Thread: Need help with radius grooving.

Originally Posted by angelw

Hello Sinha,
Absolutely, but with a whole lot more Feed/Rev. 0.2mm/rev is conservative roughing feed rate with a 0.8 TNR and a much greater DOC.

I took over 30 minutes out of a client's 60 min. cycle time on a large, deep face groove using a 12 diameter button tool, using 0.5 DOC and 3.0mm feed/rev to bi-directional face. Basically, its the same principle as HSM common to Machining Centres, implemented on a Turning Centre. I've also used the same technique in OD turning operations.

The slow feed rate you suggested would result in bird nest swarf.

It would be difficult to use with a Multi-repetitive cycle, as the indeed for the DOC can't be anything near like the feed/rev used in a Turning, or Facing operation (only one Feed Rate can be specified in these Roughing Cycles)

Regards,

Bill

Hello Bill,

Thank you for information.
If button inserts can be satisfactorily used for turning, then I think one should first experiment with G71 type 2 which would be the simplest method. If radius compensation is not available within the cycle, the offset curve can be used.

Originally Posted by sinha

Hello Bill,

Thank you for information.
If button inserts can be satisfactorily used for turning, then I think one should first experiment with G71 type 2 which would be the simplest method. If radius compensation is not available within the cycle, the offset curve can be used.

Hello Sinha,
As mentioned in my previous Post, Swarf control is going to be an issue with the relatively fine feed you would be forced to use with a G71 cycle. Following is the code for your 0.5 DOC using a 3.0 Radius Button Tool. The 1.0 Feed/Rev would be a starting feed. F2.0 will probably be closer to the mark with a 3.0 Rad tool.

I think Rob said he would be inclined to program it without using a cycle. I'm thinking he would use some thing like the following code. If a cycle were to be used to rough the profile, I think the G75 he originally suggested would be the choice, as it affords a method of swarf control.

Regards,

Bill

(3.0 RAD OD BUTTON TOOL)
(ROUGHING CUTS STARTS HERE)
G00 X112.000 Z-10.044
G02 X109.500 Z-9.062 I-2.939 K-2.456 F0.15
G01 Z-15.938 F1.0
G03 X108.500 Z-16.141 I-1.689 K3.438 F0.15
G01 Z-8.859 F1.0
G02 X107.500 Z-8.732 I-1.189 K-3.641 F0.15
G01 Z-16.268 F1.0
G03 X106.500 Z-16.325 I-0.689 K3.768 F0.15
G01 Z-8.675 F1.0
G02 X105.500 Z-8.683 I-0.189 K-3.825 F0.15
G01 Z-16.317 F1.0
G03 X104.500 Z-16.243 I0.311 K3.817 F0.15
G01 Z-8.757 F1.0
G02 X103.500 Z-8.901 I0.811 K-3.743 F0.15
G01 Z-16.099 F1.0
G03 X102.500 Z-15.875 I1.311 K3.599 F0.15
G01 Z-9.125 F1.0
G02 X101.500 Z-9.446 I1.811 K-3.375 F0.15
G01 Z-15.554 F1.0
G03 X100.500 Z-15.101 I2.311 K3.054 F0.15
G01 Z-9.899 F1.0
G02 X99.500 Z-10.575 I2.811 K-2.601 F0.15
G01 Z-14.425 F1.0
G03 Z-10.575 I3.311 K1.925 F0.15
(FINISH CUT STARTS HERE)
G00 X112.000 Z-9.500
G01 Z-8.420 F1.0
G01 X106.123 F0.25
G02 Z-16.580 I0.000 K-4.080
G01 X112.000

Originally Posted by angelw

Hello Sinha,
As mentioned in my previous Post, Swarf control is going to be an issue with the relatively fine feed you would be forced to use with a G71 cycle. Following is the code for your 0.5 DOC using a 3.0 Radius Button Tool. The 1.0 Feed/Rev would be a starting feed. F2.0 will probably be closer to the mark with a 3.0 Rad tool.

