Spindle Power Curves

[TMTCamCentre]

Keen to take a high approach shell mill for a run, don't know if I can run it to its full capability. Wondering if anyone has a 'Spindle power curve' to see if my VF-OE or VF-3 will handle it both have 20HP dual vector drive spindles.

[automizer]

I have been after a Spindle power curve for my GR-408. I think this is something Haas should have on there web site it would make programing a lot simpler knowing where you machine is most powerful

[Geof]

If you look at the machine specs on the Haas website you will find the rpm for maximum torque; for instance a MiniMill is 33 lb-ft at around 1200 rpm.

Below this rpm the torque stays fairly constant all the way down to zero; above this it falls off. The decline is gradual up to about 2000 rpm where it is around 25 lb-ft then it is almost linear down to around 5 lb-ft at 6000 rpm.

The curves for other machines with faster spindles and larger motors will have a similar profile, and if the machine has a gearbox the low speed torque will be bumped up but still fall off at the upper end of the range.

But even if you have this information how does it help? Do you know what torque is required to run a shell mill under certain conditions of depth of cut and feed per tooth on a particular alloy?

I suppose it is possible to find this information, but I simply set the rpm for the maximum sfm that should be used and start with a modest DOC and feed. Then I play with the speed and feed overrides and watch the spindle load; many times if the rpm based on the sfm is well above the maximum torque it is possible to slow the speed, moving to a higher torque, and increase the feed to get faster material removal. There is a limit when doing this because the feed per tooth is increasing so the torque needed to drive the cutter also increases so the spindle load will go down at first then start to increase again.

With a shellmill though, most likely the rpm needed for the correct sfm is going to be below the maximum torque region for the machine. Therefore it is not possible to go faster and going slower will give less torque. In this case just start with a low feed and bump it up while watching the spindle load.

[TMTCamCentre]

Haas just don't seem to like letting go of this sort of information do they.

I've just aquired a Taegu-Tec 50mm diameter (2") 10 degree approach cutter. These run at anywhere up to 2mm per Tooth (so they tell me) in carbon steel and cast iron. All the cutting power requirements of the tool are supplied by the manufacturer. I suppose the thing i'm most worried about is that if I go edging cutting data up (within suggested range) and she goes bang, because of the approach and the fact that the cutting forces are being applied directly into the spindle taper - What else is going to be damaged.

[Geof]

The numbers I gave were based on the torque for a TM machine, but what I was getting at is that you do not need the curve if you know the rpm for maximum torque because then you have a good approximation of the torque below that rpm. What are you planning on machining with that cutter? For (ductile or malleable) cast iron I would run it at maybe 300sfm which is about 600rpm, the machine torque is irrelevant for this decision. The depth of cut and feed per tooth do depend on the torque available and you can find the maximum available for your machine at any speed lower than about 1200rpm. You have the utting power requirements for the tool so just select a depth of cut and feed per tooth combination that needs a torque around 75% of what you have available and start from there.

This approach will work with ductile cast and with plain carbon steels where you do not have a hard skin to break through or do not have the possibility of work hardening the material.

Have a look at post #4 in this thread. I determined what were good conditions for using a somewhat smaller facemill on a SuperMiniMill to machine hot rolled steel. You should be able to use a similar sfm with a deeper cut and/or a faster feed. You should at least be able to use my conditions as a start without any fear of anything going bang.

http://www.cnczone.com/forums/showthread.php?t=40082

[big_mak]

TMT,

I've yused the iscar feed mills on my VF-3 on 316 stainless and had not problems that were machine related. You don't need to start your feed rate @ 2mmchip per tooth start @ 1mm and work up and see where it starts to sound nice, and the load is reasonable.

Remember that the machining info most people give you in the propaganda for maximum values are for a machine like a monster OKuma or a Makino with a 50 taper to boot. Start conservative with your feedrates, and stay in line with your surface speed and you should be alright.

It's all about seeing what your exact machine system is capable of. This includes your Machine, Arbour, Cutter, Tips, Material being cut, and work holding. Perhaps Geof can add something I've missed, but all these things in cooperation will affect how a tool will run. Oh and don't forget the Bastard "Murphy" he always likes to throw a wrench in the works!!!!

[Geof]

Originally Posted by big_mak ....Oh and don't forget the Bastard "Murphy" he always likes to throw a wrench in the works!!!!

You mean like the time I had a shell mill stall the spindle, but the feed kept going? There is a 200 millisecond timeout for the controller to detect that the
spindle is not turning at the programmed rpm and give a spindle following error alarm. At 10ipm that is about 30 thou and the spindle does not like get pushed 30 thou sideways so of course it stalled the X axis servo. And destroyed the shell mill.

Unfortunately I have learnt most of the lessons the hard way (expensive way sometimes as well).

[omy005]

Is this what you are after? I have some others if its not the right one.

Andrew.

[TMTCamCentre]

Thanks omy005 for the curve, wouldn't happen to have one for a 10,000 spindle would you?

[omy005]

Here you go.

Andrew.

[TMTCamCentre]

Searched high and low for one of these, Thank you very much for your trouble.