What RPM do you typically run single point threading on a lathe?

[alek95]

I'm using G76

Is there a different canned cycle that is better?

 

[EmGo]

I'm using G76

Is there a different canned cycle that is better?

Yeah, g33 and your brain

Canned cycles suck. If you are in a rush they work but if you want to optimize things, they are shit. Ditch all of them if you want a nice-running efficient program.

 

[Philabuster]

I never quite understood the point of babying a machine too much. They were made to make money. By the time the machines are worn out, there will be newer and more advanced machines out there.

Anyway, there will be better and more advanced machines long before

I'm still running my 1986 Mazak CNC Lathe almost daily. I tend to cap the max speed for the entire program at 2,000 RPM and sometimes go up to 2,500 RPM for small parts.

The machine takes a long time to accelerate and decelerate the spindle at speeds higher than that and I am not in that big of a hurry anyway. I ran the threading test I mentioned earlier just for my own curiosity, but I do not run the machine like that all the time.

My Mazak is 37 years old but it still makes good parts.

 

[alek95]

I'm still running my 1986 Mazak CNC Lathe almost daily. I tend to cap the max speed for the entire program at 2,000 RPM and sometimes go up to 2,500 RPM for small parts.

The machine takes a long time to accelerate and decelerate the spindle at speeds higher than that and I am not in that big of a hurry anyway. I ran the threading test I mentioned earlier just for my own curiosity, but I do not run the machine like that all the time.

My Mazak is 37 years old but it still makes good parts.

We live in different worlds.

Our oldest machines are 2012. They are pushed to 100%, 18 hours per day.

They will be a long forgotten memory by the time they are 37 years old.

I would get laughed out of the facility if I capped the RPM to 2000.

 

[EmGo]

We live in different worlds.

Yes, but .... you still don't want to abuse things. If you're using tool nose radius comp, constant surface speed, and canned cycle roughing and threading -- then saving two seconds by jacking threading speed up is not the best way to treat your equipment.

As I probably mentioned, there's this thing called inertia. Most moves, even rapids, have acc and dec in the motion - but threading can't. It's *got* to move at the proper speed then it's *got* to stop on a dime, and that's hard on stuff. You'd be way better off looking at other places to cut cycle times. Like ditching the effing g4123, the halfass roughing cycles, the css in places where it's not needed, lots of better areas to optimize than threading speed. Even threading, if you watch the chip, you will see where you can make it work better with g33.

Canned cycles are fine for making a few parts where ultimate efficiency doesn't matter - but they are shit for long-running jobs.

 

[alek95]

We don't use any canned cycles except for threading and for drilling/tapping with live tools.

 

[angelw]

Most moves, even rapids, have acc and dec in the motion - but threading can't. It's *got* to move at the proper speed then it's *got* to stop on a dime

The rate of acceleration/deceleration, relative to slide velocity, is the same whether the move is Rapid, Feed, or Threading. The only difference between G32/G33 and G01 is that the Feed Override is locked out with G32/G33. Hence the reason for a minimum start distance from the start of the Thread to circumvent Lead error due to acceleration at the start of the Thread. The same applies at the finish end of the Thread due to deceleration, only to a lesser degree.

Machines with Z Axis Load meters will indicate 100% and greater load briefly during acceleration and deceleration in a Rapid Traverse move. As its not possible to Screw cut with a slide velocity greater than Rapid Speed and generally no greater than a maximum Feed Rate slide velocity of the machine, screw cutting at high slide velocities is going to be no more detrimental to the machine than the many Rapid Traverses encountered in a roughing operation. The thing with Screw Cutting, whether by Canned Cycle, or a series of G32/G33's, is that there can be many stops and starts (depending on the Thread Depth) in quick succession. But Thread Leads of circa 1.5mm usually only require 6 or so passes and in many cases, again depending of the workpiece, less starts and stop from Rapid than in the roughing operation.

 

[DouglasJRizzo]

@alek95
It only costs money.

 

[EmGo]

We don't use any canned cycles except for threading

So ditch them on the threads, too. But I'm betting there's lots of places better to lose two seconds than by speeding up threading passes to infinity.

 

[alek95]

So ditch them on the threads, too. But I'm betting there's lots of places better to lose two seconds than by speeding up threading passes to infinity.

You really think I haven't looked at every part of the program to see where I can shave off a fraction of a second?

 

[EmGo]

You really think I haven't looked at every part of the program to see where I can shave off a fraction of a second?

