[bebob1]

They say manufacturers of machining centers generally set the maximum feed to be half the velocity of the rapids. The top mori seiki machining centers nowadays allow rapids as fast as 1800ipm. So the maximum feed is 900ipm for those machines.

How often do you use the maximum feed when machining parts provided your spindle can spin fast enough to make it allowable according to machining calculations and the chip loading? Or do you prefer to work below maximum feed even in those situations?

[underthetire]

Actually, up to 2000ipm depending on the model. And I rarely see anyone up at maximum feed rate. 400 is about as fast as most people go usually.

[bebob1]

Even when the calculations show you can very well do it in that there is enough RPM? What will be the reason behind this?

Chip clearance issues? Machine life issues? Presumably there is not much effect on tool life if the chip loading remains the same at faster speeds?

[txcncman]

Even when the calculations show you can very well do it in that there is enough RPM? What will be the reason behind this?

Chip clearance issues? Machine life issues? Presumably there is not much effect on tool life if the chip loading remains the same at faster speeds?

Good thinking. You are answering all of you own questions it seems. You forgot, "Tool deflection? Finish quality? Part accuracy?"

Keep thinking about it. You are doing a great job.

[fizzissist]

Your car is capable of 150mph. How often, if you could, would you drive it that fast?

A friend of mine has a good number of machining centers that were going thru spindles at a pretty good rate. They found that by dialing back on the rpms from the max they were able to get much longer life and productivity didn't suffer that much....

Bottom line was it was cost effective to sacrifice productivity in favor of machine life... partly because the premature down-time to replace spindles more than offset the gain in productivity by running at the max.
(this also took into consideration that as the spindle was coming close to the end of it's life, quality would begin to deteriorate, tool life decreased, and tight tolerances were tougher to hold doing critical aerospace stuff)

[bebob1]

A friend of mine has a good number of machining centers that were going thru spindles at a pretty good rate. They found that by dialing back on the rpms from the max they were able to get much longer life and productivity didn't suffer that much....

Bottom line was it was cost effective to sacrifice productivity in favor of machine life... partly because the premature down-time to replace spindles more than offset the gain in productivity by running at the max.
(this also took into consideration that as the spindle was coming close to the end of it's life, quality would begin to deteriorate, tool life decreased, and tight tolerances were tougher to hold doing critical aerospace stuff)

Where does one decide what this maximum speed ought to be? Ideally youd want some study done to know the life of machine parts vs the speed or rpm and choose the optimal between runtime and machine life. But I dont presume this data is available or most shops wouldnt have such study or data done. Then where do they decide on what the maximum feed should be? Is it just completely arbitrary based on machininst's 'feel' much like a detective's 'hunch'?

I know for me on the hobby machine, my maximum feed is set arbitrarily by me based on my priority of limiting wearing. But this is speed was selected arbitrarily and not based on data. Presumably I might not even be operating at optimal.

Even if the manufacturer made improvements that guarantees better reliability at higher speeds, will you change your feeds to higher speeds?

I think mori seiki has ballscrews with cooled cores that allows them to reach the higher speeds with better reliability. So for those machines, maybe even at higher feeds is not the same as other models without core cooling, so the rate of wear may be the same even at higher speeds?

[txcncman]

Where does one decide what this maximum speed ought to be? Ideally youd want some study done to know the life of machine parts vs the speed or rpm and choose the optimal between runtime and machine life. But I dont presume this data is available or most shops wouldnt have such study or data done. Then where do they decide on what the maximum feed should be? Is it just completely arbitrary based on machininst's 'feel' much like a detective's 'hunch'?

I know for me on the hobby machine, my maximum feed is set arbitrarily by me based on my priority of limiting wearing. But this is speed was selected arbitrarily and not based on data. Presumably I might not even be operating at optimal.

Even if the manufacturer made improvements that guarantees better reliability at higher speeds, will you change your feeds to higher speeds?

I think mori seiki has ballscrews with cooled cores that allows them to reach the higher speeds with better reliability. So for those machines, maybe even at higher feeds is not the same as other models without core cooling, so the rate of wear may be the same even at higher speeds?

As has been mentioned in another thread, a lot of what we know about machining is gained through trial and error. Trial = running machine at maximum. Result > error = machine breaking. Next trial = running machine at less that maximum. Result > no error = machine is still running.

Again, you are right on target with your thinking. Keep up the good work.

