Need Help!- G01 Parameters

[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]

Originally Posted by 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

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]

Originally Posted by 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

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]

Originally Posted by 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

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 . 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