topic Re: Can't select sketch to loft in Fusion Design, Validate & Document Forum

Can't select sketch to loft

rudi4 — Thu, 02 Sep 2021 18:35:04 GMT

My name is Lukas.

I am trying to design tire to my model and I got stuck. I need to loft three surfaces (not flat). That what I did.

Three surface revolvers from sketch (arc to revolve), sketch intersected through each, and when I am trying to loft it- cant select any. Blue sketch is enable to select, but not intersected faces.

I'll be graceful for any tip

Lukas

Re: Can't select sketch to loft

Rohan.bongale — Thu, 02 Sep 2021 18:40:35 GMT

Hello,

Thankyou fo sharing your concerns. Is it possible to share the design or video of the steps you are trying.
So that I can share the solution with you .

Thank you,
Best RegardsRohan Bongale | Senior QA Engineer | Autodesk India Pvt Ltd.
P. 20 6680 4444 | rohan.bongale@autodesk.com

Re: Can't select sketch to loft

Rohan.bongale — Thu, 02 Sep 2021 18:42:25 GMT

We cannot select combination of sketch and bodies to create loft

Re: Can't select sketch to loft

rudi4 — Thu, 02 Sep 2021 18:55:08 GMT

Thank You for reply

This is not between body and sketch, just three intersected revolves (hope is understandable what I write).

Can make a Video but first I have to find out how...! I've never done it before hehe

But share design- how to do that?

Re: Can't select sketch to loft

rudi4 — Thu, 02 Sep 2021 19:23:24 GMT

I hope I got it.

I forgot to write then I've tried also project to surface but it is not active to select too.

There's link

https://autode.sk/3gXhCuL

Re: Can't select sketch to loft

TheCADWhisperer — Thu, 02 Sep 2021 19:30:34 GMT

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Re: Can't select sketch to loft

jeff_strater — Thu, 02 Sep 2021 20:21:03 GMT

actually, you can create a solid loft between surface bodies and a sketch profile. So, there must be something unique about your design that is preventing that selection. As @TheCADWhisperer says, we'd need access to your design to see for sure what is going on.

Re: Can't select sketch to loft

rudi4 — Fri, 03 Sep 2021 12:48:01 GMT

Thanks for all answers.

I made a similar design and I noticed, then if revolve is from straight line- loft function works. But if loft is from arc loft doesn't work.

Is that how it supposed to be?

I attached small fusion file

Re: Can't select sketch to loft

jeff_strater — Fri, 03 Sep 2021 13:03:23 GMT

that seems like a bug to me. I'll look into it.

Re: Can't select sketch to loft

TrippyLighting — Fri, 03 Sep 2021 16:34:09 GMT

Just to be clear, you can get the same solid geometry with a surface loft and stitching.

Re: Can't select sketch to loft

rudi4 — Fri, 03 Sep 2021 17:14:43 GMT

Yes that's working, it's truth.

I'll do it that way, if there won't be any solution, but I cant understand why it was working before.

Around two years ago, that way (revolve-intersect-loft) was working fine with previous model.

Re: Can't select sketch to loft

TrippyLighting — Fri, 03 Sep 2021 17:26:19 GMT

@rudi4 wrote:

... but I cant understand why it was working before.

Around two years ago, that way (revolve-intersect-loft) was working fine with previous model.

Although it might sound counterintuitive given that a bug might have been discovered, there have been a number of nice improvements in the loft tool over the last 2 years ad development on the tool continues to progress.

Re: Can't select sketch to loft

jeff_strater — Fri, 03 Sep 2021 21:22:59 GMT

I spent a fair amount of time (probably more than I should, but once I got started, curiosity took over) today chasing this bug down. I found the bug - we are specifically disallowing selections of spherical or toroidal faces in Loft. I think I found when this change went in, and (while it is possible that I am misreading the history here) it looks like this was done about 7 years ago. There could easily be other things going on, but that is my current understanding. Anyway, this is a bug, and we will get a fix for it. The Fusion bug is FUS-89984. Thanks for reporting it!

Re: Can't select sketch to loft

rudi4 — Sat, 04 Sep 2021 07:35:04 GMT

Thank You very much, Jeff 😀👍

I've spend many evening to figure it out, what I did wrong. It's big relief to know the reason 😅 Thank You again.

I attached a test file. It is a part of design I mentioned earlier. It is, like as said around two years old. I used function face offset, but it is from spherical revolve too- it went fine then.

Could You be so kind and take a look on it?

About bug- can I make any upgrade to fix that bug? If yes- how? I don't see any upgrade option 🙄

Re: Can't select sketch to loft

jeff_strater — Sat, 04 Sep 2021 14:22:01 GMT

I've looked at this design. The input surfaces for both lofts are actually cylindrical, not spherical. I haven't looked into the details yet, but my debug tools show cylinders

Re: Can't select sketch to loft

rudi4 — Sat, 04 Sep 2021 16:01:41 GMT

Jeff, You are right in 100%.

Now I noticed the differences now. In test2 file all is from cylindrical revolve. I used spherical surface, just to cut the body after loft, to obtain final shape.

My bad.

Solved, clear and understandable for me. 👍

Thank You