I have tried many times to rationalize the extensive use of inches per minute as a feed rate and I can come up with no good explanation for its use other than as a constant maybe for calculating metal removal rate.

So often I see IPM used in post and at one time I would calculate out the feed per rev and best yet the feed per tooth but I can't be bothered anymore.

It seems to be a painful way to calculate a reliable feedrate.

Is there a good reason for using IPM that I have simply overlooked? I'm assuming there must be or it would not exist.

Mike

, inches of travel per minute or mm/min
parts are measured in imperial or metric
its the sams as miles/hour or km/hour

its only the distance traveled , metal removal rate is measured as cubic inches per minute

rpm and ipm are calculated usually by sfm

....Is there a good reason for using IPM that I have simply overlooked? I'm assuming there must be or it would not exist.

Mike

What do you use if you do not use IPM?

IPM, I believe, is the most basic parameter for controlling the rate of motion. If you are given IPT, then the control must also know how many flutes are active and what the rpm is, in order to then calculate the feedrate for the servo. The velocity for the motor has to be distance/time.

I believe Hu expains it the best. On a lathe, you're generally programming as IPR since for the most part, you're programming as one tooth effective. With the part spinning with the spindle, surface speed is a given and controled by X position (when using constant surface speed). A very "layman" view but anyhow.....

On a mill though, as Hu stated, there's certain information that the machine does not know. Number of flutes (being the major issue), surface speed of the cutting tool (since the diameter is unknown to the machine), and this combined with cutting arcs (or linear distance) across the part. When programming in IPM, these things are considered and calculated for. Is it a pain? Not really. Been doing it for so long that it only takes a split second to calculate.... really.....

Now, with the advent of some conversational programming controls, many mills can be programmed in SFPM and IPR. Since many of these machines have full Tool Data information (number of flutes, cutting diameter, tool material, tool type, even further to HP limits, rpm limits, etc). The Tool Data page makes it possible to program that way. Some machines even allow for the data to be used for EIA/ISO programming.

I have a different opinion.

I've always preferred IPR for machining centers, and have used it whenever possible since the early nineties.

All feedrate information is supplied by manufacturers and reference books as either IPT (milling tools) or IPR (holemaking and turning). Determining IPM always involves an extra calculation (which may or may not be a problem for you, depending on your programming resources.)

You can't look at an IPM value by itself and have any idea how hard a tool is working. IPM is meaningless without knowing RPM and number of cutting edges. Drilling with IPR involves no reverse calculations, milling with IPR requires one fewer.

When optimizing at the machine - with IPR, you have completely independent control over chip load and surface speed when using the overrides. With IPM, if you override the RPM, you're also changing the chip load, whether you want to or not.

IPM is required for horsepower calculations.

Both methods make equally good parts. One just requires more effort than the other.

Then what you may need is a good milling slide type calculator, or spend more and get the electronic one for your pocket.

Goes back even further in math/calculus.

First you have displacement, inches.

Then you have the first rate of change (usually expressed over a function of time) which is inches per minute.

Then you have the rate of change of the rate of change (which is acceleration, again per unit of time) which is inches per minute per minute.

They you have jerk which is the rate of change of acceleration or inches per minute per minute per minute.

When doing force calculations, the amount of power consumed is dependant upon now much work is performed over a time interval. Do more or the same work in less time and you require more power.

The conversion of inches to feet or millimeters or whatever unit you want to work in is simply a necessary evil and irrelevant to the "reason".

By computing the projected amount of material being removed and then knowing how fast you wish to plow the cutter through it, you can determine the VOLUME of material being removed over a unit of time and therefore the power required to do do.

When you do the math of cutting calculations, IPM is as critical as any factor in determining the RPM of the cutter and the rate of travel that you'll be able to make thru any material that you'll be cutting.

