# Basics on Depth of Cuts

• posted

Hi everyone, I am currently a student and my teacher hasn't been able to give me a real direct answer and everyone I ask just gives me what DOC they use but I want to find out how to get the DOC.

Basically I was taking to deep of cuts and keeping the feed rate high which I realized was wrong. So I am basically trying to find a formula or a log or something that will help me determine a DOC.

For example I am cutting 6061-T6 Aluminum at using a 1/4 4 Flute endmill with a FPM of 75 and a DOC of 0.025" and a Spindle Speed of

6000 since that is when the machine max's out. I understand where the RPM, IPM, and FPM comes from and how to calculate them. I just have no idea where the DOC comes from. So if anyone could explain it or give me a formula it will greatly be appreciated.
• posted

You can adjust DOC, RPM, and IPM to any value that produces a removal rate BELOW the rating of your spindle motor, and BELOW the FPM for the material (Milling aluminum, about 300 FPM) with the cutter size you are using.

In general, an end mill shouldn't have a DOC more than it's fluted length, and half the diameter, unless you absolutely have to plow a slot. If you're plowing, the lengthwise DOC will determine the accuracy of the finished work. Say 0.010 inch infeed steps for a typical key way: that means many passes but gives a good fit so the key won't bend under loads.

Material removal rate is CIM, cubic inches per minute, and it takes about one HP to remove one CIM in steel. You might get 2 CIM in aluminum, but just because the FPM is 3 times higher than in steel, it does NOT mean the CIM will be the same amount higher.

CIM divided by HP => Machinability, and the most machinable practical metals are magnesium alloys, which can produce flammable chips easily. Save the chips for Independence Day. The only thing that will put out an Mg fire is smothering it with dry sand or adding a lot of carbon to it to soak up available oxygen. Sorry, that's not right. What''s the Class D extinguisher? It's black, but it's not carbon. Is it graphite? Or coke?

So your spindle has an RPM limit built in. Below that, your cutter diameter and material gives you a FPM limit. The motor HP limit gives you a CIM limit, and DOC and IPM feed (Dimensions of cut, not Depth of Cut, that is, an area, not a linear measurement) multiply together to calculate actual CIM. Once selected, FPM, DOC, and IPM imply tolerance. Easing off on any or all three gives you a better tolerance. Pushing them to the max, if you stay in tolerance, gives plenty of good parts at the best production rate. But each reject costs you one machine cycle.

If you easy off FPM on a lathe, though, you can get stringy chips, which slow production.

Got it?

I think this is one of the most concise posts I have written here. That's rare for me. I have never set it down even for myself as well as this.

Yours,

Doug Goncz Replikon Research (via aol.com)

Nuclear weapons are just Pu's way of ensuring that plenty of Pu will be available for The Next Big Experiment, outlined in a post to sci.physics.research at Google Groups under "supercritical"

• posted

Is that HP/sec., HP/min or what?

Tim

-- In the immortal words of Ned Flanders: "No foot longs!" Website @

• posted

Your teacher can't give you a real direct answer because there is no such thing. Your depth of cut depends on too many variables:

the tool - how rigid is it - stickout length, held in collet or end mill holder, number of flutes, style (standard, hog mill, high helix, etc)

the workpiece - rigid or flimsy, held securely or not

the machine - rigidity, horsepower

the material - for example, you don't want to take deep roughing cuts in aluminum with a four flute end mill - will often chatter like crazy

- need more chip clearance

coolant - harder to get coolant to the tool with deep cuts - chips get in the way - aluminum can weld to the tool at high speed without coolant - uncooled steel cutting can fry the tool

Other folks can fill in more blanks.

What is 75 FPM ?

• posted

Tim, Power is the rate at which work is done. Work done at the rate of one HP will lift 33,000 pounds in one minute, 550 pounds in one second, etc., and remove about one cubic inch of steel in one minute. Expressions of power are not tied to other time references.

Bob Swinney

Do you have any back issues of Live Steam? There was a pretty good article on HP in the Jan/Feb edition of this year.

• posted

The key here is to look at the original units of "CIM."

Cubic inch per minute.

It takes so many joules to remove a cubic inch.

If you divide by time you get a time-rate of metal removal, and that then is connected with a time-rate of energy expenditure.

Joules per second, or watts. Similar to horsepower, up to a constant.

Jim

================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ==================================================

• posted

If by FPM you mean surface feet per minute, at 6000 rpm you are near 400 FPM. Plenty of technical stuff in the other replies, so I would like to know WTF are you using a 4 flute endmill in that material for? Get a 3 flute or high helix 2 flute and feed that puppy. And unless you are at final depth, take a deeper cut. As far as calculating depth of cut, pretty much, you don't. When looking at manufacturors speed & feed recommendations, you will find some nice numbers to use. Then you will notice the "fine Print", where they cop out by saying these are for starting purposes only, rigidity of machine & setup, greater or lesser depth of cut, radially or axially, will require variation to the...blah, blah.....Some manufacturors charts are more detailed and get you closer to more optimum cutting conditions than others. Some seem to be purposely vague. Kind of a disclaimer, if you will.

michael

• posted

^^^ Ok, didn't know "CIM" meant -per minute.

