Eliminate twisting from sweep around a helix

[spopa2]

Hello,

I am having trouble modeling a multi-layered solenoid in solidworks. The issue arises when I sweep a sketch around a 3D curve that describes my helix. Although the sweep is done as “follow path” the shape is produced correctly for the first turn after which it starts sloping instead of staying horizontal to the top plane like I want it to. I have attached the model as an example. Please let me know if you have any ideas on how to fix this.

Cheers,

Sorin

 

[ctopher]

Do you have a picture of what you are trying to achieve?
I looked at your part, but I'm not 100% sure what outcome you need.

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[vigildesign]

I do not see why it is twisting, but I got it back flat by making a new sweep. Use your sketch and 3d sketch from sweep2, then select option for twist along path, reverse direction, then I unput 79 degrees. Odd?

 

[rbpmc]

I ran into something similar, ( sorry I'm not on my Solid works comp, and can't see your part. ) I'm trying to recall this from a few years back. I believe there is a function with in the sweep dialogue where you can keep the twist normal to an edge, select a horizontal edge if available.

 

[spopa2]

Thank you for all the replies.

@vigildesign: I have tried what you suggested, it looked promising in the preview however it did not let me build because it said there would be zero thickness geometry. Did you manage to build your version after making those changes?

Also, I find it odd that this is the solution, I would really like to know what caused the problem in the first place because I need to be able to create multiple models like this with different number of wires/thicknesses and I dont want to use trial and error every time to figure out the angle needed.

@ctopher:
I have attached another part that is similar and does not have the twist I am talking about, however it is has an elliptical cross section.

@rbpmc:
There is no "twist normal to an edge" option so I cant select a horizontal edge as a reference, that would make sense though. I tried giving my sketch relations that say they must remain parallel but sw seems to ignore that as shown by the twist it creates.

If anyone has any more ideas it would be greatly appreciated!

Cheers
Thanks again for the help!

 

[spopa2]

On a side note, in both models the outer wires form bumps/bends on the longer edges of the cross section. That is at the interface of the straight segment and the curves in the first model I uploaded, and in the middle of the longer side of the ellipse on the second model.

The inner wire (whose center follows the 3d curve perfectly) does not show this problem, it is only wires that are farther out. Does anyone know how to solve this?

Cheers

 

[rbpmc]

spopa2... Take a look at direction vector " aligns the profile in the direction selected for direction vector" : Path alignment type becomes available when FOLLOW PATH is selected as the ORIENTATION/TWIST type.

So select Follow Path in the Orientation / Twist Type :then select Direction Vector : then set the twist orientation via a horizontal edge. Hope this helps.

 

[Scheffers]

I played around with your models a bit.. this is what I got..
Got the bumps out of the last model,
The first model you posted, I couldn't get it to work properly.. bumps are diminished though, but the last sweep(7) doesn't seem to cooperate.

 

[Scheffers]

second file.

 

[TheTick]

If you make a pair of helices with same pitch but one with larger diameter, you can use the second for a guide curve. Connect section sketch to guide curve using a pierce constraint.

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