I have a part design as shown in attached image 1. Now i want to get a skewed version as shown in the attached image 2. It is skewed by 5 degrees. Is there an easy way to do this? I tried to use "Sweep along a guide" with setting Orientation vector. But the normal of the front face is changed compared to the back face (sketch).
Solved! Go to Solution.
Make a copy of the original profile, translate it normal to the plane the to the desired thickness of the part and then rotate the copied profile the desire skew angle. Now simply create a body by using the Surface Through Curves method or use the Ruled Surface function. Just make sure that the Solid Body option in toggled 'ON'.
I think it depends if you want the sides to be a true helical shape or not. "Skewing" or rotating one of two sketches will work with a small angle, but with a larger angle, the sides will not be a true helix.
It also seems unnecessary to require two sketches which are identical, except rotated.
If you were using I-deas, you could Extrude with a twist angle, but you are not.
Instead, you can take another feature from I-deas that has been added to NX: Variational Sweep.
What I did was
The variational sweep command will then sweep your sketch along a the path, and rotate it based on the parameters of the Helix curve. You can then edit the parameters of the helix to change the rotation angle.
With this method, you get helical sides, not ruled curves. This will become important if you change your angle to something larger than 5 degrees.
But now that I see what Rick Hebert showed, I like his method better...