Cutting Parameters for 1" Endmill Interpolating 2" Hole

[daedalus0x1a4]

Hey guys,

I have a Hanita Varimill 1" x 4" (TF4V6525028) trying to mill a 2" bore into a block of A36.

The depth of the cut is 2.813".

To start I drilled a hole and ran a helix to the bottom of the hole now trying to spiral interpolate with a 0.100" step over.

There didn't seem to be enough room for the chips to evacuate. The hole filled up then the end mill chattered it's way through and wrecked the finish.

Now I am back at the drawing board trying to figure some cutting parameters that will work.

Had great success using a 3/4" x 2.25" with a 0.075" step over at a depth of 1.5" so I figure lowering the radial engagement and adding more air could solve the problem. But maybe I should rough it in multiple depths like d/2? (1.4075")

Any suggestions?

Thanks,
d

EDIT: Forget speed and feed. 600 SFM x 0.006" LPT

[Geof]

I have had similar problems with chip clearance. One time I solved it by mounting an air nozzle that could be directed into the hole to blow the chips out. It was a case of doing a bit of machining, lift the tool and move the job under the nozzle to blow chips then go back to cutting.

[DMF_TomB]

Hey guys,

I have a Hanita Varimill 1" x 4" (TF4V6525028) trying to mill a 2" bore into a block of A36.

The depth of the cut is 2.813".

To start I drilled a hole and ran a helix to the bottom of the hole now trying to spiral interpolate with a 0.100" step over.

There didn't seem to be enough room for the chips to evacuate. The hole filled up then the end mill chattered it's way through and wrecked the finish.


EDIT: Forget speed and feed. 600 SFM x 0.006" LPT

of course the simplest thing is lower step over. not sure how many flutes the end mill has but i think your stepover and feed is way too high. also try leaving only 0.010" or less for a finishing pass.
my calculations show a step over of 0.016" or less at that DOC

[daedalus0x1a4]

To clarify: Varimill Endmills are only manufactured with four or more flutes from solid carbide. This particular endmill has four flutes.

Lowering the load per tooth seemed to add to the problem which generally tends to be the case when making deep cuts with large diameter end mills.

Reducing the step over to .050" helped marginally but not enough to keep the vibration out of the cut.

Going to try to increase the feed to .010" per flute tomorrow. Will lower step over to .030" if that doesn't work.

[BobWarfield]

To clarify: Varimill Endmills are only manufactured with four or more flutes from solid carbide. This particular endmill has four flutes.

Lowering the load per tooth seemed to add to the problem which generally tends to be the case when making deep cuts with large diameter end mills.

Reducing the step over to .050" helped marginally but not enough to keep the vibration out of the cut.

Going to try to increase the feed to .010" per flute tomorrow. Will lower step over to .030" if that doesn't work.

daedalus, I think your problem is tool deflection leading to chatter.

If you cut at 0.050", and your total stickout is 3", 600 sfm, 0.006" chipload, G-Wizard predicts 0.0016" deflection, which is too much. You want 0.001" or less roughing, and less still for a decent surface finish. If you've got more than 3" of stickout, the situation is even worse.

This assumes you're using your pre-drilled hole to cut the full 2.813" along the flutes.

You can back off several ways.

- Less stepover. You have to go all the way down to 0.0085" stepover to keep that deflection down.

- Helix in rather than circular interpolate. If you use no more than 1" of flutes in the cut you can increase that stepover to 0.063".

Looked at another way, you can only put about 5 HP to work with 3" stickout before you get too much deflection for roughing.

Best,

BW

[daedalus0x1a4]

Bob, I agree.

I have this handy Heli2000 that I think I am going to use to helical interpolate to a rough dimension before bringing in the endmill to finish.

Aren't you the programmer behind the G-Wizard project?

Would you care to share the algorithm you are using to estimate deflection?

[BobWarfield]

Bob, I agree.

I have this handy Heli2000 that I think I am going to use to helical interpolate to a rough dimension before bringing in the endmill to finish.

Aren't you the programmer behind the G-Wizard project?

Would you care to share the algorithm you are using to estimate deflection?

Yes I am the author. Gotta pass on sharing the algorithm. It was a lot of work to research it and get it implemented, and is one of the big advantages for G-Wizard. Lots of late nights spent reading very boring Mech E journals, LOL.

Cheers,

BW

[Geof]

Spiral out using a series of interlocking semicircles increasing the radius 0.01" per semicircle.

At 600 fpm which is about 2300 rpm, with an effective chipload of 0.024" per rev means your feed can be very high due to radial chip thinning. You could be up somewhere around 250 to 300 ipm.

Programming the interlocking semicircles is tedious and probably not worth it for just a few holes but if you are doing fifty or more it is worth spending the time.

Spiralling out like this creates lots of thin chips which don't cause as much clearance and recutting problems. It also spreads the cutting over the length of the tool rather than concentrating all the cutting on the tip which is the case with helical interpolation. And it can be way faster.

[daedalus0x1a4]

Geof: I'd have to see a picture but if I understand what you are saying that is how I was doing it, except the step-over was about 10x what you recommend.

Bob: I understand, it's likely that I will have to do the same. There are some interesting research papers out on the subject.

[Geof]

Here is a picture of the toolpath run in Graphics on a Haas. It looks like a spiral but each semicircle is a constant radius just with the centerpoint offset.

Here is the program that starts with a 0.92" drilled holes and spirals out to 1.50" diameter at 0.02" per semicircle.


%
O11111 (FAST INTERPOLATION)
N1 (STARTING WITH 59/64 HOLE)
N2 G90 G54 G40 G49 G20 G80
N3 G53 G00 Z0.
N4 (---------)
N5 G10 L12 G90 P1 R0.625
N6 (---)
N7 T1 M06 (5/8 FOUR FLUTE MILL)
N8 G43 H01
N9 M03 S4000
N10 G00 X0. Y0. Z1.
N11 Z0.1 M08
N12 G41 D01 G01 X0. Y0.45 Z-0.8 F200.
N13 G03 I0. J-0.46 Y-0.47 F100.
N14 G03 I0. J0.48 Y0.49
N15 G03 I0. J-0.5 Y-0.51
N16 G03 I0. J0.52 Y0.53
N17 G03 I0. J-0.54 Y-0.55
N18 G03 I0. J0.56 Y0.57
N19 G03 I0. J-0.58 Y-0.59
N20 G03 I0. J0.6 Y0.61
N21 G03 I0. J-0.62 Y-0.63
N22 G03 I0. J0.64 Y0.65
N23 G03 I0. J-0.66 Y-0.67
N24 G03 I0. J0.68 Y0.69
N25 G03 I0. J-0.7 Y-0.71
N26 G03 I0. J0.72 Y0.73
N27 G03 I0. J-0.74 Y-0.75
N27 G03 I0. J0.75 Y-0.75 L3
N56 G40 G00 X0. Y0. Z1. M09
N57 (-----)
N58 G00 Z1. M09
N59 (--------)
N60 T1 M06
N61 G40 G53 X-13. Y0. M30
N62 (-----)
%

[daedalus0x1a4]

Yes, I use that kind of toolpath to control cutter engagement often.

Unfortunately, I did not have any success using the endmill in this manner and ended using a 1.25" Iscar Heli2000 to helix through the bore.

The surface finish isn't what I desired but the dimension is good.

It isn't a problem except on the next dash number there is a slot that is 6.5" x 8" this part. I was going to flip it and do the finishing in two sections 4" at a time. But if I can not get this endmill to perform then I do not know what I am going to do.