Why IPM? What else would you use and why not????

i ve always disliked km/hr , maybe we should change it the whole system , one universal system imperial and metric get confusing ,

how bout beers /hr
but then shots / min could be dangerous

furlongs per fortnight

furlongs per fortnight

:D A wise guy, huh? :D

In explaining why IPM is used, I did not express any opinion of whether I liked it or not. I like IPR for use on a lathe. But, if the question was "why IPM", it could be considered a legacy parameter from the beginnings of motion control itself. IPT is a higher level term which must be plugged into an equation to solve for IPM. As cncs evolve, IPT may well become the norm eventually, but will never be a 'feedrate' in and of itself.

Okay I'll be serious (spoilsport).

To me it seems quite fundamental. Cutting is done on a per tool, or per cutting edge, basis.

On a lathe there is one cutting edge and it is advancing at a certain distance per revolution so the simplest way to express feed is in inches (mm) per revolution of the workpiece; feed per revolution (fpr)

On a milling machine there can be more than one cutting edge advancing into the work by a certain distance per revolution so the simplest way to express the feed is to multiply the inches per revolution by the number of teeth and the revolutions per minuteto get inches per minute (ipm).

I will agree with mrainey that you can get into exotic calculations regarding horesepower and metal removal rates but when you are using a particular machine you are dealing with a fixed horsepower and you can use the spindle load meter to see if you are loading the machine too much.

I will also agree that if you have used the recommended feet per minute from a reference book you come up with numbers that are a nuisance to handle with mental arithmetic. Speeds and feeds always have a range so make things easy; round the recommended surface feet per minute to the next ten down and round the spindle speed to the nearest 100 or 1000 rpm depending whether you are dealing with steel or aluminum, etc. A two flute cutter taking 0.005" per tooth spinning at 10,000rpm needs a feed of 100ipm. This is not a difficult calculation.

OK here is how I see it, IPM was used on machines where the feed mechanics are not synchronised to the spindle, often because there was no NEED to do so on that type of machine....lathes and boring mills are both examples of machines that NEED this synch to be able to chase threads.......milling machines did not typically chase threads thus their feed mechanics were directly driven from the power source not from a gear train from the spindle.

Also milling machines often use a rapid traverse of some kind that simply makes the leadscrew spin faster to move the table rapidly...and you often need or want to move the table with the spindle stationary.

Bill

Screw IPR or IPM... that's kid stuff! and ancient history. Our machines are so fast that we program in MPH (miles per hour..... KPH for you metrics)..... :boxing:
.
.
.
.
.
.
.

:tired: (as I wake up).... Did someone say somethn' ???


:cheers: :cheers:

Let's look at this from the perspective of how I handle feeds and speeds in the job shop that I work at where we cut materials from aluminum to inconel.

We run mazaks and specifically I run mills. Perhaps this alters my perspective.

First I look at the drawing and what the material is. Lets say we're going to cut cast 4130.

Next I determine what operations are required to cut the features on the piece then I can explore my tooling options.

Once I have chosen my tooling I can easily determine my feeds speeds and doc's based on historic evidence of what works or in the case of new tooling I can use the manufacturers recomendations, observe tool life and wear and make changes.

I know that any tool regardless of diameter or number of inserts using an APKT 1604 insert of a certain grade from a certain manufacturer with a certain chip breaker can run at around 550 -750 SFPM and a .004 - .006 feed per tooth at somewhere between a .12 - .2 DOC full engagement.

So let's say I'm going to face the casting with a 3" 5 insert 90 degree facemill, then I'll produce a shoulder with a 1.25" 3 insert 90 degree endmill and then rough out a bore with a 1" 2 insert 90 degree endmill.

As it happens I can run the same insert in all these cutters so all I need to do is choose my starting values and they will be the same for all the above. SFPM is exactly the same regardless of diameter, chip per tooth is the same and only needs to be multiplied by the number of teeth to get the needed feed per rev.

