Broaching/keying with a lathe?

Cuda · Jul 18, 2021

I have to cut a coolant groove .375IN. X .187 DEEP 8" deep in the bore of a part, I have a single point high speed tool bit to cut the key with but what is the trick to get the machine to move in a feed mode without the spindle turning????
I tried G98 with a G1 feed command but got no movement.

Is there a canned cycle that works good for keying?

Also, there are 2 grooves 180 apart, is there a code that will rotate and lock the spindle 180 deg. from the first groove? The machine is a 2006 Doosan Puma 400 with Fanuc 21i control. Thanks

Dan from Oakland · Jul 18, 2021

Are you programming G94(inches/minute) or G95(inches per revolution). If your spindle is not turning and you program G95, your tool is not going anywhere.

angelw · Jul 19, 2021

Dan from Oakland said:
Are you programming G94(inches/minute) or G95(inches per revolution). If your spindle is not turning and you program G95, your tool is not going anywhere.

Hello Dan,
Its a lathe and if the Fanuc default parameter setting for the G Code System is set (most likely), then G98 is correct for Feed/Minute.

@Cuda
Although you may be using Feed/Minute, it doesn't necessarily mean that the Spindle can be stopped. I've seen many examples where Feed won't occur with the spindle stopped, irrespective of whether Feed/Minute mode was selected. It will be a Keep Replay setting and up to the MTB as to which one is used. Accordingly, you will have to consult the manuals that came with the machine. Normally there will be a manual that has a hard copy of the PLC Ladder included. Specification of the various I/O, Timer/Counters and Keep Relays used is usually included in that.

However, even with a HSS cutting tool, its highly likely that the Z Rapid Speed will be below the Surface Speed for the material you're cutting. Therefore, you can cut the slot using Rapid. You should be able to move the axes in Rapid with the Spindle stopped.

Regards,

Bill

EmGo · Jul 19, 2021

You could try an M03 or M04 S0 along with the other commands .... not much chance it'll work but easy to try and can't hurt. If the control only checks for direction and speed commands, not that there's tach feedback, there's a slight chance. Quickturn doesn't, kind of shocked me.

Unless you have a C axis tho, you're not going to be doin' no 180*.

Scruffy887 · Jul 19, 2021

Z axis feed may not like being used as a shaper. Likely to alarm out.

Cuda · Jul 19, 2021

angelw said:
@Cuda
Normally there will be a manual that has a hard copy of the PLC Ladder included. Specification of the various I/O, Timer/Counters and Keep Relays used is usually included in that.

However, even with a HSS cutting tool, its highly likely that the Z Rapid Speed will be below the Surface Speed for the material you're cutting. Therefore, you can cut the slot using Rapid. You should be able to move the axes in Rapid with the Spindle stopped.

Regards,

Bill

Thanks bill, we do have all the books but I don't know how to read all the ladders and stuff,
as far as programming in rapid I think I can adjust the speed some in the parameters.

Any thoughts on indexing the groove 180 deg. away from the 1st without indexing the part it's self?
I have quite a few parts to do and would hate to index each one manually.
I have used a Q in G76 thread cycle to cut multiple lead threads where Q tells the angle 0-360,
but not sure to to use it without threading???

EmGo · Jul 19, 2021

Cuda said:
I have used a Q in G76 thread cycle to cut multiple lead threads where Q tells the angle 0-360,
but not sure to to use it without threading???

All that does is move the start ;point of the threading pass. There's only one trigger on the spindle for two-axis lathes. There's no way to know where it is rotationally.

In short, you can't.

You could make an indexing fixture to hold them, but since you don't even know if the lathe can be used as a slotter, probably getting ahead of yourself at this point.

Probably easier to do in the Bridgeport. You won't have to go to the gym that week, at least for the right arm

Cuda · Jul 19, 2021

EmanuelGoldstein said:
All that does is move the start ;point of the threading pass. There's only one trigger on the spindle for two-axis lathes. There's no way to know where it is rotationally.

Probably easier to do in the Bridgeport. You won't have to go to the gym that week, at least for the right arm

#1...Yes you CAN start threads by degrees in some 2 axis lathes, I've done 8 start oil control spirals starting and stopping in a .25 wide groove using G76 cycle with this machine.

#2... This is the only machine the BOSS wants it done in!