Tim

-- In the immortal words of Ned Flanders: "No foot longs!" Website @

• posted

Ok, let me lay this out:

RPM: Revs Per Minute, spindle speed, limit by machine design HP: HorsePower, the amount needed to remove CIM, limit the HP rating of your machine FPM: Feet Per Minute, cutting speed, limit for your material, above which chips weld, tools burn, and other bad things happen IPM: Inches Per MInute, feed speed, limit the feed motor, or how fast you can spin the handle DOC: Depth Of Cut, in inches, which can be just one dimensional, or two. If two dimensional, it has units of square inches Lathe or mill. CD: Cutter diameter, on a mill or drill press. On a lathe, the average diameter of the material being removed, like turning bar stock to 3.999 inches with

0.010 DOC, would be damn near 4 inches. (4.0055) M: Machinability rating. HP/CIM, which is the factor you multiply your proposed CIM by to convert it to the HP required to make that cut.

For milling mild steel, about 1. For reaming steel, maybe 1.5. For grinding steel, maybe 2 or even 3 or 4. For milling aluminum, I am actually not sure. Would it be < or > 1? For milling magnesium, < 1.

Machinability rating is work of fracture times area fractured per second. Small chips have more surface area. Work of fracture is roughly Young's modulus times % elongation required to fracture. Tested on Instron tensile tester at NVCC, mild steel, and aluminum.

So: FPM * 4 / CD = RPM;

DOC * IPM * M < HP limit and FPM * 4 / CD < RPM limit and FPM < FPM limit and RPM < RPM limit and maybe

HP * IPM < force limit on tooling

Yes, I am using some symbols twice. But hey, we use FPM and IPM so we can refer to cutting speed and feed speed by just saying their unit names, which helps keep everything correct. They are the same type of "thing". They are both speeds: they are distance / time.

I had a great idea for a simulator: show the three DOC, RPM, and IPM selections on a 3D surface, which may be colored or warped. Then play a synthesized sound file telling the user what it'll sound like to make a certain cut that way. Or, play this:

"Crack! Beep, beep, beep..." (broken tool) or

"Hmmmmm.... pop! Whoosh! Cough, cough, cough...." (stalled motor on fire) or

"I can't believe you ran the cutter into the TABLE! YOU'RE FIRED! .... I'd like to apply for unemployment ...... Not eligible!?.....Yo, buddy, spare change?"

Yours,

Doug Goncz Replikon Research (via aol.com)

Nuclear weapons are just Pu's way of ensuring that plenty of Pu will be available for The Next Big Experiment, outlined in a post to sci.physics.research at Google Groups under "supercritical"

• posted

Hi Chris..

Here is something I developed in the early Ninety's.

Maybe it will help you get a better grip on what you are working with.

WHAT FEED RATE...?

Manufacturers of cutting tools make charts and cardboard slide rules that are supposed to tell us what feeds and speeds to use when milling various materials. It appears most of this information is derived from lathe work and is rehashed for use on the milling machine. The cutting process of milling is about ten times more complex than turning. So I find this approach less than adequate.

The intermittent cutting, the various chip thickness as the tooth enters and leaves the work, the changing tool geometry created as the tool and the work both move together independently, the different manufacturers cutter geometries which may work marginally well in some materials and "Oh boy!" in others, and the cutter buried in the cut creating a "fire" the coolant has a tough time reaching are all factors which make milling feeds and speeds a difficult puzzle to solve.

The recommended milling speeds and feeds distributed by various sources are basically inconsistent; unless one data chart is a duplicate of another. I also think some of this data was documented when railroads were still using steam engines.

First of all, we are talking about end milling and drilling with standard high speed steel and solid carbide cutting tools.

Secondly, we are talking about what the tool itself can handle, not the setup or how husky the machine is. The setup should be rigid and the machine should be beefy enough to "work" the tool without causing noticeable vibration.

We can use the recommended surface cutting speeds for the different materials; but not without forethought. When figuring RPM stay on the light side if the cut is deep. Proper coolant flow may not be available to carry away the heat, so the tool will "give up" prematurely. Remember, the recommended cutting speed is used to determine the highest production RPM with the tool on the outside of the work and drowning in lots of coolant. There is no slowest speed.

The RPM is figured by multiplying 4 times the Cutting Speed divided by the Tool Diameter. The 4 is approximately equal to

12" divided by 'Pi'. This is necessary so inches can be converted to feet and diameter to circumference.

RPM = 4 x Cutting Speed / Tool Diameter

The Feed Rate in Inches per Minute of a rotating tool is figured by taking the Chip Load per Tooth, times the Number of Teeth in the cutter, times the spindle RPM.

Feed Rate = Chip Load per Tooth x Number of Teeth x RPM

These two formulas have been around a long time; and they work in conjunction with each other. The RPM is easy to figure, you have the Cutting Speed and the Cutter Diameter; so with a little math, Presto! You can figure the Feed Rate because you know the RPM, Number of Teeth in the cutter and the Chip Load per Tooth.

