Peel Mill

[Newbeeee™]

Used the peelmill a few times since my first post.

We bought a new vice for the prototrak, and decided to cut off the cast rear mounting lug.

50mm thick cast iron, full doc with a 12mm solid carbide making a 13mm wide slot.

It went through like butter!

 

mmm, looks like we'll be trying dynamic mill toolpath next.

Cheers

[Thee Rickster ™]

Has anybody found a desire to use peelmill or dynamic in Grahite? Do you think there would be any 'significant' advantage pocketing using these methods?

[Newbeeee™]

When I was 'playing', I did a couple of 6mm wide slots by 8mm deep really close together (in ally).

There was only .5mm (20thou) of material in between. This was just to see if the strategy would be any good making heatsinks (fins).

The sidewall finish was better than 16cla and the walls were straight and parallel.

Because the toolpath is light loads (small radial cut), I assume it's low forces so would be OK for graphite (or anything that may be brittle)???

[35K chipper]

colin its 6061 t6 on an okuma u100m glass scales and super Hi-NC with nurbs.

35k

[35K chipper]

oh and thats 3926.991 sfm.

 

35k

[Tony35]

great thread

i have been using peel mill and core mill with great results looks i need to play with this dynamic mill a bit

the key is from what i have found out is to use a coated tool and get the HEAT in the chip i use air on steels and tsc coolant on alum

i use the high speed look ahead (G5 P10000) on those toolpaths so the machine dont jerk around

 

so here is some of my numbers i have been throwing at the machines using a coated 3/4 varimill with a 30hp spindle

 

A2/4140 500sfm 1.0 doc 20% stepover 105ipm

D2 500sfm 2.0 doc 5% stepover 83ipm

AL 10000rpm (max rpm) 25% stepover 465ipm

and i know i could get more out of it

 

like colin said you have to dial the tool in at the machine look at the spindle load and axis loads to see how the tool and machine is performing you will know when its happy, a nice shower of blue chips, part and tool are not hot

[Tim Johnson]

Ok right now the 1/4" em is at 200sfm, .0017fpt, 10% stepover and 40% toolpath radius which brings in the total time from 30 minutes to ten minutes per part. The end mill was really squeaking but looks and feels like new. We're getting two colors on the chips, silver and medium gold so it appears we're on the right path. I'm thinking 250/300sfm on the speed but I'm rather concerned about kicking up the chip load because of the squeaking. Any thoughts? We're running two part pallet loads so I can play but that's still 7-8 hours of run time so I get one to two shots a day.

[Tony35]

sounds like you dont have enough chip load according to the chip color

in a rigid holder?

i get i nice deep blue/purple chip on tool steels

you could decrease the step over to 5-8% and bump up the chip load to maybe .0025

[Tony35]

colin

do you have a spreadsheet or any numbers that have worked for you that you could share with me?

still trying to get more out of my cutters would like to see where i am with them. i know i need to apply chip thinning more than i do (but i get a nice blue chip so i dont mess with it) just need to understand chip thinning a little better

sounds like you have done more of this than me

 

tim

see if you can get a varimill for the job with a good coating you could double where you are now i start at 500sfm .008chip load and work up or down from there

[Tim Johnson]

It looks like the limit is between200/250sfm and .0017ipt at 10% engagement. At 300sfm and .0025ipt we snapped the em about 2 minutes into the part. The second em finished the first part and snapped about 1 minute into the second. It did sound good while it lasted though We ran at 300sfm and .0017ipt lest night and we got lots of chirping and about 4 parts tool life. We're going to finsh the order (six left) at 250/.0017 and see what the em looks like. I'm quite sure the 200sfm would run for quite a while. It sounds more like a squeak than a chirp.

 

Tony,

WE are using the Hanita Varimills with the .016 chamfer (TF4V0507002).

[Tony35]

tim

are you using coolant?

[Tim Johnson]

yes we're using soluble oil coolant. The tool cutting time went from 27_1/2 minutes to 7_1/2 so I'm considering this as a great success. Thanks to everyone that helped in this thread.

[Tim Johnson]

One thing I did have to do was add my "rest milling" contours before the finish mill which in itself was not a problem but trying to peel the contours was. I just need to play with the path a little (lot) more. So... whens dynamic rest milling going to show up?

[Tony35]

tim

if you have air blast i would turn off the coolant and see what kind of tool life you get

i only run coolant on alum

i have noticed that with the coolant on in steels i was getting thermal fracture on the endmill

but if you are going to run coolant be sure the tool is not starved for it use TSC if you have it

glad to see you got the time down

[Tim Johnson]

The nickel alloy materials generate so much heat that coolant is a must unless you're using ceramic inserts.