Cannot Sweep Rectangle Along Helix

[Anonymous]

Hi there.

I want to create a sweep of rectangular profile along helix curve, but I cannot make one. It says, " The attempted operation did not produce a meaningful result. Try with different inputs." I do can make a sweep of circle profile along the same helix, but not for rectangular profile. Can anyone help me? (pictures provided below)

[JDMather · Accepted solution]

Isn't the sweep going to be self-intersecting?

What is the purpose of creating 3D sketches?  Wouln't the Coil feature be a lot easier.

Can you post a picture of something similar to what you are really really after?

Without an image for reference - I am going to guess that the helical feature doesn't actually go to the axis of revolution in the real world part.

[Anonymous]

Hi JDMather! Yes that is definitely what I wanted to make. It does work making that rectangular thread by using coil instead of helix. Well, I want to know what is the difference between coil and helix? It seems pretty similar though, hmmm I think I'd better create another topic for this matter.

Thanks anyway JDMather!

Cheers,

Brian

[Anonymous]

JDMather, sorry I'm asking another question.

What if I want to make a rectangular coil just like the one above, but only I want one of the edge of the rectangle intersecting with the center of rotation's axis.

I tried out to make one (see the image below) but it again failed. Do you have any idea?

Thanks before,

Brian

Attachment:

Not Intersecting axis:

Intersecting axis

[JDMather]

First - the very purpose of this forum is to ask questions, so you cannot possibly ask too many questions.

Have you installed all Service Packs and Updates for your version of Inventor?

You asked the question of why to use Coil or the Helix in 3D sketch.

I never ever use the Helix in 3D sketch because it is harder to create and as far as I know (I haven't checked in later releases) it isn't fully parametric - which makes editing more complex.

But - I often have a need for a 3D helix curve.

To get this - I simply Coil a line as a surface body.

Which leads in to the intersting part of the problem.

When you use Coil feature for a circle or any profile - the profile is not perpendicular to the start of the helix, which means the cross-section at any point normal to the curve does not match the profile.  Many people miss this.  (in fact with a circular profile - any section taken normal to a point on the helix would show that the profile is not actually circular, but eliptical)

So, the solution is to get the helical curve (I use edge of helical surface which is trivially easy to edit using the Coil command rather than 3D sketch) and then create a workplane normal to the start of the helical curve.  This ensures that your sketch is normal to the path.

see attached

[Anonymous]

Dear JDMather

Thank you for the reply. Firstly I'm sorry that I asked too much question in one thread. I should've make new thread for another question. For the change, I put all related keywords in the tags so people can find this thread easily when they need it.

Thank you too for the explanation!!! I have seen the attachment and I tried to reproduce the design and I have done it. So the idea is to make the 3d curve with a coil feature and a 3d sketch (include geometry -> click on the inner  edge of helix.) Thanks for the instructions brother.

Peace,

Brian

[JDMather]

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@Anonymous.itprawira wrote:

... make the 3d curve with a coil feature and a 3d sketch (include geometry -> click on the inner  edge of helix.)

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You do not need to do this step in later versions of Inventor - Inventor will do it for you when you run the Sweep command and select an edge, Inventor automatically creates the sweep path.