[Scott_bob]

Assuming that work holding is not a factor, (material is clamped down well)...

What is the most significant 'limiting' factor in High Performance Machining, or HSM (High Speed Machining) on any CNC machine?

Or, Choose from the above list, what affects high performance machining the most...

You can only choose one, so we going to identify 1st place...

[hardmill]

Balanced tools, Rpm, and ability to take in code to the control fast enough. Lets not forget the
cutting tool itself. Very important!!. All these will weigh into the harmonics the Caminc was speaking
of and you need to decide which is of more importance. Get the jobs off the machine a little quicker
or possibly sacrifice some fretting of the tool holder and surface finish.


PEACE

[Gunner]

I believe in a production environment it is matching the work to the machine and its capabilities. From your list above it's a tough decision since they all work hand in hand. You can have the proper tools but if you don't have the spindle speed or control they won't work properly and vice-versa.

[Scott_bob]

Gunner,

Would you say the "machine" is the control? Not entirely, of course...

For instance, if i replaced the old control on a CNC say a Fadal, with say a Fanuc control, or a PC based control, would we still refer to that old original CNC as a Fadal?

I wouldn't... And, depending on the control I choose, the CNC would be sooo much faster, accurate, reliable...

[cadman]

Can't vote in this poll. HSM (as developed by the major aerospace firms) is the sum of all the processes listed in the poll, plus another important part that people overlook: machine dynamics. Removing one or more of these processes is kind of like letting the air out of your tires, it will still roll but not very well.

[Scott_bob]

It is true, that to suggest that "one of" the above Poll options would suddenly solve the problems that prevent high performance machining. This would be another one of the many myths that are common today.

IMO, one technology cannot promise (and deliver) all the solutions...

But, on the other hand, I wonder if those professionals who vote in this Poll will end up identifying the option "Most" responsible for the lack of performance...

If I may, ask yourself the question:
Rank the options, then vote on the one that is at the top of your list...
This exersize is somewhat relative because, to some of us with crappy CNC controls for instance, our option may be more obvious than the option to a guy with a good control...

[Gunner]

Scott_Bob,
I guess I'm going to take the machine control. A good control will be equiped and allow you to have the ability for HSM. I'd rather have that first. I can always upgrade the spindle and tooling. This is taking into consideration that the machine isn't 25 years old and worn.

[JIMMY]

I would have to say the tool is the mosyt important factor because without the right tool the other factors might not come into play.

[Scott_bob]

Jimmy,

If I put the finest cutting tool available in the best possible holder, run this fantastic tool on a poor quality cnc machine that has a crappy control, do you think I can get high performance out of this set up?

[camminc]

The most problematic limiting factor of High Performance Machining is Chatter. Otherwise, it would be forced vibration due to improper programming, unbalance, etc. Just so you know, unbalance is a forced vibration condition and has nothing to do with chatter. The frequency of unbalance and chatter occur at different frequencies, which can be determined. If you see MoldMaking Technology Magazine in June you can read about this

Controllers, cpu, motions of a machine tool are excellent to have, but they do not control the cutter at the tool tip during the cut. Dynamics at the tool tip of the cutter are the determining factor of the machining operation, period. Hardmill is very much correct about machine tools and their capabilities as far as controllers, cpu, etc, yet it all comes down to the tool tip after that. The machine is the platform, the cutter assembly is the end result of that platform. It all has to do with dynamics, the entire machine tool.

[Gunner]

We run CNC Lathes here in a high production environment. We don't usually run into chatter problems unless we are dealing in long parts using a small diameter stock or deep bores that have a boring bar out past its recommended effective length ratio. This part mix is minimal for us. I think the dynamics plays a bigger role when you have a stationary part and rotating tooling (such as milling) vs stationary tooling and a rotating part (like a lathe).

[Scott_bob]

Let me ask the Fanuc users out there these questions:

Can you get high performance machining or HSM without using your Fanuc high speed codes?
How much faster can you go when you activate these codes?

Ref.
On our Fadal control, by using these special codes, you get 2 to 3 times the feed rates...
G8 (FEED RAMPING OFF) *THIS IS THE LEAST ACCURATE,
BUT FASTEST ESPECIALLY WHEN GOING THRU A LOT OF POINTS

G9 (FEED RAMPING ON) *THIS IS THE MOST ACCURATE, CNC SLOWS
AFTER EVERY BLOCK, THEN RAMPS BACK TO PROGRAMMED FEEDS
G51 R0+0.5
G51 R0-0.5 (FADALS FEED RAMPING TIME CONTROL, .5 TO 2. RANGE
1. BEING DEFAULT, .5 WOULD BE 1/2 TIME, 2. WOULD BE DOUBLE)
---------------------------------------------------------------
FROM HERE DOWN, A LOT OF DETAIL MUST BE INCLUDED,
RECOMMENDED FOR ADVANCED USE ONLY, MUST UNDERSTAND THE MANUAL...
---------------------------------------------------------------

M94 (ONLY FOR HIGH SPEED LINEAR CONTOURING 'POINT TO POINT')
M95 (CANCELS M94)

M94.1 (LINEAR ONLY, 'POINT TO POINT' FEED FORWARD BY FEED MODIFICATION)
EXAMPLE:
M94.1 P179 Q33. R0+90. R1+0.1 R2+20
M95.1 (FEED FORWARD CANCEL)

It is interesting that not 1 person so far has voted on these High Speed G Codes...

[camminc]

To Gunner: That is a good point about turning. Your are very correct in saying "I think dynamics plays a bigger role when you have a stationary part and rotating tooling (such as milling) vs stationary tooling and a rotating part (like a lathe).

