Sweep Unexpected Twist

[kojiai]

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?

 

[rbpmc]

you might try direction vector and select a vertical edge

 

[JMirisola]

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

 

[kojiai]

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.

 

[CorBlimeyLimey]

Have you tried using the Lip/Groove tool?

http://help.solidworks.com/2013/English/solidworks/sldworks/hidd_dve_lip_and_groove.htm

 

[kojiai]

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?

 

[tgrimley]

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

 

[kojiai]

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.

 

[MartinShane]

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.

 

[snowshoe2]

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

 

[kojiai]

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!

 

[snowshoe2]

The function is called "Thicken", I hope it helps.

http://help.solidworks.com/2013/English/SolidWorks/sldworks/HIDD_DVE_FEAT_THICKEN.htm

 

[kojiai]

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.

 

[snowshoe2]

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

 

[CorBlimeyLimey]

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?

 

[kojiai]

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!

 

[CorBlimeyLimey]

I thought I had it, but there are a couple of problem areas you will have to work on. You may have to do a bit more surface wizardry to create a better blend.
Hopefully the attachment will give you a good start.

 

[kojiai]

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?

 

[CorBlimeyLimey]

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.

 

[CorBlimeyLimey]

Here's a clean version. I don't do much with surfaces, so there may be more efficient methods, but it was a good refresher/learning exercise.