EmGo · Jul 19, 2021

Cuda said:
#1...Yes you CAN start threads by degrees in some 2 axis lathes, I've done 8 start oil control spirals starting and stopping in a .25 wide groove using G76 cycle with this machine.

Then just tell it this is a 2 start infinite lead thread and you're all done !

colton_m · Jul 19, 2021

Cuda said:
Also, there are 2 grooves 180 apart, is there a code that will rotate and lock the spindle 180 deg. from the first groove? The machine is a 2006 Doosan Puma 400 with Fanuc 21i control. Thanks

I have used spindle orientation with an S value to accomplish this.
Sxxxx is your angle times 10.

The machine wasn't set to work this way by default, I had to do the following from the operation manual: K8.1 = "0" and NO.3702#2 = "1".
That allows the S code to work on the M19 line.

Example (machining at 0 and 180 degrees):
M19S0
<machining code>
M19S1800
<machining code>

Good luck!

angelw · Jul 19, 2021

Cuda said:
Thanks bill, we do have all the books but I don't know how to read all the ladders and stuff,
as far as programming in rapid I think I can adjust the speed some in the parameters.

Any thoughts on indexing the groove 180 deg. away from the 1st without indexing the part it's self?
I have quite a few parts to do and would hate to index each one manually.
I have used a Q in G76 thread cycle to cut multiple lead threads where Q tells the angle 0-360,
but not sure to to use it without threading???

Hello Cuda,
Although not chiseled in rock, a generic method to determine if a two axis lathe not having a true "C" axis, has Rigid Tapping is to see if the the machine responds to M19 to orientate the spindle. Conversely, if you know that your lathe has Rigid Tapping, its likely that it will have spindle orientation with M19.

If your machine does have Spindle Orientation with M19, there is a good chance that you will be able to change the Orientation position using colton_m's method using an "S" address with M19. Not all machines have this ability, even when M19 is available; its up to MTB if this process is implemented or not. If the machine does have M19, but doesn't respond to an "S" address to change the Orientation position, the Orientation position can be changed via parameter and this can be done grammatically on the fly using G10.

Regards,

Bill

chad883 · Jul 20, 2021

Cuda said:
Thanks bill, we do have all the books but I don't know how to read all the ladders and stuff,
as far as programming in rapid I think I can adjust the speed some in the parameters.

Any thoughts on indexing the groove 180 deg. away from the 1st without indexing the part it's self?
I have quite a few parts to do and would hate to index each one manually.
I have used a Q in G76 thread cycle to cut multiple lead threads where Q tells the angle 0-360,
but not sure to to use it without threading???

You could always put in 2 broach tools, 1 for X+ and 1 for X-

EmGo · Jul 20, 2021

chad883 said:
You could always put in 2 broach tools, 1 for X+ and 1 for X-

Much more practical than trying to index ... good idea !

DouglasJRizzo · Jul 21, 2021

Cuda said:
I have to cut a coolant groove .375IN. X .187 DEEP 8" deep in the bore of a part, I have a single point high speed tool bit to cut the key with but what is the trick to get the machine to move in a feed mode without the spindle turning????
I tried G98 with a G1 feed command but got no movement.

Is there a canned cycle that works good for keying?

Also, there are 2 grooves 180 apart, is there a code that will rotate and lock the spindle 180 deg. from the first groove? The machine is a 2006 Doosan Puma 400 with Fanuc 21i control. Thanks

With Doosan you may need to input say a M184 to feed with spindle off, and M185 to put it back. Check your M code list.

MotoX · Jul 21, 2021

This is the bit of code I used last time. Its been awhile so I don't remember specifics. All I remember is that it was a slow process and I was cutting a 5/8 wide keyway in a through hole.

O9926(BROACH KEY)
G28U0W0
T0909
G98
M19
M8
G00X2.815Z.5
G71U.001R.3
G71P1Q2U0.0W0.0F220.
N1G00X3.582
N2G01Z-3.375
G28U0W0
M30
%

Search

Largest Manufacturing Technology Community on the Web

Search

Broaching/keying with a lathe?

Cuda

Hot Rolled

Dan from Oakland

Titanium

angelw

Diamond

EmGo

Diamond

Scruffy887

Titanium

Cuda

Hot Rolled

EmGo

Diamond

Cuda

Hot Rolled

EmGo

Diamond

colton_m

Aluminum

angelw

Diamond

chad883

Cast Iron

EmGo

Diamond

DouglasJRizzo

Titanium

MotoX

Cast Iron

Similar threads