Create Spiral Groove
Create Spiral Groove
(OP)
Hi,
It's been a while since I've done this. I need to make a spiral groove onto a tappered bore. I attempted to use the Helix feature to create my spiral pattern, but when I sweep it, my groove is not going along the tappered face.
How can I make the spiral pattern that goes along the tappered face & allow me to get a "clean" sweep to create the groove? Also, how can I control the length of the spiral to start & stop at specified defined points?
Thanks
It's been a while since I've done this. I need to make a spiral groove onto a tappered bore. I attempted to use the Helix feature to create my spiral pattern, but when I sweep it, my groove is not going along the tappered face.
How can I make the spiral pattern that goes along the tappered face & allow me to get a "clean" sweep to create the groove? Also, how can I control the length of the spiral to start & stop at specified defined points?
Thanks
Jason Misztal
Fuel and Utility Systems
UG Designer
Goodrich Corp.
Rome, NY





RE: Create Spiral Groove
This is a tough one, It is not your spiral but your sweep that is probably causing the problem.
I would need to know what your profile is and something about the process to answer properly. Internal or extrnal diameter shape of groove, round, thread form square etc, and process are going to dictate your technique.
For a rounded oil groove I create a spiral then use it to define a cable of the required diameter which I then subtract.
If it is being produced on an external diameter with an end mill or slot drill type cutter I fear that it is really quite difficult indeed because the diameter of the cutter is at an oblique to the direction of sweep.
Otherwise you need to work up a section of the profile relative to the start of the sweep and the basic helix and possibly develop a second helix as a spine curve to control the orientation of the sweep. Logically speaking if your sweep goes wrong it usually comes down to orientation so that the basic helix tracks only one point on the trajectory and you need to create something defining the part that is going wrong in order to control it.
Hope this helps. Not seeing your part is frustrating I can't be specific to help more.
Regards,
Hudson.
RE: Create Spiral Groove
I am trying to make an internal groove that will be square shaped along a tappered face. I have 2 defined points in which I need to start & stop at & the groove cut will have a .25 depth with a .25 width.
Perhaps, the cable feature will work better than the Helix feasture, but I'm not that familiar with it. How do I get proper orientation, position & get my sweep to cut along the tappered face?
Thanks
Jason Misztal
Fuel and Utility Systems
UG Designer
Goodrich Corp.
Rome, NY
www.goodrichrome.com
RE: Create Spiral Groove
Also try to edit # of turns in the straight helix creation for correct initial start/end positions.
This was on NX3... Not sure of changes ahead.
Good Luck.
Kevin
RE: Create Spiral Groove
We run into this anytime we try to sweep a shape along a helix.
Try your sweep again but use 2 helix curves (or whatever kind if curve you want). It seems like when a section is swept along a single radial type curve it looses it's orientation along that curve so the results are less than what you'd expect.
Good luck
ugdriver
Mama's don't let your children grow up to be aerospace tool designers...
RE: Create Spiral Groove
To get it to start and stop at specific points, the easiest way is probably to make it longer than needed and trim to the required points before subtracting it from the cylinder.
RE: Create Spiral Groove
We're probably on different time zones so hence the delay in answering. I'm now assuming you'll probably create the groove with a boring tool in a lathe.
The taper helix is the go. I found that if you project the curves on onto a tapered hole then the top end of the helix strikes the wall some way below the top of the hole.
You create the taper helix per normal except that for the radius method select use law and input the top and bottom radii. I just measured the radii.
To create a sweep that worked using a square profile that described the size of your groove I first created a sketch of that profile at one end of the helix, normal to the surface. Next I created the sweep using the helix as my only guide curve and the sketched square as the section. Set the alingment method to parameter and the tolerance to zero. Seriously if you sweep a cornered section with any parameter greater than zero UG tends to approximate the section elements and create two single faces where you would natuarally want four in this case or more depending on the section. In the next dialog I selected face normals to square up my sweep by picking the tapered bore, and proceeded thru to create the sweep.
It was still slightly wrong I found, because the groove was narrower that expected, in this case 0.248. I concluded that this was because the swept section was not angled the same as the helix, which is to say slightly at an oblique. I needed a better way, so I decided to sweep just one side of the square that was normal to the surface, to create a sheet that describes on side of the groove. This when thickened the correct amount will descibe the groove. To make an even better job of it if the section curve is enlongated slightly towards the centre of the bore then once thickened the outside may be trimmed off by the bore and then offset by 0.25, then you have a groove you know to be an accurate depth, when you subtract it from the main solid.
Hope this helps.
Regards
Hudson.