[jheers]

Hey guys, I'm running an ST-20 to cut 2" hot-rolled stock down to a minimum diameter of ~.750. I'm experimenting with different spindle speeds, and I want to try going higher, but I'm a little intimidated. I've been maxing out at 3000, but I think higher speed may help my cause. The chuck is rated for up to 5000 RPM, and the part is pretty well clamped, but I don't know if there are other factors I'm missing. I have the clamping pressure cranked pretty high, but I just can't get over the innate fear I have of pushing the machine too far.

[Geof]

Actually you are pretty nearly maxed out; 3000 rpm on 0.75" diameter is around 600 feet per minute and I don't care what anybody says that is about the maximum you can run hot rolled in a lathe. Unless of course you want to burn out your tools very quickly.

[jheers]

The carbide inserts I'm using say on the package that they can be run up to 1150 fpm, which is why I'm wanting to bump up the speed. I am running with a G96 set at 600 sfm. I'd like to try pushing the speed up beyond half of what the insert is rated for.

[Geof]

That falls into the category of "I don't care what anybody says....." of course the suppler wants you to burn up inserts quickly.

Go ahead and knock your G96 to S800 and remove any G50 rpm clamp. All that will happen at higher rpm is that the bar will push back in the chuck because the grip is reduce by the centrifugal force.

You may find, if you experiment, that you can remove metal faster by keeping the rpm moderate and taking deeper cuts and/or faster feeds.

[jheers]

Haha, okay. I cranked the sfm up to 820, turned the G50 up to 4000 RPM, and it seems to be working quite well. I was looking to achieve the best surface finish, and I had found the "optimum" feed rate and DOC, but it seemed that when I went from ~400 to 600 sfm, the surface finish improved significantly, so I wanted to see if it held true for even higher speeds, which seemed to be true, but the difference from 600 to 820 was not as significant as the difference from 400 to 600. I won't be pushing it any farther, but surface finish is pretty important for this part, so I'll have to evaluate just how quickly we are burning through inserts and possibly adjust down accordingly. For the record, I am not using the bore, so I have a back stop, keeping the part from being pushed into the chuck.

Seems like I kind of wasted your time, asking for advice, then charging ahead and doing essentially the opposite of what you recommended, but I definitely appreciate the input and will keep it in mind for future jobs.

[Geof]

The time wasn't wasted, it was freely given.

Actually if what you want is a really good finish you are doing the correct thing and it may be worthwhile burning inserts out prematurely for the sake of a good finish.

[jheers]

Thank you. I had never realized just how much impact surface speed could have on finish. This part had previously been made of aluminum, and it had been pretty easy to get a good surface finish, even at lower speeds, which I still don't fully understand. I'm not used to machining steel, so this was a pretty big learning experience for me. I'm still a little intimidated by the high RPM, but the result is so nice, I think I can get over the fear.

[txcncman]

If you want to understand more about surface finish, you might want to take some metallurgy classes.

[Geof]

What aluminum alloy? The most common alloy for everyday machining is probably 6061 and you can get good to very good, bordering on excellent surfaces. But maybe those parts where made out of 2011 which probably has the best machinability of all aluminum alloys.

Hot rolled, and cold rolled steel both can give a good finish at high speeds with a good depth of cut and feed. Don't try taking a just a light skim of a few thou because it is likely the surface will not be as nice and also you can burn the tip off the tool very quickly. When the sfm is 600 or above a healthy chip is needed to take away the heat.

[jheers]

If you want to understand more about surface finish, you might want to take some metallurgy classes.

That is the plan. I'm studying for a mechanical engineering degree, but I'm taking a longer road through machining first, rather than being purely academic and entering the field with no hands-on experience. I wound up in a job with a lot of responsibility, matched by my enthusiasm, but there is a lot I just haven't gotten to yet. The schedule between school and working 45+ hours a week makes the schooling a very long process.

What aluminum alloy? The most common alloy for everyday machining is probably 6061 and you can get good to very good, bordering on excellent surfaces. But maybe those parts where made out of 2011 which probably has the best machinability of all aluminum alloys.

Hot rolled, and cold rolled steel both can give a good finish at high speeds with a good depth of cut and feed. Don't try taking a just a light skim of a few thou because it is likely the surface will not be as nice and also you can burn the tip off the tool very quickly. When the sfm is 600 or above a healthy chip is needed to take away the heat.

6061 T6. I can get a good surface finish on that in my sleep most days.

I should be making deep cuts for finishing, too? As it is I am taking off 0.0313 per pass for roughing and .01 for finishing.

I don't have the inserts in front of me, but come to think of it, I think the minimum DOC they are rated for is .039.

[txcncman]

What is your size tolerance for the finish part? Take the largest finish cut you can that still gives good finish and size. Depth of finish cut should usually be close to the tool nose radius of the insert to get good chip control but maintain finish and size.

[Geof]

I was going to say 0.01" is at the lower limit, that is 0.01" on the radius which equates to 0.020" diameter measure; more is better.

The necessity for taking a decent final cut sometimes poses a challenge when trying to get good sizes on parts that have unsupported lengths that are small for their diameter. The final cut needed to get a good finish is often enough to produce noticeable deflection and a taper over the length. This can be corrected by actually programming a compensating taper and probably in production work where conditions can be optimized this can be done. Then you have to carefully watch tool wear, actually it is one time when it is essential to use roughing and finishing tools to make the final cut more predictable. You also have to watch for differences between batches of material. If your friendly purchasing department fails to tell you they decided to save money and order something from a different mill you can produce a great big pile of scrap. If the new material is just mingled in with older stuff so you don't know which is which and they have very different deflection characteristics you have to check each bar as it is loaded in the machine

[haastec]

but I'm taking a longer road through machining first, rather than being purely academic and entering the field with no hands-on experience.

Don't let any of your engineering friends know about this; pretty sure it's not allowed. :nono: