[jmlarson]

Hello all:

Please excuse my ignorance - I am still a newbie - but I am having trouble balancing speed, feed, and depth of cut for my tabletop machines. Essentially, I know the machines are under-powered to make the cut I want to make, but I am wondering if there is a formula I can put into an excel spreadsheet that helps me balance these three items.

I have not been able to find one as of yet, and I have done some searching. Ideally, I would like to build a (hopefully) simple model that helps me set the parameters to maxamize the abilities of my machines, but not over-tax them, while at the same time avoid chatter marks, not burn up my tooling, etc, etc. (yeah, yeah, and world peace while I am at it). Finding out what I am *suppose* to do has been relatvely easy - finding out how to compensate when I *can't* get there has been a bit more challenging.

Some simple limitations that I am running into are things like spindle speed and machine power.

Any thoughts, suggestions, guidance or discussion would be appreciated.

[Geof]

I don't have an excel sheet formula; wouldn't know how to do one. But here is one approach.

You are power limited and also probably lacking rigidity. Don't worry about trying to go as fast as you 'should' be going based on your material and cutter size. This, more or less automatically, reduces the chance of burning a tool, it allows for, maybe, a deeper cut and a faster feed, both of which are conducive toward controlling chatter.

It is difficult to suggest how much slower but if you have a step pulley belt drive stay in the mid range, always taking into account of course that for some materials you may need to go slower, I have aluminum in mind in these comments. The reason for staying in the middle is you have more pulley area in contact with the belt so you can transmit more torque, sometimes your lack of power is not only lack in the motor b ut lack of driving ability.

And don't get too hung up on trying to find formulae to tell you what to do. Experiment, be systematic and take notes; eventually you will see patterns emerge.

[little bubba]

I have a lot of experience with crappy machines, I own crappy low horse floppy machines and try to make money off of them. I've worked in places with less than ideal machines, so hopefully my advice will help. I'm not sure if the OP is talking lathes or mills, but I'm going to assume mills.

I'm giving most of this advice based on steel (mild 1018-1020, to annealed 4140-4130) though it will apply to aluminum and other harder stuff.

First off, you say you are having a problem with speed and feed, those are very easy, depth of cut and width of cut are more tricky, explained below. Spindle speed, do a search for SFM (surface feet per minute) going by the seat of your pants or "seeing" it is just stupid, this is one of the areas in machining that can't be "artisticly" dealt with, you are just going to chew up endmills or be less productive than you could be. One point about surface speed, you can increase it drastically by decreasing your width of cut and increasing your depth of cut, same with feed(chip thinning, look it up). Bonuses are you are using more of the endmill that you paid for and your tool life will increase dramatically, a very good way to make the most of a floppy machine, and a way to get HUGE metal removal rates on a good machine.

Second, feed rate, do a search for chipload, chip per tooth of something like that, Inches per minute do not mean anything, its how much are you moving per tooth(the big IPM #s are fun to brag about, but they don't mean anything). Then there is chip thinning, already mentioned which allows you to increase your feed. There are tons of charts on manufacturers websites for feed, most of it is hype, knock them back by a third. Here is a quick formula, play with it, and adjust for your machine and your personal techniques, for steel, with a 4 fluter, take 2% of the diameter of the endmill as a very low advancement per tooth, at 50% stepover, 5% is about the point where you are beginning to get aggressive.

Third, don't buy crap tools, there are lots of myths running around that you need the biggest best and fastest machines to run carbide, BS!! Carbide needs to be run fast, it doesn't HAVE to be, it just CAN(run a high quality carbide on a manual mill, treat it, speed and feed wise as HSS and you will never have to buy another endmill, ever). Carbide isn't sharp BS!!! I have the scars to prove it, this comes from inserts that are intentionally dulled to give long tool life, you can get very sharp inserts, they cost more since they are ground, not just molded, these can be just as effective as HSS. You need tons and tons of coolant to run carbide, while this is more true on a lathe, milling, carbide does fantastic dry(steels), better than wet(unless you have the coolant exactly where you need it at the pressure you need it, does not happen often). Carbide does not like the rapid heating/cooling cycles. It has no problem with heat, so let it have it.

Buy quality tools, even for a crappy machine, lakeshore carbide is a great place for dirt cheap high quality endmills, I won't say they are the best for all applications, but they are pretty damn good. Look at the variflutes, they will break up your harmonics and make the absolute most of your floppy machines.

If you are still with me, now on to width and depth of cut.

What I've been using lately is metal removal rates.

Step 1) what HP is your spindle? If you have pulleys, great, its always the same, variable speed drive like on a bridgeport, same thing. Infinitely variable(VFD), you will need to learn where your peak is and your low points and adjust from there.

Step 2) general rule, one cubic inch of steel per HP(low carbon). I'm not sure about aluminum, but with a floppy machine you probably aren't going to go more than 2-3X that of mild steel (I don't play with aluminum all that often). Simple formula to find how much you are taking out, depth X width X feed in Inches Per Minute = your removal rate.

Step 3) run some experiments. You have a HP # so you have a theoretical max of how much metal you should be able to move. Start easy on the removal rate(15%?), use your calculated SFM, start conservative on chipload. Grab a piece of crap steel and start cutting, just straight line stuff, turn it all into chips. You now know about SFM(surface feet), you know about chipload, hopefully you've looked up chip thinning and how that can effect your SFM and chipload.

