Showing results for 
Search instead for 
Do you mean 
Reply

Helical Milling Airfoils - Any Ideas?

[ Edited ]

I am trying to make an airfoil milling program that is ran on a vertical 5 axis head/table machine, I want to helical mill from one end to the other keeping the tool axis normal to the surface.  My problem is that I can't get a clean tool path that doesn't gouge the part in Vericut.  I am including a file with a sample airfoil and the toolpath I used.  Any help is appreciated....

 

Thanks,

Jon

12 REPLIES

Re: Helical Milling Airfoils - Any Ideas?

Blade? I don't understand what you want... "Nice" toolpath. I cannot see any gouges. May be you must to set right preferences inside VERICUT - motion tolerances etc.?

 

But - milling a  same part with ball tool and normal to part is not a best method. I think more better will be use rounded end mill. My opinion only.

Re: Helical Milling Airfoils - Any Ideas?

Not sure where the gouges are or how deep.  I noticed that the tolerances are set to plus and minus .001.  This give NX the "OK" to gouge the part by .001".  It will be especially noticed on the smaller edge rads.  For critical surfaces like these, I would set the intol to zero and the outtol to about .0005.  Also, when selecting the part faces, you might give the small edge rads a custom tolerance that is tighter.

 

Hope this is helpful.

 

George

 

George Bennett
All NX versions
W7 Ultimate
Dell Precision M6700
Spirit of Innovation

Re: Helical Milling Airfoils - Any Ideas?


Not-Yet-Retired wrote:

Not sure where the gouges are or how deep.  I noticed that the tolerances are set to plus and minus .001.  This give NX the "OK" to gouge the part by .001".  It will be especially noticed on the smaller edge rads.  For critical surfaces like these, I would set the intol to zero and the outtol to about .0005.  Also, when selecting the part faces, you might give the small edge rads a custom tolerance that is tighter.

 

Hope this is helpful.

 

George

 


It appears to be gouging on the edges only, according to vericut the gouges appear to be around .005.  I was thinking this might be due to maybe too much rotation at a single point and the spindle is not keeping up with the rotary or vice versa.  Of course some of this could be wrong in Vericut as well, but I don't want to run a part to find out.

Re: Helical Milling Airfoils - Any Ideas?

[ Edited ]

Did you try adjusting the tolerance?  If the results are different but still not 100% then you may be on the right track.

 

I saw a trick about ten years ago presented by a consultant at NCExperts.  He created offset faces from the part faces.  The offset value was equal to the tool radius (tight modeling tolerances required before offsetting).  Then, he drove the center of the ball mill on the offset surface.  Because the offset surface was bigger, there were more tool path contact points on the small rads.  I don't mill blades for a living so I don't know of a better or more modern approach.  Also, you can specify the maximum tool axis change which will reduce the size of the facets on the small rads.  Depending on the controller type, there may be some smoothing codes available to help.  One thing for certain though is that you should not be milling the edges at plus and minus .001 tolerance.  You need to minimize the facet sizes and they should all be on the plus side of the part.  You may be able to add some decimal places to the outputs.  Some machines take up to 6 decimals for linear and rotary axes.

 

Good luck

George

 

George Bennett
All NX versions
W7 Ultimate
Dell Precision M6700
Spirit of Innovation

Re: Helical Milling Airfoils - Any Ideas?


Not-Yet-Retired wrote:

Did you try adjusting the tolerance?  If the results are different but still not 100% then you may be on the right track.

 

I saw a trick about ten years ago presented by a consultant at NCExperts.  He created offset faces from the part faces.  The offset value was equal to the tool radius (tight modeling tolerances required before offsetting).  Then, he drove the center of the ball mill on the offset surface.  Because the offset surface was bigger, there were more tool path contact points on the small rads.  I don't mill blades for a living so I don't know of a better or more modern approach.  Also, you can specify the maximum tool axis change which will reduce the size of the facets on the small rads.  Depending on the controller type, there may be some smoothing codes available to help.  One thing for certain though is that you should not be milling the edges at plus and minus .001 tolerance.  You need to minimize the facet sizes and they should all be on the plus side of the part.  You may be able to add some decimal places to the outputs.  Some machines take up to 6 decimals for linear and rotary axes.

 

Good luck

George

 


I changed the tolerance which gave a smoother appearance in vericut, it still shows it undercutting.  But when I pause the simulation right when the tool reaches the edge and then step it through with the design model turned on, it looks correct and the tool doesn't appear to violate the design model but the stock model still cuts below so when doing an auto-diff it shows gouging.  I also set the max angle change to 15 and the minimum angle change to 1 which I am hoping helps.  I created a tracking point on the tip of the tool in hopes that it tell the software what I want to be touching on the surface.  I am curious if changing the tool position from tanto to on will help any.  I looked at my dummy file and the in/out tolerance is set to .0001, not sure how it got set to .001.  But I did as you suggested and set the in to 0 and the out to .0005

Re: Helical Milling Airfoils - Any Ideas?

It's getting down to tolerance management I guess.  Try changing the max angle to .1 degree.  If it helps, you can back it off until you find a reasonable limit.  Also, what is the tolerance of the blade you're milling?  If it's say, +.0015, use an outtol of .0013 and a negative intol, say -.0005.  You need to have a lot of points on those edges to keep the facets down.  If you have more than one VC machines with similar kinematics, try the other machine and look for differences.  Could be that this particular VC machine isn't properly using G43.4 or TRAORI or whatever code applies to your machine.  You probably need to hear from another user that is closer to your issue.

 

George

 

George Bennett
All NX versions
W7 Ultimate
Dell Precision M6700
Spirit of Innovation

Re: Helical Milling Airfoils - Any Ideas?

[ Edited ]

My opinion is that who knows how well vericut matches the machine in interpolation between the points. Whenever a big kinematic change (rotaries moving fast - long pivot lengths) is taking place - I am not sure if Vericut is exactly performing like the machine. Basically like George says but I wonder what is happening in the Vericut end. Well - now I read that George just said that - nevermind. I know there are settings in the "traori" options in vericut for various behavior. They have one sample part that shows the options.

NX10.03
Windows 7 Pro

Re: Helical Milling Airfoils - Any Ideas?


Study wrote:

My opinion is that who knows how well vericut matches the machine in interpolation between the points. Whenever a big kinematic change (rotaries moving fast - long pivot lengths) is taking place - I am not sure if Vericut is exactly performing like the machine. Basically like George says but I wonder what is happening in the Vericut end. Well - now I read that George just said that - nevermind. I know there are settings in the "traori" options in vericut for various behavior. They have one sample part that shows the options.


 

I have the same concerns, I know our vericut file is most likely not set up properly but I do not have the knowledge to ensure that it is.  I really hate to just cut a part and "see" if it is right, eventually that is what I will have to do but that will come after I have tweaked all settings possible.

Re: Helical Milling Airfoils - Any Ideas?

I believe the issue is that the leading edge surface is not tangent to convex and concave surfaces.

 

I noticed in TOOLPATH VERIFY that there is a small "back-up" move when the tool hits this non-tangent area.

 

If you fix the surfaces I believe your problem will go away.

 

Tony Centa

GE Aircraft Engines

Wilmington, NC

Learn online





Solution Information