[bmlw]

Back to Basics!
I have been given a program and told to run it just like it is.
My problem is I do not recognize one of the parameters for G01.
The program was for a Yasnac control on a Mori SL1 and I will be running it on a PUMA with FANUC 15T control.

Here is the code
N5 (NPR50.5)
G51
G97T500S4500M3
G0-.02Z.05T505
G1ZoF.002
X.02
X-.376K-.024
G51
M1

What is the K-.024 for. I understand this in a drill cycle for peck depth but for linear interpolation?

Thanks
Geoff

[littlerob]

Back to Basics!
I have been given a program and told to run it just like it is.
My problem is I do not recognize one of the parameters for G01.
The program was for a Yasnac control on a Mori SL1 and I will be running it on a PUMA with FANUC 15T control.

Here is the code
N5 (NPR50.5)
G51
G97T500S4500M3
G0-.02Z.05T505
G1ZoF.002
X.02
X-.376K-.024
G51
M1

What is the K-.024 for. I understand this in a drill cycle for peck depth but for linear interpolation?

Thanks
Geoff

Geof you know the answer; sorry inside joke. Disregard

The K is an incremental command for Z- alot of that code would be accepted on a Yasnac without being in G91 mode(incremental). I don't think the 15t will buy it though, so you'll have to change it to Z- instead of K-. But it's just a chamfer, looks like .0084c with a .0156r tool.

Robert

[bmlw]

Robert,
Thanks for the quick reply.
Please enlighten me on the inside joke.

Just to clarify the chamfer,
The chamfer will start at x -.02, z 0
and end up at x.376, z-.024? Is that what you see?

Thanks
Geoff

[dcoupar]

littlerob, I beg to differ. Every Yasnac I've ever seen has used W for incremental Z, not K.

On a Yasnac, K is used for chamfering with the G11 command, but I've never seen it with G01 on a Yasnac.

Are you sure your example came from a Yasnac? It looks more like a Haas (in Yasnac mode) program with that G51 in there.

Most of the Fanucs (at least from the 6T on) will use K with a straight X and I with a straight Z feed to chamfer at the end of the line.

I don't have any early 15T manuals, but I believe it should run. Get rid of the G51's though, I know the Fanuc will fail on that.

[bmlw]

Dcoupar & Robert

Here is What my edited file looks like at the present with the exception of the K parameter for the G01

N5 (NPR50.5) *This kennametal insert has a .005r
G00T1104
G97S4500M3
G0X.02Z.05
G1Z0F.002
x-.02
X.376 (WHAT THE HECK DO I DO WITH THIS K-.024?)
T1100
M1

Geoff

[bmlw]

Dcoupar,
I have seen the Mori SL1 and the owner is the original owner. He states the control is Yasnac. Me, I just have to make it work on my FANUC 15T.

Geoff

[dcoupar]

Dcoupar & Robert

Here is What my edited file looks like at the present with the exception of the K parameter for the G01

N5 (NPR50.5) *This kennametal insert has a .005r
G00T1104
G97S4500M3
G0X.02Z.05
G1Z0F.002
x-.02
X.376 (WHAT THE HECK DO I DO WITH THIS K-.024?)
T1100
M1

Geoff

Put the K-0.024 back in with the X.376. But I believe you'll have to do a Z- move in the block following to make it work.

X.376 K-.024
Z-.03 (IIRC this must be > than the K value).

[bmlw]

Dave and Robert,

The mentioning of the chamfer sent me to page 188 of my operators manual under Chamfering and Corner R.
It lists the comand format as G01XbK+/-k; Specifies movement to point b with an absolute or incremental comand.

Therefore I beleive the correct line for my program should read
G01Z0F.002
X-.02
X.376K-.024 which will give me a 45deg chamfer starting at X.352,Z0 and ending up at X.376,Z-.024.

Regards
Geoff

[angelw]

Dcoupar & Robert

Here is What my edited file looks like at the present with the exception of the K parameter for the G01

N5 (NPR50.5) *This kennametal insert has a .005r
G00T1104
G97S4500M3
G0X.02Z.05
G1Z0F.002
x-.02
X.376 (WHAT THE HECK DO I DO WITH THIS K-.024?)
T1100
M1

Geoff

Geoff,

The K is to machine a chamfer when used in conjunction with G01.

