Loft Twisting
shai_perednik
Member Posts: 56 ✭✭
I'm struggling with lofting from a big rectangle to a smaller one. Seems no matter which verticies I match, even though they both have 4 segments, I get this twisting effect, like the segments don't line up. Any ideas what I'm doing wrong here? Doc is @ https://cad.onshape.com/documents/14f3d01d62b5237f728896c5/w/40e0afc950b8ca0dfecf9ef8/e/48d62775ba30708d4aae1614
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Best Answers
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Thanks for sharing the doc url. I took a look and it appears this may be a bug. Please submit a ticket from within the doc so we can take a closer look.
To submit a ticket, select the "?" icon and then select "Feedback".Tim Rice | User Experience | Support
Onshape, Inc.5 -
Hi Shai!
This is definitely a bug, but I made a workaround for you.
https://cad.onshape.com/documents/585d46f6f8e2481026feea90/w/44023bb57993425fb42458c8/e/55dcad2c614e5820ba0e8a91
I extruded the lower sketch into the circular part at 1mm to create a new very small sheet-like part. I then hid the red circular part and lofted between then face up the upper part (not sketch 6) and the new utility part. The loft came out correctly and I deleted the utility part and unhid the red circular part. Because I made the utility part extrude into the red part (rather than away from it) your loft should be touching both parts as intended.
Hope this helps!Jake Rosenfeld - Modeling Team5 -
Awesome, I can confirm Jake's workaround works
Now for a more complex loft, will post shortly
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I just examined the first case you filed the ticket with. It looks like there's a problem with your sketch and it's constraints on the red body. Please see the attached images. The Top view shows the two problem corners, and I have zoomed in to them.
As you can see there's one extra edge created on your sketch, which is causing loft to try to match a 4-edged face to a 5-edged one.
I recreated the sketch by just "Use"-ing the 4 corners and joining them with lines. The loft succeeded without any twists. Give it a try! It might be the same issue with the second loft you posted. I'll take a look.
We can talk further about this through the ticket, but I wanted to post this here as this is something I've seen other people run into. If the sketch is not being projected correctly, then loft has trouble and because the edges are so tiny it's hard to track down.
7
Answers
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Thanks for sharing the doc url. I took a look and it appears this may be a bug. Please submit a ticket from within the doc so we can take a closer look.
To submit a ticket, select the "?" icon and then select "Feedback".Tim Rice | User Experience | Support
Onshape, Inc.5 -
Hi Shai!
This is definitely a bug, but I made a workaround for you.
https://cad.onshape.com/documents/585d46f6f8e2481026feea90/w/44023bb57993425fb42458c8/e/55dcad2c614e5820ba0e8a91
I extruded the lower sketch into the circular part at 1mm to create a new very small sheet-like part. I then hid the red circular part and lofted between then face up the upper part (not sketch 6) and the new utility part. The loft came out correctly and I deleted the utility part and unhid the red circular part. Because I made the utility part extrude into the red part (rather than away from it) your loft should be touching both parts as intended.
Hope this helps!Jake Rosenfeld - Modeling Team5 -
yes, please do submit a ticket. I'm suspecting a problem with the sketch imprint on the red circular face.0
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A ticket has been submitted for @shai_perednik0
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@ shai_perednik .Without matching vertices also it should work but it is not working even if you select the vertices .
As a work around Try this,
Extra face can be removed by using Delete face option,
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Awesome, I can confirm Jake's workaround works Now for a more complex loft, will post shortly
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Trying this loft from the yellow parts bottom face (rectangle) to the face of the gray round part (or to the sketch), and neither generate properly. I believe this is because of the mentioned above bug.
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Hi again Shai,
I think the bug here is due to lofting between sketches. Can you try your loft between faces of geometry rather than sketches? If there isn't a face that perfectly matches your sketch you can first extrude-new your sketch away from the loft, use it as a parameter to the loft, and delete it as I did in my first workaround.
Let us know if that works, Thanks!Jake Rosenfeld - Modeling Team0 -
@Jake_Rosenfeld I'll try that
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I just examined the first case you filed the ticket with. It looks like there's a problem with your sketch and it's constraints on the red body. Please see the attached images. The Top view shows the two problem corners, and I have zoomed in to them.
As you can see there's one extra edge created on your sketch, which is causing loft to try to match a 4-edged face to a 5-edged one.
I recreated the sketch by just "Use"-ing the 4 corners and joining them with lines. The loft succeeded without any twists. Give it a try! It might be the same issue with the second loft you posted. I'll take a look.
We can talk further about this through the ticket, but I wanted to post this here as this is something I've seen other people run into. If the sketch is not being projected correctly, then loft has trouble and because the edges are so tiny it's hard to track down.
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@shai_perednik
Congratulations - you just met Dr Tosun (Elif)
Besides being an awesome person, she also wrote our loft. Now, it might not be for me to say Onshape is awesome (I am biased), but someone else might say "it's a pretty cool CAD company when you can ask the developer that wrote the code why your thing doesn't work"!
#iloveonshape
Philip Thomas - Onshape0