Premise one

Cutting tools of different diameters from the same manufacturer and of the same series have the same geometry and therefore look the same under various powers of magnification. An 1/8th inch end mill magnified 4 times looks just like a 1/2 inch end mill.

Premise two

A smooth piece of material doesn't look any different to a 1/16th inch diameter tool than it does to a 5/8 inch diameter tool. Therefore we can look at one tool diameter as being a percentage of another tool diameter.

So lets play the percentages.

There are three basic conditions in end milling. The slotting cut where 100% of the tool diameter is cutting and the trough left behind affords limited chip flow. The roughing cut where the tool is only using 65% of its diameter and has an open side for sufficient chip removal (65% is chosen to make the overlap at the right angle corners during successive side passes). And the finish cut which takes 3% of the tool diameter or less.

During slotting, the tool sees the highest cutting force as it is removing maximum material, therefore it works best at about

2/3rds the roughing cut feed rate. This important fact allows us to increase a pocket-clearing feed rate by 50% except for the initial slotting cut which would be programmed as usual. This makes a nice production increase when spiraling a pocket inside out; because we are not "locked" into the slower feed rate of the initial "slotting" cut.

A given end mill diameter has an optimum "metal-peeling" strength. The factors which try to overcome this strength include, material toughness, percentage of end mill diameter cutting, and depth of cut. Additional tool length reduces this strength a lot; so keep it stubby.

An end mill's Depth of Cut should be figured as a percentage of its diameter. Depth of Cut for all tool diameters will then be easy to figure. Tool depth for pocket clearing in brass and aluminum works well between 1/2 to 2/3rds end mill diameter. Steel is tougher so use 1/4 to 1/3 end mill diameter. This constraint is imposed by the initial "slotting" cut.

Well here we are at chip load per tooth. So how do we figure it for different tools?

Empirically! Drive the tool, what ever size it is, to it's maximum comfortable productive limit. Then write down this data: feed rate, number of teeth in the cutter, rpm, and tool diameter.

We can now figure a Feed Index Number.

FIN = Tool Diameter x RPM x Number of Teeth / Feed Rate

Divide a different tool diameter by the Feed Index Number and we immediately have the Chip Load per Tooth for that tool. This assumes of course, we are working in the same material under similar cutting conditions.

Each of the three basic cuts has its own Index Number. The Slotting number is related to the Roughing number by a factor of

2/3rds; and the Finishing number can be adjusted to suit surface finish. The Feed Index Numbers we use for 6061 aluminum and 360 brass are: Slotting, 117; Roughing, 84; Finishing, 70. These numbers are quite productive; but still allow us to run a tool all night long and have finished parts when we come in the next morning. For slotting with a 1/16th inch (.0625) end mill we divide .0625 by 117 to yield a .00053 chip load per tooth. This times 2 teeth times 3000 rpm equals 3.2 inches per minute feed rate. For roughing use Index number 84 to reach a feed rate of 4.5 inches per minute. Roughing with a 1/2 inch end mill at 2000 rpm and 3 flutes we figure 36 inches per minute.

The feed rate formula now reads:

Feed Rate = RPM x Number of Teeth x Tool Diameter / Feed Index Number

This concept works for drilling too. You can eliminate the number of teeth from the formula if two flute drills are all you use.

FINDrill = Tool Diameter x RPM / Feed RateDrill

Feed RateDrill = RPM x Tool Diameter / FINDrill

This approach allows you, as a specialist in your own shop, to develop feed rates based on the brands of cutting tools and types of material you work with.

Advantages of this system include: more productive feed rates with unfamiliar tool diameters, ease of programming actual feed rates, fewer broken tools, and realistic feed rates for quoting jobs.

A corollary situation developed while drilling. We noticed in drilling aluminum and brass at our popular RPM of 3000, we could use the decimal size of the drill and multiply it by 100 to figure the feed rate in inches per minute. Therefore a 1/8th inch drill who's decimal diameter equals 0.125" would be programmed at a feed rate of 12.5 inches per minute. This also worked for drill diameters up and down the decimal chart. Naturally if the RPM of 3000 is to fast for the application then lower the feed rate in the same proportion as the RPM. Copyright STAN DORNFELD 1989

Feed Rate Corollary

Assuming there is enough RPM available, theoretically speaking, different diameter end mills will be fed at the same rate. Here's how:

Material 316 SST with a surface speed of 50 feet per minute. The end mill is a .75 diameter three flute. Four times the cutting speed divided by the tool diameter gives

266 RPM. The end mill diameter divided by the index number, 117, gives a chip load per tooth of, .0064,

Depth of cut depends on material toughness and the ability of an end mill to eject chips.

Stanley Dornfeld

• posted

I don't usually top post but will make an exception here, simply because I think the entirety of Stanley's post deserves to be preserved. But I did recall reading another similar tretise on this subject and a brief google search brought up teenut's comments and they are worth a read:

Jim (hoping that the wrap works...)

================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ==================================================

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.