SPEEDS,FEEDS,TOOLS,ANYTHING, HELP!!!!

[GREG]

We are trying to machine a pocket with islands 2.2" deep. The max cutter dia is

3/8 and the mat`l is 6061 T6 aluminium.

M/c is a 20000rpm horozontal Makino.

Chatter every where,and we have 500parts to make.

Any tips , strategys, tooling recomendations,

speeds,feeds, anything to stop my arse getting kicked.

 

Thanks

[cadcam]

can you share the file so i can see how big of a tool and what you are doing now?

put the file on rhe FTP.

my server & i will down load it to see if i can help & mostlikly i can.

[Michael Reynolds]

Hi Greg! My rule of thumb for chatter is...if yer gittin' it, either increase the feed or decrease the speed. The key is, you have to make your tool work harder, so it doesn't just 'sit' there. Also, are you using solid (coated) carbide? That would probably help too.

Hope this helps!

Mike R.

[ 08-31-2001: Message edited by: Michael Reynolds ]

[Charles Davis]

Drill out your corners so the cutter won't get "trapped" and chatter.

Rough and finish with a larger cutter, then use remachining to clean up the missed areas.

Slow the speeds and feeds way down whenever you get a tool whose length/diameter ratio is above about 2.5 to 3.0.

Get a cot and set it in the tool crib, put on a set of headphones, and plan on spending some long nights nursing this one.

[cadcam]

i think he is hanging the tools way out.

alone with thought go in with a standerd as big as you can the a longer one then some of what the others are saying after removing the sock.

[gcode]

Greg,

I'd use an ealier suggestion and pre drill

all corners with a 23/64 drill.

Use the biggest cutter you can to rough down to the island tops.

For a finish tool get a single end 4 flute

solid carbide endmill with a 1 in lenght of cut. Clearance grind the shank about .02

undersized from the top of the flutes

to the 2.2 depth you need. You will have to make multiple passes because you've only got 1in LOC.

For feeds and speeds, I'd start with 1600 RPM

and about 6 ipm. You may need to build the same thing out of a solid carbide rougher

to rough all the stock out first.

This approach has worked for me in the past.

best of luck with your challenging project

[ 08-30-2001: Message edited by: gcode ]

[GREG]

Thanks for your help

We are using solid carbide with a releved shank , drilling the corners,small depth of cut,cant fit any bigger dia cutter in,ect

Just about to try boring corners with finish end mill.

Hope it works for them cause Im off to the PUB

[Trevor Bailey]

Greg,

One thing I do in situations like that is drill the corners as mentioned leaving about .010 stock in corners. For the chain around the floor that your tool is going to follow, change the fillets to be .005 bigger than what the print calls for. Run you routnine, then come back with your .375 finish end mill to "plunge" in the corner as you would use a drill cycle. I would also use a tool with a LOC of .750 to 1.000. Solid carbide of course with a high helix. Add about 20% more to your normal fed rate. This should do the trick.

Trevor Bailey

[Rekd™]

Speeds will do it without boring, redrilling etc.

Run the RPM down as much as 75% to 80% LESS than normal milling for that diameter of cutter while in the corners.

The squeel you get, which in turn creates chatter marks, is because the endmill is not working hard enough. It has time to vibrate from one side to the other, bouncing if you will. Increase the chip load drastically and it should clean up nicely. I'm guessing, but feed about 10-15 ipm and speed about 1000 or less. Maybe as low as 500.

Use the RPM override to adjust during the cuts, and you'll find the right one. Then change the program so you don't have to override it manually.

This method works for most cutters down to .1875 diameter or so.

[beav700]

I just finished five molds Thursday that required some plunge milling with 3/8 ball 2" deep in 6061. First I tried high speed, no go (chattter and tool deflection), then we got 3" long(1" flute) solid carbide four flute .375 ball from J&L for $32.Worked like a dream. Had to slow down the RPM to 2200 and 14ipm feed. Anything higher than that was creating tiny ripples right in the corners, even though I did not hear any chatter anymore.

Get four flutes instead of two. Two flutes cut better in aluminum but are not as solid as four flutes when it comes to deep cuts.Here is a photo I took today of the part.

[ 08-31-2001: Message edited by: beav700 ]

[Guest CNC Apps Guy 1]

I would reccommend 3 flut cutters because you get almost the identical IC (Inscribed Circle) as you get with 4 flute tools AND you get almost the same chip evacuation characteristics of a 2 flute. Kind of the best of both worlds.

JM2C

[Toby]

Greg,

Have you ever tried CGS carb e-mills? They work like a dream reducing/eliminating chatter due to the wierd cutter geometry. You can bury the hatchet and get beutiful finishes at higher feed rates.

[Bob]

E.C Cutting tools

Hitachi Tool Engineering,Ltd.

List No. 1703

For Aluminum EXTRA LONG Length

TWO Helical Flute

Single End with Weldon Shank

Item No. AMX-212

3/8" Dia. of Mill 3/8" Dia. of Shank

Length of Cut 2-1/2"

Overall Length 4-1/4

Hope this cutter info will help

[Ron_Roy]

Howdy All,

A high speed machining method that has worked for me is to finish a layer at a time. When I was machining heat sinks on a part I would remove 0.06" and then finish at 0.06". Then drop down another 0.06" and finish that level. By repeating this process to the desired depth the heat sink fins had much more support and the cutter had an easier time of it due to a small depth of cut. 3 flute is definately the best way to go! At high speeds feed your cutter hard.

Good Luck,

Ron