G32 thread cycle

[cuttergrinder]

I need to machine grooves in a cable drum. Ive always done these on a manual machine but we want to try one on the cnc lathe. The groove does not run clear off so I need to plunge and then retract in X while in the thread cycle. Im thinking of using a G32 thread cycle. Will code such as this work?

G00 Z-3.
X 10.1
G32 X 9.9
Z -13.
X10.1
G00 Z-3.05
G32 X 9.85
Z -13.05
X10.1
G00 Z-3.1


And keep repeating at smaller X values and moving over in Z slightly. If this code will work, I can generate code on a spread sheet that will profile the groove with a small round grooving tool.

 

[EmGo]

I need to machine grooves in a cable drum.

Are you talking about the kind of thread that doesn't go around in a regular helix, but has a kind of jog in it at one spot ?

The only one I have ever heard of that could do that was G&L. Would be interested to hear if there's others now.

(In standard code, if you did a G33 with an X departure you'd get a face spiral. The G33 goes in the line with the Z departure. But who knows what evil lurks in these weirdo controls ? da angel do )

 

[cuttergrinder]

The grooves are just a thread with a round bottom and fast lead that plunge in and retract in x while still cutting. These grooves are a 13/32 radius with a 7/8 lead. The cable drun is about 10' long and 14" in diameter. It needs 54" of grooves on each end. 1 end right and the other left.

 

[EmGo]

The grooves are just a thread with a round bottom and fast lead that plunge in and retract in x while still cutting. These grooves are a 13/32 radius with a 7/8 lead. The cable drun is about 10' long and 14" in diameter. It needs 54" of grooves on each end. 1 end right and the other left.

Ah. On an American control that's easy, but takes three blocks per pass. Position the tool in X off the part surface at the Z start point, then first threading block a G33 with a Z and an X and your K lead, then next block no G33, just the Z departure, no lead, then next block again no G33 but an X and a Z departure and no lead, then back to the start point in rapid. You only want to read the lead and the modal G33 once at the beginning of the pass. Your plunge in will be a little tricky because it takes a moment for the slide to start moving but since this is not a real thread probaly won't matter. I usually did a 45 because that's easier but not necessary, could be any angle you want. Spindle in G97 and don't change speeds, the threading is just a marker pulse so anything you change between passes is going to mess it up.

But there's another style that G&L had codes for, where there is a jog in the thread. Supposed to get more cable on the drum or something ... they were the only ones I heard of doing that.

 

[cuttergrinder]

My machine only seems to use G32.

 

[sinha]

Plunge with G01, cut with G32, radial retract with G01, followed by axial retract by G00.

 

[angelw]

My machine only seems to use G32.

Hello cuttergrinder,
There are Three G Code Systems available via parameter setting, System A, B and C. System A uses G32 for Basic Threading, B and C use G33. Your control is set to the default of System A.

Plunge with G01, cut with G32, radial retract with G01, followed by axial retract by G00.

Hello Sinha,
In the OP's case it would be better to Feed in and out with G32 as it will be synchronized with the Spindle the same as for the Axial move. Using G32 in this way is Called Continuous Threading, as the system is controlled in such a manner that the Synchronization with the spindle does not deviate in the joints between blocks wherever possible. Accordingly, it's possible to performed special thread cutting operation in which the lead and shape can change midway.

For the most part G32 functions the same as G01, except that its fully synchronized with the Spindle and Manual Feed Rate override is blocked. On critical Drilling Operations where the operation is sensitive to Feed Rate, such as when using an Elector Drill, or Gun Drill, I use G32 instead of G01 when feeding the Drill.

Regards,

Bill

 

[GENERALDISARRAY]

I need to machine grooves in a cable drum. Ive always done these on a manual machine but we want to try one on the cnc lathe. The groove does not run clear off so I need to plunge and then retract in X while in the thread cycle. Im thinking of using a G32 thread cycle. Will code such as this work?

G00 Z-3.
X 10.1
G32 X 9.9
Z -13.
X10.1
G00 Z-3.05
G32 X 9.85
Z -13.05
X10.1
G00 Z-3.1


And keep repeating at smaller X values and moving over in Z slightly. If this code will work, I can generate code on a spread sheet that will profile the groove with a small round grooving tool.

After watching this it should feel like cheating, he explains it soo good.