Lets add a couple endmills into the mix and say I'm going to finish that bore with a .625 coated carbide endmill to 1.25 deep and I'm going to mill a slot to .5 deep with a .5 endmill. Again I'm going to recall that I should be able to run a coated carbide endmill in this material at about 250 SFPM at between a .001 -.0025 chip per tooth depending on engagement. So in the slot I choose 200 SFPM to start with a .005 FPR at .25 DOC and finishing that bore I'll go 300 SFPM full depth at .OO8 FPR.

Once I'm up and running I watch my tooling and make adjustments up or down to my SFPM or my feed per rev or maybe I'll change my DOC and make an incremental adjustment to each.

Quite simple. I could really care less about the rpm or the IPM unless I want to calculate the time difference between cutting strategies which I've usually already done when I choose the tooling.

SFPM is speed and Feed per rev is feed, IPM is the combination of both so why would I want to take the extra step and now be in the dark as to which variable is maybe causing a problem? How can I start to understand what speeds or feeds work if I move beyond them and into IPM?

SFPM and chip per tooth are universal for a given material and a given family of tooling at common doc's. So I still don't see why I, not the control, would use IPM for cutting conditions.

Mike

We run mazaks and specifically I run mills. Perhaps this alters my perspective.


As you state it.... and I suspect you're running Mazatrol.... which alters your view some since conversational programming is somewhat different than the "non-conversational" world that many people are in... But the points you make are well worth noting.... and the very reason why many question the use of or question the reasoning behind it.

sfpm will become a sad mistake of the past , its missing too many variables
sandvic has formulas on their site that gear more to cubic inches/min , the speeds and feeds are based upon variables : ,depth , engagement tool dia , # teeth , type of material , insert grade (if not solid), normally the sfpm is calculated far beyond what is stated on the box , with better tool wear and faster production

with that said it still calculates it out to ipm and rpm

Ok, even if I ran a straight g-code machine with no conversational control I think I would still want to think about the work my cutter is doing in SFPM and FPR. I write G-code subs for the mazaks and even though I have to calculate the RPM I can program the feed as feed per rev. I could on the Hass machines at school as well. I also relate that information to others as SFPM not RPM.

Lets look at an example from the fast stock removal post.

"I have used a 1" 3 flute at 3055rpm and 27 IPM on a Haas TM-1 with a 0.100" DOC. and no problems in 1018 steel."

Say what?

Lets get out the calculator because I have to reverse engineer those figures to find out how that cutter is really running.

Once I know that what he is really saying is "I have used a 1" 3 flute at 760 SFPM and a .009 FPR " I can say to my self "Hey that's .003 per tooth. The .100 DOC in 1018 is maybe a bit shallow but the rest is not bad."

Can anyone look at RPM and IPM and not have to do what I have to do to get a "feel " for what's really happening?

dertsap, I have and occasionally use Sandviks Cutting data module, I have it on CD. It works very well for Sandvik tooling. Unfortunately the only sandvik milling tools we have are the R-210 feedmills.

Mike

[QUOTE=MDLang;


dertsap, I have and occasionally use Sandviks Cutting data module, I have it on CD. It works very well for Sandvik tooling. Unfortunately the only sandvik milling tools we have are the R-210 feedmills.

Mike[/QUOTE]

it works just the same on other tooling it s just a matter of comparing grades between different manufacturers

for me material (cubic inches /minute) removal rate makes more sense , a guy can have a better sense of how many consumables are needed for a job , better idea of how long the tools will be cutting

I agree 100% with you, Mike. I think we're in the minority here, just not sure why. :-)

Two quotes, both correct;

"IPM is meaningless without knowing RPM and number of cutting edges"

"SFPM is speed and Feed per rev is feed, IPM is the combination of both so why would I want to take the extra step and now be in the dark as to which variable is maybe causing a problem? How can I start to understand what speeds or feeds work if I move beyond them and into IPM?"

However if the machine wants you to express things in IPM in the command setting feed rate then you use IPM. If you don't like that I guess you will have to invent time travel and retroactively chnge a lot of things.

That's why I said I use IPR whenever possible. If a control won't accept it, well .. you do what you gotta do.

