Carbide conundrum

[derekBPcnc]

Hi,

I have a Bridgeport J head machine converted to CNC / Mach3 / Stepper motors/ spindle VFD etc.

Up until recently I have used standard HSS slot and end mills, but due to wear, I have been experimenting with Carbide tooling.
Even using brand new carbide cutters (2 and 3 flute) I get a lot of chatter and vibration, for example, cutting a 10mm wide slot 10mm deep in ali, 10mm dia cutter, 50mm/min feed and about 2,500 RPM.
With a HSS cutter its a knife through butter but with the carbide it sounds like the machine is going to shake itself apart.
I tested a cut with the axis locking handles lightly nipped and that did not make any difference

I must be doing something wrong (feed /speed/ RPM), can anyone help?

Thanks,

Derek.

[SCzEngrgGroup]

Derek,

That's a mightly slow feed rate, especially for carbide. You're running about 2 in/min. I usually run 1/2" HSS 2-flute endmills at 10 in/min in 6061 at 3100 RPM (with coolant, of course). Carbide should be able to run twice the RPM, twice the feed rate.

Regards,
Ray L.

[davereagan]

What helix and rake on the endmills you use makes all the difference. A standard 30 degree helix will perform very poorly for full slotting compared to a high helix endmill made specifically for cutting aluminum. If you need specific tool parts numers, email me and I'll send you some.

Dave

[littlerobb]

Derek,

That's a mightly slow feed rate, especially for carbide. You're running about 2 in/min. I usually run 1/2" HSS 2-flute endmills at 10 in/min in 6061 at 3100 RPM (with coolant, of course). Carbide should be able to run twice the RPM, twice the feed rate.

Regards,
Ray L.

I am probably totally out of line here, this is not my forum, I am not familiar with Bridgeport, (we do have one but it is in the fab side of the building, with a retro fit EZ trak I think) I am over the CNC side, but we use 2 flute 60 degree helix, Garr 242M endmills for 6061, 1 inch diameter, .75 DOC, 190 IPM. I understand the retro is not going to have that kind of rigidity, that being said I would run that thing as fast as you dare. My two cents, Robert

[DareBee]

I need to agree that carbide is not just carbide (which you already know). There is probably thousands of variations of geometry, grind type, coatings etc.
But
A base rule of thumb is use 1000 SFM for cut calculations and chipload recommendations from the cutter manufacturer.
Such as on this chart.
So I would start out running that cutter (10mm x 3FL) at 9500RPM and 70IPM.
I don't know your max spindle (maybe 4000RPM?) but lets say 25IPM at 3500RPM.
High helix, special alum grind, and/or TiCN coatings or superb for aluminum and can add up to 30% increase in cutting speed and double+ the tool life.

[derekBPcnc]

Hi All,

Thanks for the help.
I have just been trying some test runs.
Spindle speed on max, the head nameplate says 3,600 but I was running at 60hz on the VFD so this will be more like 4,200 (I need to tach this to be sure).

Feed set to 250mm/min (~10"/min).
With a piece of 3/8 x 2" HE30 Ali bar, facing off the end at 4.0mm off the end.....all OK. (Climb milling)
Also OK at 300mm/min (12" / min)....humm that aint bad.

Then tried to cut a slot across the bar at 1/2 thickness (5mm deep) and I got bad chatter. reduced the depth of cut to 3mm and its like a knife through butter.

I think I'm at the limit of my set up in terms of spindle speed, and probably more importantly, rigidity.

Still, I'm now running at 6x the feed rate now and even if I have to run round the profile 3x I'm still twice as quick overall.

I'll experiment with cutters designed for Ali (my current stock are standard helix) to see if I can improve things a bit more.

Cheers
Derek.

[little bubba]

As someone who has a CNC knee mill, I can tell you that due to the quill design of the spindle, they do not slot well at all.

When slotting that quill is just bouncing around up inside the head there, when profiling or cutting only on one side of the endmill, the quill is pushed to the side and everything is good and stable.

You could go with an even smaller endmill and try trichoidial (sp?) paths for your slot, or sometimes ramping down the slot will load the machine up and keep it stable. If that doesn't work, you are pretty much limited to shallow cuts, but you can usually feed really hard and move the material pretty quick.

[SCzEngrgGroup]

I need to agree that carbide is not just carbide (which you already know). There is probably thousands of variations of geometry, grind type, coatings etc.
But
A base rule of thumb is use 1000 SFM for cut calculations and chipload recommendations from the cutter manufacturer.
Such as on this chart.
So I would start out running that cutter (10mm x 3FL) at 9500RPM and 70IPM.
I don't know your max spindle (maybe 4000RPM?) but lets say 25IPM at 3500RPM.
High helix, special alum grind, and/or TiCN coatings or superb for aluminum and can add up to 30% increase in cutting speed and double+ the tool life.

Don't think you'll get close to those rates on a BP - not stiff enough, and not enough spindle power with the typical 1 to 1.5 HP motor. Also sounds like this particular BP may be a bit on the "loose" side.

Regards,
Ray L.

[SCzEngrgGroup]

Derek,
You might want to explore *why* you get so much chatter. Sounds to me like maybe you have some slop somewhere that's getting in your way. Check the leadscrews/ballscrews, quill, and gibs. I think you should be able to do better. Mine (a cheap Chinese/Taiwanese BP clone) runs smooth as can be at 3100 RPM, 10 IPM, 0.6" DOC, even with my worst (5 years old - very dull) Chinese 2-flute end mill.

Regards,
Ray L.

[derekBPcnc]

Derek,
You might want to explore *why* you get so much chatter. Sounds to me like maybe you have some slop somewhere that's getting in your way. Check the leadscrews/ballscrews, quill, and gibs. I think you should be able to do better. Mine (a cheap Chinese/Taiwanese BP clone) runs smooth as can be at 3100 RPM, 10 IPM, 0.6" DOC, even with my worst (5 years old - very dull) Chinese 2-flute end mill.

Regards,
Ray L.

Hi Ray,

Thats interesting and sounds like I should be able to do alot better.
Thinking aloud, I have fitted the cutter into a "blank" clarkeson collet so maybe its got some runout or its just the length.
I might try the cutter direct into a R8 collet just a test, but for "production" using collets will be a PITA beacuse I need set tool lengths entered into the tool table.
FYI, the knee is driven for the Z, the quill is locked about 1/2 way out.
X ballscrew is a new THK ground screw so thats OK, the Y is not as good but OK. I get about 0.015mm backlash
I might try tweaking the gibbs in a bit, maybe they are just a tad too free.
Spindle bearings were replaced by a BP expert and the taper reground about 9months ago.

Thanks again

Derek.

[SCzEngrgGroup]

Derek,

For best stiffness, you want to keep the quill full up and locked. And use the shortest tool you can get away with. A long 1/2" endmill will flex quite a bit on a heavy cut.

Regards,
Ray L.

[DareBee]

A long 1/2" endmill will flex quite a bit on a heavy cut.

It will also flex quite a bit on a light cut.