Sweep with a non-planar path 3

[mkmech]

Hi everyone

I have a profile which I want to sweep along a curve that is not planar. Is it possible to do this?

Thanks

 

[mmurphy50]

Yes, you can. If you are using a helix I have had better luck converting it to a 3D sketch.

 

[Theophilus]

Usually it's best to create your path first, and then pick the path and one of the path's endpoints to create a plane "normal to curve". On that plane, sketch your profile and pierce it to your path. Create a sweep.

You can also create additional guide curves if necessary to stretch your profile geometry along the way, or to better define twist, etc. along the path.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[mkmech]

Thanks guys! I tried doing this and it almost worked. I created a 3D sketch first to work as the path. Then created a profile perpendicular to it. But when I sweep it, it gives error "Can't create because of zero-thickness geometry". I am not sure what's the problem..

 

[Theophilus]

Zero-thickness geometry would be the same problem I alluded to in my post to your Cavity question--you probably have a place in your sweep where the profile touches itself along the path (either an edge, surface, or point) such that the geometry is logically unsound.

If you post pictures of what you're doing, it could help in debugging your sweep. Make sure your profile doesn't collide with itself while traversing the path (taking too tight a turn in the path) or you'll have more logical problems and the sweep won't form.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[mkmech]

I don't know how to put an image in this forum...anyone?

 

[CorBlimeyLimey]

The FAQ section is full of suprises

faq559-1100 or faq559-1177


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[mkmech]

Thanks guys!!

This is the image:

http://209.250.130.101/downloads/FsxInfo/mybox.jpg

The problem is:

The sweep is following a 3D sketch. The profile goes around the box/base along the 3D sketch and joins the starting point. Now if you look at the top straight edge, you will see 2 faces of the sweep which are separated by a vertical line. That means when sweep comes around the upper left fillet, it doesn't align with the starting face, so there is a gap between 2 faces.

I am not sure how better to explain this, but hope you understand.

Thanks to all the readers.

 

[SBaugh]

Make the sweep path into one composite curve.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[J-C]

I've had this problem before trying to run a gasket around a curved groove and lip. The end faces don't want to line up perfectly so the part has difficulty making a solid. Problem is the sweep alignment when it comes full cirlce, the faces don't match.

What I ended up doing was sweeping half of it, then mirroring. Think I swept it around a little more than half way and used the mid plane to trim it back. Then the mirror worked. Of course you'll have to uncheck "Merge" to do this and then use "Combine" to boolean/add it back to the main body.

Also, you may try a loft with guide curves instead. You may have to extract a second sketch on top of the other one to end the loft or perhaps you can use "Contour Select" to select the one sketch twice.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2

 

[PlasticFantastic]

I have found that fit splines tend to make sweeps work.

 

[sg20]

From your photo, I think using surfacing technique works better. You only need one line to create a surface... and then one line to cut the profile.

 

[mkmech]

Hav eno experience or knowledge of surfacing...any good references/sources on surfacing?

 

[CorBlimeyLimey]

The SW Online Tutorial has a section on Surfaces. That would make a good start ... along with the SW Help file.


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[Plastserv]

The problem is self-intersection. You can convert the non-planer curve to a plane and use that as your path. Then use the non-planer composite curve as a guide curve.

The outcome will be for-shortened dimensions in your profile. If this is a problem you can use a combinations of lofts and sweeps to get around the for-shortning. No magic button. brep.