With a Fanuc control the next block must be a movement along the axis perpendicular to the axis containing the K.

The code that you have now could be a bit risky to use, because without seeing the code that may precede the code you've posted, there is no movement to a tool change position. The G51 in your first sample program was to cancel the tool offset and return home. Accordingly, with a Fanuc control I would modify the program to something like this:

Regards,

Bill

N5 (NPR50.5) *This kennametal insert has a .005r
G28 U0.0 W0.0
G00T1104
G97S4500M3
G0X.02Z.05
G1Z0F.002
X-.02
X.376 K-.024
Z-0.025 (WITHOUT A Z MOVE AFTER THE CHAMFER BLOCK, THE CONTROL WILL ALARM)
G28 U0.0 W0.0
M1

Alternatively, the last part of the program could be written as follows:
X-0.020
X0.328
X0.376 Z-0.024
G28 U0 W0
M01

[littlerob]

I was wrong, Dcoupar is right about the coding. K for chamfer with G11 only.

The inside joke is a member here on The Zone, who is really an authority on coding. With a very similar name to yours.

But now I'm looking at post 3 and the answer is no, it will not leave a 45 chamfer. The tool starts at X-.02 and ends at X.376 with an (assumed) -Z movement of .024. Friends that's a tapered face not a chamfer!! It's all my fault (chair). I agree with all posts (except mine), and the alternate toolpath that Bill posted is the easiest and correct. IF you want a 45 degree chamfer that will measure about .008. Don't forget to add the line X.328 line before the chamfer.

Robert

[stevo1]

I have an old 12t out on the floor which is still using G50’s. They have used the K values for chamfering in the past but IIRC the operator once told me it was related to using cutter comp.

Now I do know on the Fanucs that U is for incremental X and W is incremental Z so if you need to make a chamfer in incremental mode then use U and W. I also agree with Dave and Angel that you should remove the G51 as I don’t see this listed in any of my Fanuc lathe G-codes. I only see it on my machining centers as “scaling”.

Stevo

[bmlw]

Hi to you all,
Thanks for the input.
I have modified the program as follows to include a Z move to clear the material for a tool change as follows

N5 (NPR50.5) *This kennametal insert has a .005r
G00T1104
G97S4500M3
G0X.02Z.05
G1Z0F.002
x-.02
X.376K-.024
Z2.0
T1100
M1

Thanks
Geoff

[littlerob]

I have an old 12t out on the floor which is still using G50’s. They have used the K values for chamfering in the past but IIRC the operator once told me it was related to using cutter comp.

Now I do know on the Fanucs that U is for incremental X and W is incremental Z so if you need to make a chamfer in incremental mode then use U and W. I also agree with Dave and Angel that you should remove the G51 as I don’t see this listed in any of my Fanuc lathe G-codes. I only see it on my machining centers as “scaling”.

Stevo

@ Stevo; G50 is a max spindle speed command, I recomend you keep using that.:cheers:

As far as the U,W,I,K go, the "U" and "W" are NOT incremental commands. They are representative of those axes. "I" and "K" are incremental. So the answer is no you would not use U or W in order to generate a chamfer.

[littlerob]

Hi to you all,
Thanks for the input.
I have modified the program as follows to include a Z move to clear the material for a tool change as follows

N5 (NPR50.5) *This kennametal insert has a .005r
G00T1104
G97S4500M3
G0X.02Z.05
G1Z0F.002
x-.02
---You will need X.328 here, IF you want the chamfer.
X.376K-.024
Z2.0
---here you are going to want the G28 U0 W0 line that Bill inserted
T1100
M1

Thanks
Geoff

Sorry Geoff I was posting at the same time.

[angelw]

@ Stevo; G50 is a max spindle speed command, I recomend you keep using that.:cheers:

As far as the U,W,I,K go, the "U" and "W" are NOT incremental commands. They are representative of those axes. "I" and "K" are incremental. So the answer is no you would not use U or W in order to generate a chamfer.

Actually, on a Fanuc Lathe Control, G50 has two uses.
1. As you stated to limit the max RPM when in Constant Surface Speed Mode, G96. Example G50 S3000, would limit the spindle speed to 3000 RPM. I note that the program uses the set spindle speed mode G97. Accordingly, G50 as a speed limiter would be not be required in this case.

