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Sweep Unexpected Twist

Sweep Unexpected Twist

Sweep Unexpected Twist

(OP)
I'm trying to create a basic 'rib' along the top surface of a part. However, Solidworks can't seem to correctly resolve the path and I get "Sweep resulted in topologically invalid body" error.

I have the path as a 3D sketch along the surface of the part, and the profile, a simple square, perpendicular to the path. When the sweep is created, it begins to unexpectedly twist as it moves along the path around a corner and over a curve, as shown in the pictures. I'm not sure why this is occurring, but I suspect this is causing the error, and even if it's not, it's not what I intend.

For 'options' I have Orientation set as "Follow Path", and Path Alignment type as "Minimum Twist". I have tried just about every other combination of setting without any improvement.

Any ideas on how I can resolve this?





RE: Sweep Unexpected Twist

you might try direction vector and select a vertical edge

RE: Sweep Unexpected Twist

I suspect it's the transition by the slot feature that's causing the issue. You might try offsetting a sketch as a guide curve.

Jeff Mirisola
My Blog

RE: Sweep Unexpected Twist

(OP)
I seem to have uncovered the realm in which Solidworks struggles because I have a trouble at every step. For each curve I have to do a sketch on a plane, project it onto the curved surface, then convert it to a 3D sketch before I can use it. I seem to run into random problems at each phase.

Perhaps I'm just approaching this problem wrong. I want to add a 'ridge' or 'rib' along the surface to a joining part can fit snugly on it. How would other people go about adding this to the part?

I'm trying to use a second curve as a guide curve, but so far not having any success.

RE: Sweep Unexpected Twist

(OP)
CorBlimeyLimey, thanks for bringing my attention to that. It's a useful second-option. However, it doesn't allow me to center the lip/groove in the way I wanted. Ideally, the ridge would run along the center of the surface. Is there another similar option for this?

RE: Sweep Unexpected Twist

Have you tried breaking the groove down into segments to determine which portion causes the twist?

RE: Sweep Unexpected Twist

(OP)
Yes, it appears to have trouble navigating the arched portion. This may be because the arched portion begins to rise as it is still curving around the corner, so it's not a straight up-and-over, if that makes sense. I would still assume Solidworks to be able to navigate this geometry, but maybe I'm wrong.

RE: Sweep Unexpected Twist

JM's suggestion to apply a second sketch / curve as a guide is likely to work. Alternatively you could form the faces of your tab using surface extrusions + trimming, then knit them into a solid and combine with your existing structure.

RE: Sweep Unexpected Twist

Have you tried extruding the 3d sketch as a surface and then thicken the surface as required?

RE: Sweep Unexpected Twist

(OP)
snowshoe2, it doesn't look as though I can extrude or widen a extruded surface. Perhaps I'm missing something?

I've been trying to use a second sketch as a curve guide, but keep running into problems such as "too many entities share a point" or some other error. Not sure why, sometimes it works, sometimes it doesn't. I can re-sketch everything and it will work and then I try something else and it all falls apart and I have to start over. It's like the nexus of the universe in here!

RE: Sweep Unexpected Twist

(OP)
snowshoe2, very cool trick. I'll have to remember it, thanks for pointing that out to me. Unfortunately, using this method doesn't maintain the cross-sectional area of the ridge as shown in the pic.

RE: Sweep Unexpected Twist

Yep, I see the dilema. I wish I had a bit more time to help out.

RE: Sweep Unexpected Twist

kojiai,

That doesn't look like a thickened surface. A thickened surface should create an equal cross-section. What you show looks like an extrude with a direction vector.

Can you post the actual SW parts (or simplified versions) to work with?

RE: Sweep Unexpected Twist

(OP)
CorBlimeyLimey, the pic does in fact just show an extruded surface, just happened to be when I took the screen grab. I can thicken that surface and get closer to what I'm aiming for, but the shape remains the same. The thickness of the ridge narrows as it moves down the curve.

I attached the file so you can play around with it. Thanks!

RE: Sweep Unexpected Twist

(OP)
Closer than I've ever gotten, thanks CorBlimeyLimey.

Could you run me through the steps you took a bit. What was the Surface-Offset operations for?

RE: Sweep Unexpected Twist

Use the rolback bar to step through the history.

Surface-offsets 1 & 2 were create to be the trimming planes for the Zero-offset surface, but they had to be extended first.

RE: Sweep Unexpected Twist

Interesting CBL. I play in surfaces a fair bit, and never used the intersect feature before. I'll have to look at that closer as it seems like at the very least it can eliminate a step in the model tree compared to my standard routine of knit + combine.
In the interest of seeing how few steps this could be done in I modded your Sketch 1 and took out the surface extend to simplify a bit further. As a thought exercise I'd be interested if anyone gets it down simpler than this. With CBL's method its down to 5 items in the model tree, including the new reference plane.

RE: Sweep Unexpected Twist

And the added plane I guess doesn't have to be there, so 3.

I Have a hunch that it could be done with 2 features, using just a boundary surface and the intersect, Possibly 1 with a boundary boss/Base feature. Both of those would require additional sketches though, so there'd be more work involved than this method.

RE: Sweep Unexpected Twist

OK... so what, I have to refresh every time right before I post to make sure CBL hasn't already reposted what I was doing??? :)

RE: Sweep Unexpected Twist

(OP)
You've blown my mind. Surface extrudes, offsets and intersect?! Never would have crossed my mind.

Thanks for all help and effort from everyone. This has been a really interesting lesson.

RE: Sweep Unexpected Twist

(OP)
Okay, I have yet another question.

Clearly this 'ridge' needs to interface with another piece. So now I'm looking at doing the inverse, rather than an extruded shape, it's a cut shape into the part. I've been playing around with it, but putting surfaces inside another part is somewhat pointless. What's the best way to proceed with this? Thanks!

RE: Sweep Unexpected Twist

Quote:

putting surfaces inside another part is somewhat pointless
Not so! Use those surfaces to create a non-merged solid body, and then use the Combine function with the Subtract option.

Or you could use the Insert > Part function to insert the part with the rib, into the part needing the recess (multi-body part), and then use the Combine > Subtract method.

Or you could use the Insert > Part function to create a multi-body part (of the parts without any rib or recess) and then use the Rib tool twice (once on the inside edges & once on the outside edges) to create the rib and recess ... maybe.

RE: Sweep Unexpected Twist

(OP)
Thanks for the tips. I'm trying a combination of them, but the Combine option is always greyed out. I was playing around witht he subtract option earlier, but it always removed something that I didn't want it to, so I'm likely setting it up improperly. I'll keep playing around with it, but any other tips are appreciated. Thanks!

RE: Sweep Unexpected Twist

kojiai,

Find a local SWUG (SolidWorks User Group) in your area. Your VAR should be able to help locate one for you. If one exists there will be other SW users there who should be able to help you. Your VAR should also be able to offer some training.

The Combine tool is only available in multibody parts ... not assemblies.

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