Peel Mill

[Newbeeee™]

Just finally gotten around to trying the peel mill in anger today.

St Stl 316 producing a slot 3.5mm wide x 3.5mm deep on a prototrak R8 knee mill.

Length of slot 550mm.

3mm cutter

3.5mm doc

0.125 stepover

Feed 200mm/min

Speed 3000 rpm

Coolant

Tool looked new after and no burrs with mirror finish.

Hats off cnc. This toolpath is gunna get used a lot from now on.

[Goldorak]

i use peelmill about everyday , i always get good result

 

i simply use toolpath trim to cut the unnecessary movements

[TheePres]

I have a plate of A36 4" x 36" x 170" thats all pockets.

Would peel-mill be efficient toolpath to cut pockets, or stick with high-speed pocket with trochoidal moves?

[Goldorak]

^x1000

 

dynamic HST is almost the best 2D HST , you can rough about any shape with a fast and clean toolpath

 

since X4 i never use pocketing or core roughing on any of my job

[Chris Parish]

Goldorak:

 

clean toolpath...yes... but fast I haven't found that to be...we cut several parts and found that the "legacy" style was faster but a lot of climb/conventional direction cutting

 

As for the "Dynamic pocket"..it was great for tool wear.

[neurosis]

CParish,

 

You have to change your thinking a little to use dynamic hst efficiently. It is a high speed tool path. Used correctly, you can feed your tools much faster achieving much higher material removal rates. Some times it doesnt make sense to use this path, but used correctly when the situation calls for this type of strategy, it is a very nice path.

[Dave.L]

quote:

---

With a 12k spindle I could have been cutting at close to 500 IPM.

---

Maybe if the features are large but on small features the machine will not respond well enough and the features will be way out of spec. (my experience)

[Tony35]

colin

were you using G5 P10000?

[Goldorak]

i just rough a pocket with a 7/32 EM at .725 DOC 12% step over at 350 ipm

 

took less than 5 minutes to cut roughly a 4x5in pocket with .25 corner radius

 

instead of drill/rough /finish/rest mill

 

1 tool do the job faster than 4 tool

 

and i don't had to hold the part with 40 clamps to hold it in place , just 2 is more than enough

[Tim Johnson]

What do you think I can achieve with a 1/4" varimill at .680 deep in 20CB-3? I'm currently running at 100sfm/.001fpt at .125doc/65%-80%woc with about 2 hours of cutting life.

[Dave.L]

be aware that the more passes you make, the more the tool will wear and that's why in many cases a heavy cut can provide better tool life. However, IMO it all comes down to how much volume can you remove with the tool and obvioulsy the fastest method to remove the volume.

[TheePres]

Sounds all awesome, perhaps by the time X6 is out i will be experimenting with these X4 toolpaths.

[Tim Johnson]

Wow Colin, if I can kick up to speeds/feeds in this material to your specs that is a monster volume upgrade. I'll give this a shot on Monday. I understand chip thinning but standard thinning at .035 would bring the feed up to .0016 per tooth. (yes it's four flutes) Can you normally double up speed/feed specs without burning or snapping the tooling with this process? 20CB-3 sort of machines like a stainless but it also generates heat like a nickel alloy.

[Tim Johnson]

Colin,

 

This is on a 1-1/2 and a 2 year old Enshu JE80S horizontal with a Fanuc 18i control. Max rapid/feedrate is 3543ipm(90000mm) x,y,z. This is a sensitive part so I won't be able to show it. The material is 1"x1_3/4" flat stock sawed to 1.6". The outside shape of this part is something like a very fat smallcase lower case letter t (or a cross) with various recesses and is also where most of the material is removed. The wings of the "t" are posts .66" tall and the floor is about 3/8" thick. The intersection of the posts and floor must be sharp. I use a separate sharp 1/4" stub length for finishing the floor at a 30% stepover. This surface requires a mirror finish with absolute flatness and using a larger em or a larger stepover increases the amout of polishing and the subsequent possibility damaging the flatness. There are currently 28 tools being used with the smallest drill at 1/2mm (.020) and the smallest em at 1/32". One part currently has 6 hours of machine time in three operations. The 1/4" roughing op takes a little more than 1/2 hour of that time and right now is my best opportunity to decrease this time cost.

[Dave.L]

That's a very small part (similar to what we do) to run very fast feedrates since the machine (our Mazak's) can't move that quick in small features. I would be interested to know how your machine performs. Recently I was engraving a part with .06 tall letters (.005 deep) and I was going 100 IPM and needed to slow down to 60 IPM so the letters could be read. And even at 60 IPM they were still not perfect (probably would have needed to be 40 IPM)

[Tim Johnson]

Dave,

The Enshu website used to have the acceleration specs but I see they dumbed the website down. I think it's 1g. The highest feedrate I've programmed is 1620ipm but the fastest feed I've seen on the screen was about 12-1300ipm on an 8"? cut. We run a 303sst heatsink with a 1/8" high feed mill at 15000rpm, 330ipm, .005doc. The longest slots are just under 2" and on those slots we do hit that feedrate. I don't worry about part integrity, I just set my finish feedrates and let the contour control (G05.1) worry about that.

 

Ok back to peel mill

[Josh Kinney -Elite Engineering]

I use this toolpath on an ancient Fadal VMC with what seems to be a 1hp spindle.

 

316L

1/2" 4 Flute

800SFM

0.030" Radial DOC

1" Axial DOC

90IPM

0.010" Microlift

150IPM back feedrate

0.125" rounding Radius

 

It just plain rips material out and the spindle load is nill.

 

You have to be careful with the transition from cutting to back feedrates. If your machine is not tight (like mine) then you need to play with this and the rounding radius to keep it from banging. Also use the arc filter to get the code down in size. Use "retract at distance" and play with the lenght to get the tool to retract instead of traveling around the part if using a core rough.

 

I live by this toolpath. especially on Stainless and Tungsten parts....

 

I use dynamic mill for core roughing and pocketing and peel mill for cutting slots and even contoured features. I cut through 1" thick tungsten in an arc with peel mill at 90IPM at full depth...

[Dave.L]

Tim,

 

Thanks. BTW, I was not trying to hijack the thread. I have just been disappointed when I can feed anything close to what the cutter can handle if I want to make in-tolerance parts.

 

We will try these paths on roughing in the future.

[gcode]

I've got a job coming up that has 2 .280 wide

slots in 302 SS.

The part is .400 thick and I have to work on both sides.

I was thinking I'd try 3/16" 3 or 4 flute and

rough with a peel mill .200 deep from each side, then finish with a 1/4" from the second side.

Does a 15% radial stepover sound about right for a cut like this??

 

[ 08-29-2009, 08:43 PM: Message edited by: gcode ]

[35K chipper]

gcode, ever use any destiny tool 3/6 raptors? i use them in 303 all the time. i got to try them with peelmill. the dealer in your area is

HIGH DESERT TOOLS Riverside CA 661-945-4323

 

35k

[gcode]

I checked Destiny's website and NuTech Sales

out of Brea is our main perisables supplier.

We have a couple of vending machines to dispense

inserts, drills traps etc and Nu Tec stocks them.

That will make it easy to try some of thier tools.

Thanks for the lead

[35K chipper]

i love these tools. for example .500 3flt .625 loc at 30000rpm at 1400ipm viper stealth. get me another chip barrel please.

35k

[mig]

can anyone put his file on ftp with good example of peel mill or dynamic mill usage?

[Dave.L]

Did I read this correct? 30K RPM?

[Tim Johnson]

Colin,

 

You're killing me man. I was just starting to warm up to the idea of 200-250sfm, now 400?