[Caprirs]

I run an 2006 Okuma HMC that has rapids of 2362ipm and spindle speed of 15K rpm. It is silly fast for the sort of work we do on it. However, if we had to run lights out 24/7 making the same parts over and over, the speed matters over the course of a year.

Everyday, we machine aluminum at 12K-15K rpm and 200-300 inches per minute feed rate often with 3/4" and 1" tools at 1/4" depth. If our programmers would be willing to adopt high speed machining tool paths, we could go much faster on the feed rate.

However, running max'ed out all the time does shorten the life of components. Thus, there is a trade off between more parts per day compared to the obligatory down time to service the machine. That trade off will vary from shop to shop.

[underthetire]

I do know mori probably with a fanuc option, does have adaptive tool life management. You simply set a load for that tool, and the control will modify the feed to maintain that load. Works pretty good for roughing.

[bebob1]

800ipm:

[ame=http://www.youtube.com/watch?v=E3AqIZURMbI&feature=related]HIGH SPEED MACHINING(REALLY HIGH!!!) - YouTube[/ame]

[txcncman]

Ok. Yeah, pretty fast. But what is the actual MMR? Looks pretty low to me.

[Geof]

Ok. Yeah, pretty fast. But what is the actual MMR? Looks pretty low to me.

Yes.

Actually the dead time, air cutting time, is longer than the metal removal time. But it does show the one time you might use close to the maximum feed rate for the machine and that is when you are peel milling a very hard material taking a very small stepover and benefiting from radial chip thinning.

[Delw]

that looks like an old fadal mill with box ways it aint feeding at 800IMP.
more like about 200-300 tops.

Feeding a fadal that fast with that short of stroke will beat the crap out of that machine, I know cause I run one everyday at 150-200" a min and the ball screws dont last very long going over that not to mention tightening the gibbs has to be done alot. and you burn through brushs fast.
its kinda like a jack hammer effect. granted mine is a 40x20 so has alot of weight with 5 kurt double locks on it. I dont like feeding it above 100 IPM on anything shorter than 2" lengths.

My haas has linier guides and better motors it feed nice at 200 but never need to go there cause like was mentioned above there is no big savings, most people waste more time talking and farting around than what you would save for max.

I do lots of surfacing work. on longer lengths I can use larger ball endmills becuase I can spread the step over out farther for the same finish. as a small step over for small endmills. if you think about it a 1/16 endmill for a decent finish you run about a .002-.004 step over. for runnng a 3/16 endmill on the same program you can run about 010-0.015
Thats saving basically 5 passes. when you have surfacing parts will thousands of lines of code thats alot of time savings. where as if you increase the feed you wont go any faster on the entire part.
I been surfacing for about 15 years its just the way I do things. most endmills wont tolorate highs feeds for long durations. with one exception you use oil instead of coolant, but thats a freaking mess.
running coolant with high feeds I have seen no advantage.
right now my tool life last bout 3-4 weeks on one ball endmill. feeding faster ( but yet getting practially the same amount of parts due to finish the endmills last about a week if that. ( for alum) I run 3/64's to 3/16 ball endmills mainly.

[bebob1]

thats what the vid claims anyway. Its possible it never reaches that speed cause its changing directions a lot after a small distance so it probably never accelerates to the commanded 800ipm. But it looks faster than 300ipm though. Depends which portion of the video you are looking at. There are a few passes in the video where its slow, but there are many more bits in there at higher feeds.

[Drassk]

thats what the vid claims anyway. Its possible it never reaches that speed cause its changing directions a lot after a small distance so it probably never accelerates to the commanded 800ipm. But it looks faster than 300ipm though. Depends which portion of the video you are looking at. There are a few passes in the video where its slow, but there are many more bits in there at higher feeds.

A retrofitted Fadal can hit some high speeds. With a better control you get smoother motion which really reduces the load on both the screws and the motors/drives. My '94 will feed at 600IPM smoothly with the KFLOP control, I sized the encoder resolution to the max input frequency at 600IPM so I can't test higher. Accel is set such that it hits 600 in the first 0.75" of travel.

I use 400 IPM on aluminum, and 400 is the max feed rate of a stock '94 Fadal, but I'd never have gone over 200 on the stock control as it wouldn't be able to keep position on a HSM toolpath. This one went over 400 a bit, I think- up to maybe 500-550 on the long passes. It was a very safe cut, though, and an experiment. [ame="http://www.youtube.com/watch?v=ZOfzLbodL_8"]Retrofitted Fadal 4020 (1994) burning through aluminum - YouTube[/ame]