I think Rob said he would be inclined to program it without using a cycle. I'm thinking he would use some thing like the following code. If a cycle were to be used to rough the profile, I think the G75 he originally suggested would be the choice, as it affords a method of swarf control.

Regards,

Bill

(3.0 RAD OD BUTTON TOOL)
(ROUGHING CUTS STARTS HERE)
G00 X112.000 Z-10.044
G02 X109.500 Z-9.062 I-2.939 K-2.456 F0.15
G01 Z-15.938 F1.0
G03 X108.500 Z-16.141 I-1.689 K3.438 F0.15
G01 Z-8.859 F1.0
G02 X107.500 Z-8.732 I-1.189 K-3.641 F0.15
G01 Z-16.268 F1.0
G03 X106.500 Z-16.325 I-0.689 K3.768 F0.15
G01 Z-8.675 F1.0
G02 X105.500 Z-8.683 I-0.189 K-3.825 F0.15
G01 Z-16.317 F1.0
G03 X104.500 Z-16.243 I0.311 K3.817 F0.15
G01 Z-8.757 F1.0
G02 X103.500 Z-8.901 I0.811 K-3.743 F0.15
G01 Z-16.099 F1.0
G03 X102.500 Z-15.875 I1.311 K3.599 F0.15
G01 Z-9.125 F1.0
G02 X101.500 Z-9.446 I1.811 K-3.375 F0.15
G01 Z-15.554 F1.0
G03 X100.500 Z-15.101 I2.311 K3.054 F0.15
G01 Z-9.899 F1.0
G02 X99.500 Z-10.575 I2.811 K-2.601 F0.15
G01 Z-14.425 F1.0
G03 Z-10.575 I3.311 K1.925 F0.15
(FINISH CUT STARTS HERE)
G00 X112.000 Z-9.500
G01 Z-8.420 F1.0
G01 X106.123 F0.25
G02 Z-16.580 I0.000 K-4.080
G01 X112.000

Thank you Bill. If possible, please post the toolpath also.

Sheesh Bill, not quite that in depth. As Lynard Skynard said, "I'm a simple kind of man".

More like
G0 Z-
G1 X
G0 X
Z-
G1 X
G0 X
Z-
etc.
etc.
Then Finish pass.

R

Lynard Skynard is a person BTW.

Originally Posted by sinha

Thank you Bill. If possible, please post the toolpath also.

Hello Sinha,
Following is picture of tool path.

Regards,

Bill

Originally Posted by litlerob1

Sheesh Bill, not quite that in depth. As Lynard Skynard said, "I'm a simple kind of man".

More like
G0 Z-
G1 X
G0 X
Z-
G1 X
G0 X
Z-
etc.
etc.
Then Finish pass.

R

Lynard Skynard is a person BTW.

Hello Rob,
I was answering Sinha's question and his suggested 0.5 DOC. With a small DOC you can use a lot of Feed Rate, in the same manner as HSM with a Machining Centre. The OP's job is not the perfect example for this technique, but with a much larger groove, its hard to beat in terms of cycle time. As mentioned in my earlier Post, I've used 12 diameter Button Inserts at 0.5mm DOC and 3.0mm Feed/Rev. You can't use that type of Feed Rate with a hefty DOC and you will get Zero Chip Control with a Feed Rate commensurate with a considerable DOC.

Regards,

Bill

Originally Posted by angelw

Hello Sinha,
Following is picture of tool path.

Regards,

Bill

Hello Bill,

I believe you CAMed it and later edited the feedrates?

Originally Posted by sinha

Hello Bill,

I believe you CAMed it and later edited the feedrates?

Why would that matter? I mean we've basically derailed the OP's thread, but why would the manner of determining feedrate make any difference?

R

Originally Posted by litlerob1

Why would that matter? I mean we've basically derailed the OP's thread, but why would the manner of determining feedrate make any difference?

