Need Critical Help on Helix Cut

[DesEngineer4]

Hello,

I need some critical help on Helix Cut in UG NX 11. I'm converting one dumb solid to Parametric part. I didn't understand where I went wrong in making a Helix cut, I have added helix and Thread triangle. I have tried couple of times but failed. Could anyone help me on this? I have attached the working sample part; in the same part you can see dumb Parasolid.

Thanks in advance for your help.

Thanks & Regards

 

[cowski]

Use the swept command. Pick your sketch for the section curve and the helix for the guide curve. Turn on the "preserve shape" option and for the orientation choose "vector direction" and pick the axis of the helix (+Y in your case).

www.nxjournaling.com

 

[DesEngineer4]

Hi Cowski,

I tried as per suggestion, but it is not subtracting the material. I tried with Boolean operations as well.

Thanks & Regards

 

[cowski]

If you sweep the current geometry in your file, the result is completely within the solid cylinder. Uniting will have no effect and subtracting won't have a visual effect (but you will have a void in your solid). Adjust the size of your cylinder and/or the swept to get the proper result.

www.nxjournaling.com

 

[DesEngineer4]

I have observed one more issue, the helix I have added is 3 turns, first 2 turns were matching with dumb solid but 3rd turn is not matching.. Any idea?

Thanks & Regards

 

[SDETERS]

I measured the pitch of the original part at 5.1089901240000000 You have 5.08 It also looks like the I.D. gets a touch smaller as it goes around the helix. A radius change of 0.1354021660000000 per turn.

 

[DesEngineer4]

Hello,

Even after increasing the pitch, I'm unable to match the profile.

My thread requirements

Major Dia 59.53
Minor Dia 51. 05
Pitch 5.08
Thread length: 15.24
Angle; 60

Can someone please help? I tried nearly 10 iterations still failed

Thanks & Regards

 

[SDETERS]

Try these Helix values. Also you will need to move the helix up so it is aligned in the middle of the start of the thread. Also you need to change your sketch so the tip of your tooth to 25.92285172 is at the minor diameter

Your sketch profile does not exactly match your tooth.

I would suggest doing a sketch, then do a curve intersection and get the exact dimensions of the thread tooth. When you sweep, make sure you have preserve shape turned on, and sweep orientation is vector direction, which should be the y direction.