Why can't threading speeds be changed on CNC lathes?

[Hogger]

I've always wondered this, I've ran several different CNC lathes in my life and all of them will cross thread if you make a thread and then decide you need to change the speed in the middle of the thread to reduce chatter, or if your running a roughing tool and a finish tool the speed has to be the same for both, you can't run say 500 RPM on the rougher and 800 RPM on the finisher. It seems to me the machine should know where it is at all times and speed wouldn't matter.

[Eurisko]

Interesting...

was the programmed feedrate in inches per minute or inches per revolution? I can understand i.p.m. messing up the threads if the rpms change, but you'd think that i.p.r. would sync to the spindle speed.

It should be possible to cut tapered threads in G96 (constant surface speed) mode if the feedrate is programmed in i.p.r.

Also, (If I recall correctly), the Cincinnati lathe I ran years ago locked out any speed or feed overrides in threading mode.

Even the vertical machining centers lock out speed & feed overrides while in tapping cycles.

Weird.

[HuFlungDung]

My best guess would be that the acc/dec rate of the Z servo is constant. When you change spindle rpm, the feedrate increases proportionately for threading at the higher rpm, however, the servo still cannot accelerate any faster than it did before, and it has to accelerate for longer to get to a higher feedrate.

A certain number of cpu cycles is required to detect the encoder index, and to initiate motion. Since the time delay between detection and motion is fixed, it seems reasonable to assume that a faster running spindle has managed to turn a little bit further than it did previously, before the servo gets up to higher speed at the faster rpm. This amounts to a change in timing.

[jackson]

I've always wondered this, I've ran several different CNC lathes in my life and all of them will cross thread if you make a thread and then decide you need to change the speed in the middle of the thread to reduce chatter, or if your running a roughing tool and a finish tool the speed has to be the same for both, you can't run say 500 RPM on the rougher and 800 RPM on the finisher. It seems to me the machine should know where it is at all times and speed wouldn't matter.

Well some machines you can use the the override on the control it kind of a pain cause you have to wait for it to come back to the z stat poin then ajust the override

[Geof]

I am not sure if this is what you mean but this program runs okay on a Haas TL1. Starts at 1000 rpm and then drops down to 800 then 400 and the tool stays on track.

%
O00016 (THREADING)
G20 G40 G80 G99 G61 G97
G53 G00 X-2. Z-18.
T202 S1000 M03
G00 Z2.
G00 X2. Z1. M23
X1.77 Z0.2 M08
G92 X1.74 Z-1. F0.125
X1.7
X1.66
X1.62
M03 S800
X1.6
X1.58
M03 S400
X1.56
X1.54
X1.52
G00 X2.
G00 Z6.
M30
%

[jackson]

I am not sure if this is what you mean but this program runs okay on a Haas TL1. Starts at 1000 rpm and then drops down to 800 then 400 and the tool stays on track.

%
O00016 (THREADING)
G20 G40 G80 G99 G61 G97
G53 G00 X-2. Z-18.
T202 S1000 M03
G00 Z2.
G00 X2. Z1. M23
X1.77 Z0.2 M08
G92 X1.74 Z-1. F0.125
X1.7
X1.66
X1.62
M03 S800
X1.6
X1.58
M03 S400
X1.56
X1.54
X1.52
G00 X2.
G00 Z6.
M30
%

looks like i may have to try this

[sencinia]

I've always wondered this, I've ran several different CNC lathes in my life and all of them will cross thread if you make a thread and then decide you need to change the speed in the middle of the thread to reduce chatter, or if your running a roughing tool and a finish tool the speed has to be the same for both, you can't run say 500 RPM on the rougher and 800 RPM on the finisher. It seems to me the machine should know where it is at all times and speed wouldn't matter.

Some lathes do allow spindle speed changes via the override knob on the control. But they need to have that option from the factory.
We do it all the time on J & L 4 axis lathe to find the optimum speed, then edit the program to that.
Most machine will cross thread if the speed is changed.

[Hogger]

Our machines won't let you change the speed with the override, just last Thur. I was making a 6" long 1 15/16-10 LH thread gage for a part we had to make, I was running a center in it and tried to thread it at 600 RPM, guess what... it chattered badly, so I slowed it down in the program to 300 RPM and tried it again, setting the wear offset high so I could see where the tool tip was cutting, I ended up having to use -.025 Z wear offset to get the tool back in the center of the tread.