R

He can try Bill's program.

Originally Posted by angelw

Hands up all those that have taken an inch wide plunge cut in other than plastic, on your typical sized Turning Centre found in most machine shops, not built like a Brick Shit House (typical of a Kia SKT 200), and could still hear the radio over the chatter.

I've done 3/4" face grooves that way. Not my first choice but because I didn't want to spend a bundle on holders for two parts. Worked okay. No chatter.

Machine was previous generation tho, box ways and pretty stout. American Tool.

Based on Bill's experience, I think Fanuc should modify the roughing cycles to include two feedrates, one for plunging and the other for turning.

Originally Posted by EmanuelGoldstein

I've done 3/4" face grooves that way. Not my first choice but because I didn't want to spend a bundle on holders for two parts. Worked okay. No chatter.

Machine was previous generation tho, box ways and pretty stout. American Tool.

You're not masquerading for Johnny Larue by any chance?

Originally Posted by angelw

You're not masquerading for Johnny Larue by any chance?

I think he's masquerading for Monochrist.

Originally Posted by angelw

You're not masquerading for Johnny Larue by any chance?

Had to look it up

Nah, I just like beefy lathes. Machining centers I can see taking tiny cuts and zipping around but a lathe oughta have some balls.

Originally Posted by EmanuelGoldstein

Had to look it up

Nah, I just like beefy lathes. Machining centers I can see taking tiny cuts and zipping around but a lathe oughta have some balls.

Yeah, you're Johnny Larue alright; or his clone.

Originally Posted by angelw

Hands up all those that have taken an inch wide plunge cut in other than plastic, on your typical sized Turning Centre found in most machine shops, not built like a Brick Shit House (typical of a Kia SKT 200), and could still hear the radio over the chatter.

The groove is only .5518 inches wide at it's max.
Perhaps you math is off and/or you need a better tooling supplier who can handle such with the needed low cutting force and no chatter.

For sure catalog standard tools need not apply for this type work.
The singing, dancing and waiting forever is best often for such and for sure this is the best and most profitable way in small runs.
The thing is that with the cnc age some people forget or have never seen another way. This will maybe just be lost as "old school" or never tried.
Perhaps it can only be done fast with "big iron" so we settle for longer cycles as we buy smaller machines. That is great if your dollar per hour paid to employees or shop owner is held low
Bob

Originally Posted by CarbideBob

The groove is only .5518 inches wide at it's max.
Perhaps you math is off

My math is just fine. The contact with a 7.08 rad form tool, with the profile being discussed, is through 162.757deg. Unwrap that and its 20.1117 (0.7918").

And with regards to Goldstein's example 3/4" wide face groove with a similar width tool, the effective DOC with a face groove is tantamount to a conventional turning OP simply applied inboard of the work-piece OD. Unless the tool is profoundly positive rake and minuscule feed rate used (kind of defeats the purpose in production), that's not going to happen with the OP's machine and those similar.

I give up and bow to your many decades of tool design, experience and application.
I just try out here on the fringe as a rookie and for sure do not know it all.
After only 45 years of doing it I'd like to think I've gained some knowledge but I do get proved wrong often.
Not afraid to say that I'm wrong or that my concept won't work so I tap out and you win.
We have no need to argue.......I find all your post to be spot on in the cnc world and much respect given from this side for all of your contributions to the board.
You know things about how these machine controls work in different versions or rev levels that is amazing.
Bob

But I like it when the wise argue. That's some real edumukasun.

R

Originally Posted by litlerob1

Lynard Skynard is a person BTW.

I'll be damn! I've listened to this band my entire life and I did not know this. Apparently Skinner gave some members of the band shit over their long hair in high school which is what started the whole thing off.

"Leonard Skinner (January 11, 1933 – September 20, 2010) was an American high school gym teacher, basketball coach, and businessman from Jacksonville, Florida. He is known in popular culture as the namesake of the Southern rock band Lynyrd Skynyrd."

Brent