REAL MACHINE FEEDS AND SPEEDS

[KMI]

Hi,

I'm trying to compare a haas vf3d and a fadal 4020. I have been told by each of the sales staff what they think the machines can do. I thought I would put it out to the people that really know. The test is with a 4.0 inch face mill with seven round .375 rad inserts. What we are looking for is the realistic feed and speed based on a .100 ramp cut . I look forward to hearing what you think is possible.

[Keith Graydon]

What material are we cutting in this test?

[Trevor Bailey]

What make of tool is it? Insert grade? Wet or dry?

[KMI]

sorry about that. The material is 6061 t6. The cutter is a sandvick facemill RA200 -083R38-19M. The insert is RCHT 19 06 00-KL. We are trying to find out what a good production feed and speed rate would be. The ramping operation is going down .100 per revolution over a 11 inch diameter.

thanks for the quick reply.

[bryan.davis]

I use sandvik cutters a lot and generally speaking I find that the book feeds and speeds to be a very good guide to what is achieveable.

At the end of the day youve not quoted those factors that I feel will really limit your cut.

The real limiting factors for a cut with a 4" cutter are going to be the power of the machines spindle, and the ridgidity of your setup, remember, if you are going to take a 30Kw cut, then you had better have the workpiece clamped down to the bed such that it can withstand that sort of power, the same goes for every other element in the setup.

Once youve got the workpiece and toolholder at maximum ridgidity, youve got to look at the next weak links in the chain, which are all down to the machines manufacture, I know there are machines out there with 35Kw spindle motors, but quite frankly their chasis are not capable of handling that sort of power, much in the same way that a golf buggy cant handle a Jaguar V12 engine...

The best thing to do is to experiment, start with a maximum ridgidity setup and then take trial cuts, gradually increase the power requirement of the cut by increasing the width of cut and depth of cut, until you reach a point where you feel the machine is at its limit, then use these figures to calculate the power consumed by this cut (formulae are in Sandvik handbook). Once you have the consumed power figure remember it. You can then use this consumed power figure to calculate the maximum possible cut you can take on this machine using most any cutter IN IDEAL CIRCUMSTANCES!!!

DONT forget that whilst your machine may be able to take 35Kw of cut not all cutters workpieces, or setups can, as I said earlier, Sandvik figures are generally good in IDEAL circumstances, but you must always take into account all those factors that make this particular cut less than ideal.

[KMI]

Thanks for the info.I have the sandvick catalog and will recheck what they say. The real problem seems to be that the reps say the machine can face at a certain speed and we have been trying to get close to those numbers and cannot. The machine will alarm with a spindle overheat. I wanted to know if it is the machine, ie: are others facing that cut at say 60 - 80 ipm and we can only get 32 ipm. We have had alot of problems with a new vf3d and I'm trying to get realistic numbers on what other machine shops with the same or similar machines are able to do. We do use a very ridgid setup. We are currently running at 30 ipm at 2800 rpm ( recommended by haas)and ramping at .100 depth. This is loading the spindle meter to 100 %. If we do part after part the load will steadily go up and finally alarm with a spindle overheat. Are we running to hard or is this machine not facing up to what would be expected?

Thanks for the info.

[Rick Lawler]

KMI,

There is an other thing to look at which may be more important than the maximum horsepower of the spindle.Your machine tool rep should be able to provide you with a chart showing the power output vs RPM. Many machines with 8-10,000 rpm spindles don't make enough power at the lower rpms to take the heavy cuts. Look at these charts and compare them with the horsepower requirements of your cuts

[bryan.davis]

A spindle overheat could point to a number of factors....

It could point to a lack of power in the spindle drive chain, but I would expect for you to notice stalling and stuttering if that were the case.

Generally speaking the 100% load rating on most machines in my experience is a continuous load rating, with it being possible to run the machine at up to 150% for short periods of time

It more than likely points to poor spindle cooling, check you spindle cooling unit (if you have one, and if not get one), some units allow you to set a cooling value, normally set about 2 degrees below ambiant, but I often set it much lower if I feel that the temperature is likely to rise.

Ive got to confess that I dont know what the material spec is, Im not familiar with the exact cutter you are using, and you dont quote the insert grade, but from what I can tell is that you are running at a surface speed of 880 (sorry Im a metric guy) which may be a little high, but if its correct then I would expect a feedrate of somewhere between 875mm/m (34ipm) and 1750mm/min (68ipm) with a 7 insert cutter.

[Will Slota]

I used to have a haas and would routinely use a 3" face mill in 6061. From your description and past experience I feel that you are indeed at the limits of your machine capabilities. Two factors to consider are your horsepower and of the spindle is belt driven or is it the geared high torque head.

We had the belt driven model with only 8 Hp.

I usually ran my 4 flute 3" face mill at .08 depth of cut 28 ipm and 3600 rpm, which at a .002 chipload gave a beautiful finish.

[mcrae_andrew]

The issue here is not limited horsepower but Torque. Horsepower is torque multiplied by RPM. In order to reduce the amount of torque and allowing us to get a higher spindle speed for a given SFM, go with a smaller diameter cutter and then increase the DOC to maintain the same MRR. with a button cutter, don't forget Axial and Radial chip thinning when calculating table feeds.

[gmenzies]

we have a fadal 3016 box way machine with a 27 inch clearance on z. 10,000 rpm

we use sandvick 390 type cutters (helical inserts) . i cut 80 to 100 imp with a two flute (h-13 grade) 10,000 in 70/75 no problem

generally i program at 2,500 sfm with alliminum . .100 to .150 depth of cuts

the 2 inch (5 inserts) 5000 rpm, 100 imp.

the cutter sounds like a chainsaw , it just rips it out.

1025 grades in a 390 --450 to 800 surface feet depending on brinel hardness.

the fadal /hass level of machine are pretty much the same.

also your code is important. you can't do a 100 imp on a .25 rad . accel and decell have to be there. these machines , depending on size . cannot handle the g-forces requred to go realy fast.

as far as spindle over heat and the cat 40 not releasing the tools for a tool change.

I sure hass has a solution for that. our fadal has a chilled spindal. but the tools sometimes still stick. espesially on long

cutter tool paths

cutter geometry is the key. with good code.