I haven't run into a machining center control in a long time that can't be configured for it, but I'm sure they exist. We recently had to pay a few bucks extra to get IPR on some new Okuma & Howa and Toyoda HMC's with Fanuc 16i's. One parameter change did it.

Can anyone look at RPM and IPM and not have to do what I have to do to get a "feel " for what's really happening?


Yes. It all comes with experience in using it, and the ability of ones mind to be able to retain the data. I think of it kind of like learning the multiplication tables in elementary school. At some point, you memorize them so you don't have to figure it out in "long hand". The rest of it, you have a general idea of where things are at... or "feel" as you state.

for me material (cubic inches /minute) removal rate makes more sense

Programming directly to MRR doesn't necessarily mean the optimal for particular cutters. It's only a reflection of volume. I've been using MRR for many years though as a baseline in which to figure out cutter usage, efficiencies and comparisons for tooling when checking out new stuff. It's also a good gage for HP usage (in respects to machinability) and acceleration data for different cnc builders. And it does give a good general idea on "how long a tool will be cutting".... as an amount of time though, not as wear.

As Mike (Rainey) changed on his machines, many machines can be changed to IPR with a simple parameter change. Most you can even force with a G code (for example, program in "G95" as opposed to "G94"). Then you don't have to change a parameter. Most machines have a default status parameter for G94 or G95. That's probably what the guy changed. The problems you may run into however, are going to be with some options. Some control options (like G5 or Nanno use for instance), may not be able to utilize and control itself under a IPR feed. The control variables are set and written for IPM. Now, its possible that some controls may be able to change parameter sets or Ladder to correct this for IPR.... not sure though since I've never done it.

Yes, going back and forth between modes is usually as simple as choosing either G94 or G95.

I did use IPM for probing.

And, responding to what somebody said - rapids work the same in either mode (on the controls I've used, anyway) - spindle doesn't have to be running.

IPM is just a convenient way of specifying velocity to the controller, you could just as easily program in MPH. The controller works in counts per second ( actually counts per 1/1000th of a second) from the encoders. On a lathe it knows the spindle speed so the computer coverts your feed per rev to IPM which it can then convert to counts per second. On a mill the cnc doesn't know your cutter dia. or the number of teeth so it can't do this math by itself.
From the cutter's standpoint what matters is SFM and chip load per tooth. SFM is how fast the cutter is passing across the steel. Think of a shaper, higher ram speeds equal higher SFM. As the material is sheared by the cutting tool at higher speeds more heat is generated at the cutting edge. Get the speed high enough and the cutting tool material breaks down from too much heat. This is why carbide runs at higher speeds than HSS it can withstand much higher temperatures before it begins to break down.
The other major variable to the tool is chip load per tooth. Many people confuse this with feed per tooth but they are not the same. In milling chip load equals feed only when 50% of the cutter is in the cut. The chip thins with lower cutter engagement which is why you can sidemill at 5 times the feedrate you would cut a slot . On a lathe you thin the chip with lead angle or radius size, feed per tooth equals chip load only with a 0 deg lead and 0 radius. The easiest way to determine chip load is: A: draw it in CAD, or B: measure the chip produced with a pair of calipers and divide by a fudge factor (usually about 1.4 for steel)
I'm sure the people at Sandvik would be floored by the comment that SFM is a sad mistake from the past. It is the most crucial parameter in correctly applying a cutting tool. There is no one correct SFM for a given material which is why the cutting tool suppliers specify a range. For example in side milling the tooth is in contact for a very short time so it does not absorb as much heat and a higher SFM can be used. But one thing is constant, higher SFM means more heat (until you reach supersonic speeds, then things get really strange, heat goes down and HP requirements diminish).

