3D Surfacing speeds and feeds question

[MILLRUNNER]

I had a thread here a few months about trying to understand the 3D surfacing side of X9 if I was on mill level one. I have gotten all that straightened out now and have my bearings. It turns out, level one will do surfacing, but only on one surface at a time. That is perfectly fine for what I am doing at the moment. I am able to use the feature just fine and have already created a few tool paths.

 

I have never done any 3D surfacing stuff, and the first thing that stands out is the machining time, especially with small stepover. The only thing I can figure on this is that since the stepover is so small, the tool should be able to withstand significantly faster speeds and feeds.

 

Is this something that the typical speed and feed calculators have provisions for? I have never looked at that side before.

 

Also, I guess that larger stepover is ok for roughing type operations, and then save the small stepover for final finish passes.

 

What I'm doing will be roughing with a .25" ball, and then finishing with a .125" ball.

 

I have a 10K spindle.

[AMCNitro]

Remember that the bigger the diameter of the ball endmill the bigger the stepover you can go with.  The bigger endmill will leave a shorter scallop which translates into a better finish.  

What material are you cutting?  Also, do you HAVE to use a ball?   If you use a BULL(or rounded edge flat) endmill you will get a better finish, but if you have features that only a ball can get into...

[MILLRUNNER]

Ok points taken. I actually have a half inch ball to use as well, and this might be better for the roughing. As far as the bull, I don't really have any endmills that have corner radius at the moment, but I'm just thinking of how the compensation would work. Would I run on left or right cutter comp vs Center or off?

 

I was using the .125" tool because I have a feature that needs it, but it amounts to about 5% of the overall surface operation. I may split that off into its own little surface, and then use the .125" tool there. I need a .065" internal radius and that's why I'm using that tool. I had it finishing the whole op though, and that was taking forty forevers with a .002" stepover.

 

I may go back with the same .25" ball tool that I did the roughing with, and try to make a finish pass with it on the 95% of the surface that remains.

[JayM]

 

 

Would I run on left or right cutter comp vs Center or off?

Surface toolpaths do not use compensation (G41/G42).  All motion is calculated from tool centerline, Mastercam will offset the XY position based on the tool diameter and tool nose radius.

 

 

I was using the .125" tool because I have a feature that needs it, but it amounts to about 5% of the overall surface operation. I may split that off into its own little surface, and then use the .125" tool there. I need a .065" internal radius and that's why I'm using that tool. I had it finishing the whole op though, and that was taking forty forevers with a .002" stepover.

 

I may go back with the same .25" ball tool that I did the roughing with, and try to make a finish pass with it on the 95% of the surface that remains.

 

If you find yourself programming these features often I would look into upgrading to Mill 3D.  The restmilling operations will save you a lot of time programming and machining.

[absolute technologies]

We routinely finish keller heat treated stainless at 500-1000 SFM and up to .010 IPT so a 1/2" ball end mill will be over 150 IPM. However your tool can't be running into to other features at that high of feed rate.  We typically finish the adjacent profiles prior to finishing the surfaces this way your tool doesn't run into them when finishing the surfaces. There are times I even trim the surfaces and shorten them up by .010 or so as to prevent the tool from leaving small gouges caused from the servos over-shooting at the higher feed rates. Definitely use high speed look ahead if you have it and any time you can post G2/G3 do so because the servos will typically get to the programmed feed rate faster than point to point on most controls. Also if you're going to do a lot of kellering it can be cost effective to have your servos tuned to optimize the acceleration/deceleration. Most machine tool builders use a generic parameter set for their servos and don't optimize them on each machine built. Also a 4 flute end mill will have twice the feed rate of a 2 flute so the more flutes the better, it only takes about 6 seconds for tool change, so put in a multi-fluted tool when ever you can.

 

Cheers!

Len Dye  

[Matthew Hajicek - Singularity]

 

 

The only thing I can figure on this is that since the stepover is so small, the tool should be able to withstand significantly faster speeds and feeds.

 

And you've discovered chip-thinning.  There's a program called HSMAdvisor that will help you calculate how much faster you can push that tool under what cutting conditions, and will actually tell you how much cutter deflection to expect.  The Milling Advisor from Helical Tools is similar though not as full-featured.