Why IPM?

[CarbideBob]

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).

[dertsap]

Originally Posted by CarbideBob 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

[cdlenterprises]

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

[Salty72]

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...;

[davereagan]

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

[Kai_DK]

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?)

[gridley51]

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.

[fpworks]

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.

[Paul_S]

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.

[wisp]

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