Why IPM?

[MDLang]

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

[dertsap]

, 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

[Geof]

Originally Posted by MDLang ....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?

[HuFlungDung]

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.

[psychomill]

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.

[mrainey]

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.

[Cruiser]

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

[NC Cams]

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????

[dertsap]

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

[Geof]

furlongs per fortnight

[HuFlungDung]

Originally Posted by Geof furlongs per fortnight

A wise guy, huh?

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.

[Geof]

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.