2. As a Coordinate Set command, similar to the same way G92 on a Fanuc Mill Control is used. G50s to Set the Coordinate System was available as the only option up to the end of the 6 series controls. Example G50 X8.0000 Z10.0000, would tell the Control that the tool tip is at the distances set in the G50 line from the work X Z zero, from the position the G50 was commanded. If the control has Geometry Offset Programming available, then this is by far the safer option.

U and W are in fact incremental commands. The Mill Control uses G90 and G91 to select absolute and incremental mode respectively, but the Lathe Control uses X and Z for absolute and U and W for incremental. You can mix absolute and incremental moves on the same line. Example X0.500 W-0.100

Stevo Wrote
Now I do know on the Fanucs that U is for incremental X and W is incremental Z so if you need to make a chamfer in incremental mode then use U and W

You can only use U and W to machine a chamfer in incremental mode if the tool is parked at the start of the chamfer, as in the alternate program method I suggested. Using the K will automatically start the chamfer when the tool reaches the X coordinate of the X commanded 0.376 - 2x0.024 using the focus program of this thread as the example.

Regards,

Bill

[dcoupar]

@ Stevo; G50 is a max spindle speed command, I recomend you keep using that.:cheers:

As far as the U,W,I,K go, the "U" and "W" are NOT incremental commands. They are representative of those axes. "I" and "K" are incremental. So the answer is no you would not use U or W in order to generate a chamfer.

littlerob,

Where are you getting your information?

On Fanuc, Yasnac, and Haas controls (among others), U and W are used for incremental X and Z. And yes, you can use U and W to create a chamfer. You can even mix X and W, or Z and U in the same block.

I and K are incremental when used in a G02 or G03 or when used in a chamfering/corner rounding block.

And Geoff, I stand corrected. Apparently starting with the Yasnac LX-1 series you CAN program a chamfer or round with G01 in addition to using G11/G12. I was looking at the 2000G manual when I said that you couldn't chamfer or round with G01 as you could on a Fanuc.

Also with the LX-1 G51 was offered as an option. You learn something new every day.

[stevo1]

You can only use U and W to machine a chamfer in incremental mode if the tool is parked at the start of the chamfer, as in the alternate program method I suggested. Using the K will automatically start the chamfer when the tool reaches the X coordinate of the X commanded 0.376 - 2x0.024 using the focus program of this thread as the example.

Thanks for the info Bill. I have only seen the K a few times and never really questioned it. Nice to know. I also do know that the U and W are incremental from the current position that the tool is at. Use it all the time

On Fanuc, Yasnac, and Haas controls (among others), U and W are used for incremental X and Z. And yes, you can use U and W to create a chamfer. You can even mix X and W, or Z and U in the same block.

Thank god I thought that I was using the wrong code for all these years and no chamfer was ever created.

A bit OT. How do you break a guy who is set on G50 when the machine has offset memoryC, workcoordinates and he is a few years away from retirement? Don't get me wrong I am not looking forward to the task of modifying/cleaning all the G50's out of the programs but I am nearing the end of setting up the 25million dollar product line and I have saved this task for last. Suggestions are welcome.

Stevo

[littlerob]

OWNED humbly zowned

Robert

[g-codeguy]

A bit OT. How do you break a guy who is set on G50 when the machine has offset memoryC, workcoordinates and he is a few years away from retirement? Don't get me wrong I am not looking forward to the task of modifying/cleaning all the G50's out of the programs but I am nearing the end of setting up the 25million dollar product line and I have saved this task for last. Suggestions are welcome.

Stevo

Bad news Stevo. You don't. Us old farts can't be taught new tricks. Surely a smart man like you is aware of this! Well...I can be taught something new......occasionally, but that is because I have a young man's outlook in an old man's body. No idea how I got to be this old. Seems impossible. And unfair.

Now that I've reached a point where I can talk to the opposite sex without turning red, they won't look at me. Oops! Maybe a little too far off topic. That's another problem with us old farts. We forget what the subject was about.

[Geof]

.....The inside joke is a member here on The Zone, who is really an authority on coding. With a very similar name to yours....
Robert

Only on Haas.

I saw: 'Yasnac', 'Mori SL1', 'PUMA' and 'FANUC', realised I was out of my depth and closed the thread (until now).

g-codeguy; the alternative to growing old is much more unfair than growing old, especially when you still feel young.