Create Spiral Groove 1

Jason,

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.

Hi Hudson or Whoever Else That Can Help,

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

I played with this a little and found that after you create a straight helix around the axis, you can project it to the tapered face using "Along Face Normals". The new curve will not be associative, however, so as far as start/end points, you can spin the result curve around its axis until the start is "clocked" correct and then also trim the the other end to the right position. Then be sure to set up your "Section String" normal to the start of the new tapered helix before sweeping. Then when using Swept, for Orientaion choose "Vector" and select the axis of your taper.

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

Jason,
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...

I like Kevin's suggestion of projecting the helix to your surface, and if you toggle the associative option it will update when you update the helix parameters. An alternative would be to control the radius with a law, but that can get complicated depending on your surface and will not be associative to the surface. Also, using 1 helix as the guide string and using the axis as the vector direction does a great job of keeping the section shape from twisting as it is swept.

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.

Jason,

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.