Sorry, but from evidence given here, no I don't

Or to be more exact, I agree you've looked at it but some of your ideas are less than wonderful.

Not to beat you up but, for example

I'm doing .004 per pass and 3 finish passes. Carbide tool of course.

.004 ? Thread depth is .034, personally I'd do it in three plus a spring/light finish, you are taking 8 plus 3 spring passes ? Even the mistubishi chart shows 6 total

https://www.mitsubishicarbide.com/application/files/5314/7191/5783/tec_threading_depth_external_en-us.pdf

way better off to kick up the doc a little, save several passes, rather than spin the thing to the moon and torture your z axis drive and motor.

I'll go out on a limb here and say, if you are roughing any amount of material ? You can kick the doc up a lot and save passes. That's more effective on a lathe than faster speeds and teensy tiny cuts.

 

[SND]

IF anyone here has a Doosan Lynx2100LB, how fast are you guys threading?
I've only gotten up around 300rpm, using G76, tried a bunch of different settings, pretty loud bang every time the tool retracts, just doesn't sound happy. Changing the number of turns on retract just seems to get ignored by the controller and always pulls in about 1/4 of a turn.
Not sure if its a parameter thing or wtf. anyway, i don't thread often at all and at least it makes a nice thread on these parts but sure seems to me something isn't working as it should.

 

[DouglasJRizzo]

@SND
A loud "bang?"
Call service.
I routinely thread around 1000 or so RPM with operation being smooth and quiet.
Really, have the machine looked at, it shouldn't be like that.

 

[michiganbuck]

And on a manual lathe stopping at a shoulder, the pull away is aided with the compound at 30* (291/2) because you pull away from the part.

I never got a reply on my putting a slip of tape on the chuck lets me stop on the dime, looking at the chuck rather than the part.
50/60 rpm, like Seifieberg said is a good speed..and sometimes 150 or so.

 

[sfriedberg]

50/60 rpm like Seifieberg said

Who dat?

 

[escapethewrmhole]

Seems odd to pick any one RPM. I do the math for the surface footage and go with that. Usually ends up around 400SFM.

 

[EmGo]

Seems odd to pick any one RPM. I do the math for the surface footage and go with that. Usually ends up around 400SFM.

Which is roughly 2,000 rpm for a 3/4" thread, cooking right along there ...

 

[alan speyrer]

Yeah, threading on a manual lathe with neither an automatic feed stop nor a spring loaded tool retract, I am frequently at 50/60 RPM. My lathe has no clutch, but it does have a brake, which I am using pretty solidly even at that low speed to avoid smacking into shoulders. On a machine that doesn't even have a brake, I'd at least double the thread runout groove.

turn the threading tool upside down and thread away from the shoulder.

 

[exIT]

I'm doing some 9/16-18 OD threads in 4130

I started off at 750 rpm. It was fine.
So I went to 1000. Also fine.
Then I bumped it to 1500. Also great.

How far do you guys push it? Should I try 2000? 2500?

Im doing .004 per pass and 3 finish passes. Carbide tool of course.

Machine is a Doosan Lynx 2600 SY and the insert is a mitsubishi insert VP15TF grade.

Find out what the max threading feed rate should be from the manufacturer. On my Hardinge Talent it is 120 IPM. If I was threading 9/16-18 I would probably run the spindle about 1800-2000 RPM which would result in about 265-295 SFM and 99-110 IPM. The only reason to go slower would be if you don't have any room at the end of the thread. Going faster will result in a larger imperfect end of thread.

I use G76 almost exclusively. Works for me. I would use the variable doc and start with a Q value of .015 and set the parameters for one finish pass.

 

[cnctoolcat]

For an equal load on the tool you take a big bite the first time, then a smaller one, then smaller again, until the last pass is only a thou or so. And then a spring pass if you need it.

Mazak has been doing this since 1981, with the introduction of the Mazatrol T1 conversational control.

Threading is one of the many beauties of Mazatrol: you can override any of it, yet the program auto-fills SFM, thread height, first DOC, # of passes. It's all right there in plain English: infeed angle, infeed method...although it takes a parameter tweak to run only one threading pass (who does that anyway?)

Mazatrol can feed down one flank at the angle you program, feed down the other flank, or straight-in, equal cutting on both flanks. Pretty capable stuff...

I've always single-pointed at less SFM's than most: chatter is often reduced or eliminated, threading is so fast it don't matter, tool life is more predictable, easier on my machines.

ToolCat