HOW TO EXTRUDE A FEATURE ALONG A TUBE

[imagineers]

I can't figure this out for the life of me lol. I am trying to re-create corrugate fep tubing in solidworks 2010, see attached. I want the corrugate to be tangent to the tubing along the path as it would in real life. I can pattern it using sketch driven but the corrugated bumps won't stay tangent to the path as it patterns, it won't let me. Can anyone help

 

[StrykerTECH]

I am on 2009 so I can't see your part. But I can tell you you have to piece it out in 1 plane only, you can't use a 3D sketch. then hit the check box tangent to curve, on a curve driven pattern.

StrykerTECH Engineering Staff
Milwaukee, WI

http://www.stryker-tech.com/

 

[imagineers]

Ahh, that sucks. That is a pretty serious limitation for Solidworks I think. There must be a way. I have once seen a wire made in SW once where it had handles that you could twist the wires by adjusting these handles, almost like the wire was a piece of string you could mold twist into whatever shape you want. Maybe you can start the tubing straight then find a way to make it bend ?

 

[DesignerGuy16]

Swept boss/base.

Basically make a 2d sketch on a plane for your profile, then a 3d sketch as your path. For the 3d sketch, make sure it intersects your profile. If you need to control twist, make a 2nd 3d sketch just like the first and use that as a guide curve.

Should be able to do that in any recent versions of SW.

James Spisich
Design Engineer, CSWP

 

[DesignerGuy16]

Nevermind, I just looked at the model, was something completely different.

A few notes:
For any type of pattern like this to work, the profiles need to be dead nuts from one to the next. Ie, if you need to make a second 3d sketch for your pattern path, convert the existing path from the other. You may need to start the nub feature at the start of the tube profile, and then extend the profiles after the fact from the nubs.

From looking at the model, don't just fix the base 3d sketch in space, use the origin to define the start point. You can fully dimension and define, even the most complex curves with construction lines, angles, and curve distances.

Start by cleaning up what you've got and it may just work.

James Spisich
Design Engineer, CSWP

 

[imagineers]

really hard to do. I settled for extruding a ball shape along the 3d path, it's not perfect as you do not see the proper separation between the arches, but from a distance you cannot tell. If anyone comes up with anything feel free to post

 

[itrans]

Have a look at this, hopefully it will do for you or you can modify as you see fit. I used your base model as a starting point. You can hide the first Surface Sweep feature if you want.
(Unsuppress everything to see the model)
Cheers

Itrans

 

[imagineers]

itrans, that appeard to work. So you swept a line along a path and followed it, then used that surface as the face to be normal to when using curve driven pattern. I would have never guessed this. Thanks.