? Trying to learn here..

Re: Failing loft

TrippyLighting — Tue, 06 Jul 2021 12:33:36 GMT

@arnou-verfaillie wrote:

Ok, so fit point splines might not be the best solution (it's the 2nd time I'm designing something from a 2D scan). I'll try it again with the control point spline.

While I also would use a control point spline, fit point splines a fine. Just don't mirror them. I would not mirror a control spine either. In fact I very rarely see the need to mirror or pattern anything in a sketch.

There is no need to mirror anything in a sketch in this design.

Re: Failing loft

TheCADWhisperer — Tue, 06 Jul 2021 12:50:45 GMT

OK, I'll jump back in here...

I question whether Loft is even needed/wanted for this geometry.

It looks like Revolve and Extrudes might be the solution to me.

I'm suspecting I would do a Shell and then perhaps Split.

Any Split I would do would most probably be done with Sketch rather than extraneous planes.

The line of symmetry in the first sketch (Sketch28?) isn't even constrained to the Origin (it is slightly below).

How will this part(s) be manufactured?

I try to keep the guys and gals out on the shop floor in mind when designing and Design for Manufacturability.

As a machinist - this fairly shouts to me - noooooooooooooooo

Now if splines are needed, they are needed, but otherwise I use Lines and tangent Arcs - keep the geometry in as primitive form as possible.

What is this part(s)?

Re: Failing loft

arnou-verfaillie — Tue, 06 Jul 2021 13:05:23 GMT

@TrippyLighting What is so bad about mirroring? The part of which I scanned this from was handmade back in the 70s, when mounted it actually shows off center. Which makes it look weird (makes it look like the wheel of the bike is not centerend). The mounting holes are centered, so if I design one side, mirror them around the centerline of the holes, I have a symmetric piece? Yes I could run the entire control point around the curve, but that would still make an off centered piece.

I actually just redesigned the entire piece with control point splines, mirrored it and now the loft works as intended. Not sure what the issue with fit point spline is...

@TheCADWhisperer Yeah not much is constraint, because it was just drawn from the canvas. That center point not being in the origin did not really bother me, as it doesn't have any constrains/ dimensions anyway. It was just drawn to define the mirroring line.

This part will be 3D printed and the first attempt allready worked great, but the overal shape was wrong. Just revolved the outer edge and printed it, but the actual part has a straight piece (the loft) and then a revolve.

Re: Failing loft

arnou-verfaillie — Tue, 06 Jul 2021 13:09:35 GMT

This is the part in question actually: rear end cover for the seat of a Yamaha RD50 dx. These rear ends are hard to find and I want one in the same colour as the rest of the bike, but I don't want to ruin this chrome one by repainting it.

Re: Failing loft

TrippyLighting — Tue, 06 Jul 2021 13:45:36 GMT

@arnou-verfaillie wrote:

@TrippyLighting What is so bad about mirroring?

Mirroring in the sketch environment simply adds a lot of constraints that constantly have to be evaluated by the sketch engine, and thus cost performance. That is not the case if you mirror geometry instead of sketch objects.

The number of constraints also make it difficult to debug a sketch.

I linked to a thread in my previous post that explains why mirroring fit point splines in particular is not recommended.

Re: Failing loft

arnou-verfaillie — Tue, 06 Jul 2021 14:02:22 GMT

Ah, mirroring geometry instead of sketches, that's a good tip. Will keep that in mind!

Yeah I read about the fit point splines, will try to avoid them from now on.

Re: Failing loft

jeff_strater — Tue, 06 Jul 2021 14:53:09 GMT

This is, at the root, a problem with "point mapping". When the profiles in Loft have a different number of points, Fusion has to try to figure out which points map to which in each profile. Even modeling just half here (which is, indeed, a good strategy) still has mapping problems. Sometimes, you can untangle the mapping by dragging on the white point handles, which is tedious at best. I played a bit here, and was unable to make it work. The usual approach in these cases is to add rail curves. Rails help constrain this point mapping problem, and guide the algorithm. Even that is a little complex, since you then have to put conditions such as tangency, etc on the rails. But, one could probably make a decent result using just one or two rails (I did not try).

And yes, the fact that the profiles meet at the corner could produce a pretty bad surface near that corner.

Personally, for something like a motorcycle seat, I would be very tempted to do this as a Form (T-Spline) feature. T-Splines are very good at this kind of "soft" modeling. Again, use symmetry so you only have to worry about half of the seat.

Re: Failing loft

arnou-verfaillie — Tue, 06 Jul 2021 15:01:38 GMT

In all honesty I have never touched the Forming features as I am more used to normal sketching with known or measurable dimensions. This is the first case of me actually trying to reproduce a shape from a canvas. I have learned a lot today and will definitely test things like this further. I will be printing my V3 shortly.

Thank you all for the tips!