[Geof]

A few people have posted queries about the capabilities of the TM machines.

We just installed a TM3P and the first job on it involves machining 32" lengths of 2" x 1/2" 5083 T0 flat bar to the profile shown in the first picture.

Four bars are clamped on a fixture and there are four roughing passes at 1/2" deep, full width engagement at 4500 rpm and 30 ipm, which works out at 7.5 cubic inches a minute with the spindle load hovering around 100%.

This seems to be the best the machine can do; increasing the speed causes a fall off in torque so the feed has to be reduced, decreasing the feed increases the chipload so the feed has to be reduced.

The cutter is a GAR high helix two flute and obviously flood coolant is used.

[Kool Parts]

Geof,
Been a long time since I heard of 5083. Cant even remember what its advantages are. Sounds like you like the machine so far.
Gary

[Geof]

Geof,
Been a long time since I heard of 5083. Cant even remember what its advantages are. Sounds like you like the machine so far.
Gary

5083 is easy to bend that is why we get it T0. The tapered ends each get a 90 degree bend about 5 inches from the center boss to form a U-shaped base for things mounted on the boss.

[fpworks]

Geof,
Do you suspect error with the load meter?

[Geof]

Geof,
Do you suspect error with the load meter?

No.

Why do you ask?

I experimented with a few different speeds and feeds to find the combination with the fastest feed that would not put the load much above 100%. That is what I mean when I say the load is hovering around 100%.

[fpworks]

100% indicated load at that cut seems way high, so I wonder if it is erroneous, especially since you experimented with finding the power band.

[Geof]

100% indicated load at that cut seems way high.....,

Have you used a MiniMill or any of the TM machines? They only have a tiny motor; Haas rates it at 7.5hp but that is a bit fake because that is the peak at 180% or 200% capacity and only useful for 10 minutes or so. Really it is a 3.75hp motor that can be overloaded significantly for a shortish time.

[fpworks]

No, I haven't run either, but I used to have a Fadal EMC, which I thought would be pretty close...also with a "claimed" 7.5 hp. It did have "5 hp" on the nameplate and it could do about 30 cubic inches/minute out of it at 100% load.

With my Mazaks, I get 100-110 cubic inches/minute on the 25 hp machine and ~150 cubic inches/minute with the 35 hp machine, right at 100% load.

Even with an actual 3.75 hp, I would still only expect ~50-60% load at that cut, unless 4500 rpm takes it way out of the motor's power band. In one of the other forums, somebody else said large errors in the load meter is not too uncommon. (from the factory)

(btw, did Haas supply you with a graph illustrating power/torque vs speed at duration?)

[Geof]

......Even with an actual 3.75 hp, I would still only expect ~50-60% load at that cut, unless 4500 rpm takes it way out of the motor's power band......
(btw, did Haas supply you with a graph illustrating power/torque vs speed at duration?)

No I do not have a torque curve for the machine; I have no idea whether Haas has them.

I am well away from the region of maximum torque; this is at 1300rpm. The problem is that trying to run at maximum torque means going slower overall because the ipm has to be reduced. I am running at just over .003" per tooth on a two flute, if I drop the speed I have to drop the feed because the tooth load goes up quicker than the torque, and if I increase the speed I have to drop the feed because the torque falls off badly.

I am not saying this is good bad or indifferent, and I am not comparing it with other machines. As I say in the first post my intent is to give some idea of what the machine can do because people have posted queries.

If I really needed to hog these things out quicker I would buy a VF3 with a 10,000rpm spindle, but I can almost get two TM3Ps for the same price and get better productivity for dollar spent.

[fpworks]

Geof,
I'm only comparing to other machines to validate my concern that your load meter may be erroneous. (or the spindle can only make 1.5-2 hp at 4500 rpm, but that doesn't seem right considering it can run at up to 6000 rpm)

Peak torque shouldn't be the concern, but moreso the rate at which torque falls as rpms climb. The torque falloff rate is unlikely to be constant, so you need the chart...also, under certain conditions, it may be possible to have your spindle motor run cooler if you apply the information in the chart. I understand that you're not using the machine for volume work, but I'm sure you wouldn't complain if you could double roughing capability. (or run the machine easier)

You probably already know this, but a better tool can run a lot heavier chip load. FWIW, you can run a 0.5" Data Flute ALDH at over 80 ipm at only 3500 rpm in a 1xD slot. Maybe the spindle makes significantly more power at 3500 rpm...or your spindle load meter is reading way high and you could go quite a bit faster without knowing it?