 

[EmGo]

Plunge with G01, cut with G32, radial retract with G01, followed by axial retract by G00.

This won't work. He'll get a groove at the beginning of the thread, then a waggly start, then an uncontrolled straight pullout at the end. The entire pass needs to be locked in at one feedrate, synchronized to a particular spot on the circumference of the part.

I forgot that in my example you need an I as well as a K in the feed-in, fed-out portions of the pass But that's not Fanuc, just a general example.

For the most part G32 functions the same as G01, except that its fully synchronized with the Spindle ...

On Fanuc, is it fully synchronized ? On all the controls I have owned there is a marker pulse. Threading is synchronized to that, which is why you cannot change spindle speed, but not in a continuous manner thruout the pass. Maybe on something with a C axis you could ? But most 2 axis lathes spindles don't have C axis feedback, except for the marker pulse.

They could, now that controls are more capable, but do they ?

 

[Vancbiker]

......On Fanuc, is it fully synchronized ? On all the controls I have owned there is a marker pulse. Threading is synchronized to that, which is why you cannot change spindle speed, but not in a continuous manner thruout the pass. Maybe on something with a C axis you could ? But most 2 axis lathes spindles don't have C axis feedback, except for the marker pulse.......

On Fanuc, the spindle encoder one revolution pulse is used to initiate the thread cycle. The spindle encoder is used to monitor spindle speed and feed is adjusted as needed to retain synchronous operation. Changing spindle speed within a threading cycle changes the starting point of the pass due to time lag of the one rev pulse and commencing the motion. Once in the cut, if the spindle is slowed by cutting force the feed is correspondingly adjusted.

Here are some clips from various Fanuc description and connection manuals for the 16/18 series controls regarding threading...

In general, thread cutting is repeated along the same tool path in rough
cutting through finish cutting for a screw. Since thread cutting starts when
the position coder mounted on the spindle outputs a 1–turn signal,
threading is started at a fixed point and the tool path on the workpiece is
unchanged for repeated thread cutting. Note that the spindle speed must
remain constant from rough cutting through finish cutting. If not,
incorrect thread lead will occur.

Tool movement is synchronized with spindle rotation when cutting
threads. The spindle speed is continuously read through the position coder
attached to the spindle. Then, it is converted to a cutting feedrate (feed
per minute) to feed the tool.

 

[sinha]

This won't work. He'll get a groove at the beginning of the thread, then a waggly start, then an uncontrolled straight pullout at the end. The entire pass needs to be locked in at one feedrate, synchronized to a particular spot on the circumference of the part.

That is correct. Bill also said the same thing. There will, of course, be a groove at the start of the thread because feed motion of G32 would wait for the marker pulse, while the spindle keeps rotating.
However, I cannot imagine a design consideration where a groove at the start of the thread would hurt. If a groove is permitted, it would be more convenient to first make a groove, and then use G92. The program would be much shorter if multiple passes are needed. The only problem with G92 is that it plunges with rapid rate. Let it plunge in the previously made groove.
The initial lead error would, of course, be there, but it is expected in G32 method also because the axis motor has to start suddenly.

 

[angelw]

There will, of course, be a groove at the start of the thread because feed motion of G32 would wait for the marker pulse, while the spindle keeps rotating.

Hello Sinha,
Actually no. G32 is used for Continuous Threading, where Direction and or Lead can be changed without impairing the threads.

Regards,

Bill

 

[sinha]

Hello Sinha,
Actually no. G32 is used for Continuous Threading, where Direction and or Lead can be changed without impairing the threads.

Regards,

Bill

Plunging with G01 would leave a groove. That is what I was saying. G32 is fine.

 

[EmGo]

Plunging with G01 would leave a groove. That is what I was saying. G32 is fine.

But sinha, why would you do that ? It's not only ugly, it works worse and takes at least as many blocks.

@Vanc - same as the controls I am familiar with. The spindle speed and feedrate are coordinated, but it's not a real controlled axis, like a rotary table would be.

 

[sinha]

Yes. G32 should be used for plunging. There is no good reason to use G01 for plunging.

 

[cuttergrinder]

I made a little program with g32 x, z and anther x move and it ran fine. I was just cutting air though. I was running 100 rpm and had a .866" lead programmed. We tried reving it to 300 rpm but the machine will not feed that fast.it limits out at about 230 inches per min. On the feed.