Run profiling passes where you only have engagement on one side(different depths and widths). The real problems you are going to run into with a floppy machine is in slotting, they can do OK when loaded in one direction, but bounce around horribly on a full slot, experiment with ramping while slotting, sometimes you can load up the machine enough to pull a good cut.

One more thing, if you have chatter problems, push it harder if you can(HP limited). A lot of chatter problems can be attributed to the machine/spindle/tool whatever not being pushed/twisted/forced in one direction enough, allowing it to bounce around.

[BobWarfield]

I'll add a little to what these guys said.

Chatter is a resonance effect. Often, changing either the feedrate or spindle speed can minimize it. A VFD let's you twist the knob when you hit chatter and maybe get away from it. I always try feeding harder, then increase spindle, then decrease spindle, then feed softer in that order.

I think Little B's width of cut is very important as is the advice to use quality cutters. The latter are cheap on eBay if you shop carefully.

Use positive rake tooling, it reduces your cutting force.

Lastly, you can play with a lot of these parameters in a piece of software like ME Consultant Pro. What's cool about ME Pro is you pick your operation, cutter, depth of cut, and width of cut, and it will recommend your spindle speed and feedrate. But you can vary those parameters and it will rebalance. It will also tell you the horsepower required. The latter has two important purposes. First, you'll make sure you don't bury the cutter too aggressively and stall your spindle. Second, and more importantly, the HP is a measure of the cutting force. The more cutting force, the more force is trying to overcome your machine's rigidity. You can play with parameters and see how to keep those forces in limits your machine can handle.

Best,

BW

[jmlarson]

I'll continue on with this information.......
I appreciate it.
Regards
James

[cncprofessor]

Essentially, I know the machines are under-powered to make the cut I want to make, but I am wondering if there is a formula I can put into an excel spreadsheet that helps me balance these three items.

Some simple limitations that I am running into are things like spindle speed and machine power.

In the absence of the suggested ME Consultant Pro software (worth every penny), for whatever it’s worth, try the following formulas for the milling operation.
Hope it helps!

(1) N = 4(V)/D (2) Rmr = v x 12 (fr)(d)
(3) fr = (N)(nt)(tl) (4) HPc = hp/(in³min)( Rmr)
(5) HPm = HPc /E

Where:

N = revolution per minute
Rmr = material removal rate
HPc = horsepower at the cutter
HPm = horsepower at the motor
nt = number of teeth in a cutter
V = material cutting speed (sfpm)*
D = diameter (affected by the cutting force)
hp/(in³min) = required horsepower per cubic inch/minute
fr = feed rate (in/min)
d = depth of cut
4 = constant
tl = tooth/chip load*
E = machine tool efficiency rate (%)*
-------------
* Ref. Machinery Handbook (Tables)

http://www.cncci.com/pdf/MEPro%20brochure.PDF

[Eclipze]

I've just tried milling aluminum. Not sure what grade it is, just material from the local hardware store.

I've got a Wigit Midi-Router with a Proxxon Spindle (100W) and milling with a very new 3mm (1/8") 2-flute carbide end mill.

I first tried a cut of 1.6mm (0.06"), which was the thickness of the material, 20,000rpm spindle speed and ~30mm/min (~1.2 inches/min). The cutting noise was excruciating!!!

It was really loud!!! Having watched a machinist carve steel like it was damp clay, with nothing more than a slight chugging noise as the material is carved away, I immediately realised I was way off. The finish of the edge was really bad. It was far from smooth and in fact altered the dimensions. Hence I became aware of the whole world of chip thickness etc...

I downloaded ME Consultant 2.0 (which is free) and run a calculation for a 1mm DOC (0.04"). It recommended a feed rate of 600mm/min (24"/min) at my maximum spindle speed, 20,000rpm. I generated a profile which ramped the tool down to the depth and gave it a try. It happened very quickly, however it ramped down to depth and cut and got a further 3mm (1/8") along before it stalled and snapped the bit.

Now I checked the ME Consultants calculations and it advised the power needed was 23W. The Proxxon is 100W, so I thought there was plenty of margin. Obviously I was quite wrong.

My confusion is now about getting the tool to move at an appropriate speed, but also knowing the limitations of the spindle - without breaking tool bits. If I reduce the feedrate, the tool make make a lot of noise and not cut efficiently (rub). I can reduce the depth of cut, however given the tool stalled at estimated 23W load, how do I determine a better approximation?

Also of importance... what are the effects of too fast vs too slow. What do I look for to refine the feedrate and depth of cut to be closer to optimal?

Any advise would be appreciate... I've attached the ME consultant calculations...

[Eclipze]

I just tried reducing the feedrate to 400mm/min (15.7"/min) with a depth of cut at 0.25mm (0.01") and it seemed to cut quite cleanly! I did use some cutting lubricant as well, just a light spray on the cutting tracks. I didn't notice the spindle slowing down, though this time I had ear muffs on. Edge finish was sooo much better than the original 30mm/min feedrate.

I'm keen to know what depth I can cut at. I would hate to cut at half the depth of what I actually can... and go through tool bits twice as much from only using a small percentage of the cutting edge.


I think the best approach might be to hook up a spindle speed monitor so I can accurate see if it starts slowing down. Then I'II have a better measuring stick to know when I'm getting close to the spindles capability and back off before I risk the impending cascade slow down, stall and snap scenario.