I'm just saying that it doesn't add up...one way or another, I think the machine has quite a bit more in it.

[Geof]

You are missing my point; I experimented with different speeds and feeds to see what conditions gave me the best material removal. Maybe I could go to a different cutter but for simplicity we stick with the GAR high helix series.

The machine is used for volume work and that is one reason I have this machine rather than a VF3 for long travel parts; I can have two machines running for the same dollars invested and get better productivity overall.

[fpworks]

No, I get it...but without a spindle power curve, you're still guessing. Spindle motors frequently have dramatic "steps" in their torque curve and you could be drastically influencing available power with a small speed increment. (spindle torque/power curves are often shown in a logarithmic scale so they don't look so bad)

Something is seriously wrong with the spindle power (of 3.75 hp) versus the indicated load at such a small cut...for volume work, you should be concerned. Perhaps it is something as simple as a load meter calibration...maybe not. Either way, I think it is worth looking into a bit deeper.

Best of luck.

[big_mak]

Geof,

I have a way fro you to increase your metal removal!!!!! you can send them to me!!

But hav eyou tried using a Roughing cutter to try and increase your metal removal rates????? A 3 Flute by Robb Jack may help you out!!! The roughers Garr Offers are only in 4 flute and tend to sing a bit. You know who carries them. PRicey, but may be worth a shot!! I know how you cut metal and it's generally a take no prisoners approach!

[Geof]

..But hav eyou tried using a Roughing cutter to try and increase your metal removal rates????? A 3 Flute by Robb Jack may help you out!!!....

Probably I should be systematic and try different cutters, but I am dubious about going to three flutes never mind four. With aluminum my experience has been that the high helix two flute gets the chips out better; the times I have tried more cutting edges I have had to drop the ipm to prevent chips jamming in the flutes.

[big_mak]

Remember that the roughers will create smaller chips of course so it's not quite the issue if you went for the three flutes.

We were running the Ø5/8 version in Mic 6 Tooling PLate @ 1/2" DOC and full width @ 12K RPM and well over 100IPM

[Matt@RFR]

With aluminum my experience has been that the high helix two flute gets the chips out better; the times I have tried more cutting edges I have had to drop the ipm to prevent chips jamming in the flutes.

I don't know if you care to look into it further, but I run 1/2x1.25" 3 flute endmills from lakeshore carbide in pockets .375" deep, 75% stepover, 12,000rpm and 216ipm. That's .006"ipt and I've done pockets with that setup over 1.125" deep with no problems at all with chips.

I wonder how much effect chip load has on how an endmill ejects chips. Sounds like you're limited to around .003ipt on your TM, and maybe that's why it doesn't like 3 flutes. Like I mentioned, I run double that chip load and have never had issues with chip recutting.

[Geof]

......We were running the Ø5/8 version in Mic 6 Tooling PLate @ 1/2" DOC and full width @ 12K RPM and well over 100IPM

Well if you scale things I don't think I am doing too bad.

You have about three times the hp, running at about three times the rpm with your feed going about three times as fast compared to my conditions. Your cutters a bit big I will admit.

And MIC 6 machines a lot different to 5083 T0, had you noticed what horrible stuff I am working with.

[Geof]

I don't know if you care to look into it further, but I run 1/2x1.25" 3 flute endmills from lakeshore carbide in pockets .375" deep, 75% stepover, 12,000rpm and 216ipm. That's .006"ipt and I've done pockets with that setup over 1.125" deep with no problems at all with chips.
....

Like I said to Big Mak, I don't think I am doing to bad; I am cutting a 1/2" wide and 1/2" deep, which is a bigger cross-section than you are cutting, with a machine that has only a fraction of the hp you are dealing with. My VF2s routinely handle cuts 5/8" wide and 0.4" deep at 11,000 rpm and 110ipm; a TM3 is not a VF2.

[Geof]

I decided, for once, that I would not be stubborn; so I did pick up a three flute rougher. Yes the machine can drive it faster, 5000rpm and 42ipm at about 110% load. However, the machine can also snap it clean off when the flutes load up with chips.

So I have gone back to my way where I, and my guys, can confidently walk away from the machine during a cycle, and load another machine.

[big_mak]

did you use corn cob type rougher? Or just a garr blah 3 flute?

The roughers make smaller chips, so the plugging isn't as bad a risk!!!!!