I'm sure the people at Sandvik would be floored by the comment that SFM is a sad mistake from the past. It is the most crucial parameter in correctly applying a cutting tool. diminish).

at a company i worked for these were common speeds and feeds i was running a 3/4" 3flt on 1018 , .125 depth of cut at .25 engagement , with simple 4030 grade


been a while since i've had a box of sandvik inserts in my hands
maybe you can refresh my memory what sfpm does it recommend on the back of the box

almost forgot to mention , insert live was near double from what we used to follow on the back of the insert box

Wow...this is making me dizzy. I like the beers/hour suggestion :cheers:

I think the IMP (G94) is great especially if you have no feedback and can't determine spindle speed.. otherwise IPR (G95) would result in no travel and no cutting, _HOWEVER G95 is a really good option if your spindle has been dis engaged thru an MO5 command. as you wouldn't want travel if you have no rotation of the cutter...;

When I changed from G94 to G95, it gave me more control of the process. Most programs I write are gone in 5-10 minutes because almost all my work is prototyping, so more flexibility is better. If in G94 and I need to cut override the speed and cut it in half, I need to simultaneously move the feedrate pot an equal amount or the chipload will double. Also, if the setup turns out more rigid, I can override speed 50% and feed per tooth by 50% for a total of 2.25 times the productivity. With G94 IPM, I could only increase productivity by 50% on the fly. In production this is all happy crap, but prototyping one off parts, it frequently makes a difference. There is a downside. Forgetting to change the number of flutes in the tool file after taking a 6 flute endmill out last week and putting a drill in that pocket this week gets me in trouble, but not too often. I watch the drill go in. The biggest trouble is importing a program that works in G94 and changing it over to G95, but leaving the feddrate in inches per minute, like 8 or 16. That's an enormous chipload. LOL. Ugly. Overall though, well worth the difference. Wish I had started with G95.

Dave

How is the data for the tool loaded, when using IPM (teeth, load, etc.)?
G94 aaa bbb ccc ddd?
G10 aaa bbb ccc ddd
What's the metric conversion for IPM? (MPM?)

I`m in the minority as well,prefering ipr.Well mmpr over here.Lot simpler,you look at a multi tooth cutter,you think 0.004" per rev,ten teeth,feed is 0.040" per rev.If you want to use the speed overide the feed stays the same.
I think ipm is a throwback to the days of manual machines.

Several months ago, I was almost convinced to change all our milling programs over to IPR (G95) since it seemed to make everything simpler. Before I changed my first program, I realized that IPR gives me absolutely no feel over how fast the machine is feeding. Toolpath geometry is sometimes the most important consideration when choosing a feed rate and IPR doesn't tell me anything about how fast I'm about to interpolate something like a small circle.

The IPT is important to the cutter and second to cutter tool life. (SFPM is number one issue to tool life.)

But for finish feeds I calculate my IPM based on RPM and IPR. Especially for peripherial cutting of surfaces. I use for an AA or Ra finish of 125 the muliplier of .0405 x sqr(tool dia) x RPM to give me the finish feed rate. If I want a better finish then I multiply by the sqr( finish wanted / 125). Works quite well.

End cutting if the cutter has no radius I use .0048 as the minimum multiplier to RPM for my IPM. Again this is for finish. If the cutter has a radius the above .0405 x sqr( 2 x radius) x RPM works fine.

Don't forget about Degrees per minute. If you are programming using a 4th axis you will likely be using DPM. Most machining centers control the rotary axis with feeds expressed as DPM. DPM = 360 x IPM / circumference of your workpiece.

Which is fine if you are ONLY feeding with the rotary axis, but what if are also feeding with say, the X axis while rotating? You must account for the X distance and the rotational circumference distance to calculate a chipload. Example: you want to index the rotary 2 degrees while simultaneously feeding 20 inches along the X axis. If you commanded a feedrate of F360, (1 RPM), it would only take the rotary a second or two to index the 2 degrees, but the X axis would try to move the 20" at the same time, resulting is a nicely snapped off tool.

And for five axis simultaneous programming...... inverse time feed. and a big pain in the fanny.

hehehe cheers,
Michael