I have not talked that much about turning. I have to say, I am not an expert in turning, I can only recommend this from what I have seen, used and shown.

From my experience natural frequency of the cutter / holder / called Stackup assembly is the same with milling as with turning. You can measure the frequency of a lathe tool and flexibility of it the same as with a milling cutter to determine proper RPM and depth of cut. Yet you can also determine dampening characteristics for turning. In most cases it is not required but with longer cutter parameters special devices can be incorporated into a lathe tool body to further enhance length of cut, so called stick out, such as a set of springs with a carbide plug or heavy metal, to dampen any cutting vibration frequency. Spring pressure, length and weight of carbide mass can be measured with the proper equipment to maximize. Just turn a screw to maximize once a reading is taken. Increase spring pressure or decrease. It is a simple thing to do as with performing an impact test of a milling machine Stackup, not complicated as every one thinks.

By doing so, you can further maximize a turning tool, giving much higher lengths of cut. In milling, one cannot work with dampening characteristics as much because the assembly is in rotation. Dampening of a such method in milling cutter would cause massive unbalance due to rotation force as spindle speed increases of that assembly creating problems, creating forced vibration. As in turning the cutter does not rotate giving it an advantage as not to rotate - thus enabling it to dampen into the structure / holding device, etc. This is Dynamics.

[avsfan733]

Where would coolant fit into the equation....flood through spindle. granted they aren't specific to HSM but still somethign that should be brought into the equation as it is a definite facilitator

[cadcam]

avsfan733, to a point it helps but one of the thoughts of HSM is to remove the chip fast and take the heat with the chip.

So some time this may be done dry with some inserted tooling.

[Gunner]

Camminc,

I've never heard of using springs as a dampening method. Is there a link or documentation describing a recommended procedure or setup diagram? We are always looking for a better, faster way. Thanks.

Avsfan 733,

Coolant or the ability to keep the cutting edge cool is definetly a factor as is all the other components we've discussed from above. It doesn't make any sense to "crank" speeds and feeds to get one part out quickly and then incur downtime to change all your tooling. I think the ideal situation would be to reduce the part cycle time and extend tool life. After all, in the high production environment we're all after more good completed parts at the end of the day, hopefully not causing undue stress or problems for the machine operator . We've discussed some of the pro and cons of high pressure coolant systems in other posts. I believe it was in the high speed machining thread.

[Scott_bob]

The HSM CNC control retrofit is installed and is running!
The results I'm sure, will be worth the the time it took. If there is one thing that I've learned through this process it's this.

If a project is worth doing, make sure it's done right or don't start it at all.

It's early still, but by replacing the CNC control we are seeing feed rates 3x faster with better quality parts. Profile tolerances of +/-.001 at programmed feed rates of over F150. At 1st we were trying to see just how fast could we go, but surface finish tolerances force us to slow down. Also, we have to use 3 fluted end mills in aluminum as having 50% more flutes per revolution we get better finishes. Sloting is almost as good as a 2 flute end mill and with the increased coolant pressure and volume we get good chip removal...

At programmed feed rates of F300. the control is not moving this fast all the time of course, when small radii are coming up or a sharp corner the feed rate is reduced as needed, automatically. This is extremely helpful in optomizing a program as the feeds are compensated based on the geometry detected by the look ahead and by the limitations of the acc and dec of the servos.
You've gotta see this thing to believe it.

In summary:

We have a 1996 Fadal 4020 VMC with a 2 pallet changer, box way model, with DC drive servos, and 15,000 spindle, 30 tool changer. Easy to use PC based, extremely high speed control (None faster). Huge file size capable, incredibly smooth motion control able to dynamically control motion up to this machines rapid traverse rate of 700 inches per minute.

Investment?

Less than some shrink fit systems and holders...

[Gunner]

Scott_Bob,
Just wondering how the control retrofit is going now that you've had a few weeks play?

[Scott_bob]

Awsome...

I can't even tell you how much better the CNC performs cause I start to sound like a fanatic.
Just as an example:

4-19-04 We are cutting oval .250 wide slots by .375 long and .37 deep.
Using a .187 3 flute carbide stub end mill, 3 passes .13 each...
(we do drill the start point with a .23 diameter drill)
At 14,000 Rpm this tool has just one feed rate of F70. that's 70 inches per minute!

The slot measures .250 wide x .375 long +/-.0005
The Control is not always trying to do tiny radius motion at F70. it slows the feed depending on the geometry ahead (thru 5 axis motion look ahead), we only do 3 axis...

Far better accuracy, basically we don't have accuracy problems on the machine any more...

Today 4-20-04 We are circular interpolating a 1.375 Dia bore to within +/-.001 feeding at F110. The bore is round within .001
We used to have to ream this bore and it was a hastle with that big a reamer... The 3 flute 3/8 carbide end mill using G03 programmed at F162. also made an excellent round bore, but needed a better finish so we slowed to F110. (should have used a 4 flute).

Last night, 4-23-04 We were roughing 1/8" thick 6061-T6 Aluminum sheet at F366. (That's three HUNDRED sixty six) inches per minute with a 1" diameter 2 fluted Sandvick Insert end mill, then finished a highly contoured profile with a 3/8" 3 fluted carbide end mill F216. (two HUNDRED sixteen) inches per minute. Profile tolerance? Within +/-.003, inside radii vary from R.188 R.500 R1.250 up to R4.750 an interesting pattern...
By the time I got in to work in the morning, all 60 parts were done, and the next job was being set up...

[JIMMY]

I agree with you camminc, I didn't think about it like that. Thank You. I am so used to using top performance machines that I worry about the cutters most of the time. Thank you for the info.