CNC programing

[Fryzss]

Can I create a batch file in G code to have y axis = c axis? Or is this software dependent? I'm trying to manual code, no other software being used right now.
Thanks,
Jeff

[Ottmar-Petry]

Hi.
You only want to change all Y-coordinates to C-coordinates ?
Then you can use any kind of text-editor to do this modification by replace-command.
But I think that you need to do something different, or ?

Ottmar

[Paulo E.]

As long as your mindfull of changing the necessary codes to enable the C axis you should be golden if you just change the "Y" to "C". Out of curiosity what machine are you doing this for ???? only reason I ask is that certain machines you dont even need to change the "Y" value such as Haas lathes.

[rgm]

Is this a "C" Axis on a Lathe or Mill?

RGM

[cnc_ken]

Sounds as if you want to translate yaxis to rotary over a known diameter.
If you have variables and math functions you can make a G code program.
What you need to know is the circumference of the part. Then multiply
360 * [Y/Circumference]. That will give you the Angle that Y plots out along the circumference of your part. Did a few of those in the early 80's before CAD was readily available.

[Fryzss]

I am helping an older guy (I'm 57!) who purchased a Servo ll Impact milling machine over 10 years ago. He has a 4 axis setup that he wants to drill .0625 holes on a 1" diameter by 1-1/2" long cylinder. I need to figure out the spacing so as not to collapse the edge or adjoining holes.
He's thinking in terms of spacing using threads per inch (lathe guy?) and I was an architectural type of guy so our getting to the same point is much different.
The reason for the question was if we were to try another software program that might be limited to 3 axis. I was wondering if I could state Y axis is = C axis. Heck I was always proud of the fact that our projects seemed to always fit
like a large puzzle and always produced what we wanted. Now playing with what seems to be a maze of micro puzzles I can't give enough praise to you machinist. I believe I'm starting to understand the basics of code but man Autocad was easy compared to this. I might be more comfortable with a simple cad-cam program to get up to speed. It would also help if I were a machinist to understand the process!
Thanks for the imput, anymore will be appreciated,

Jeff

[cnc_ken]

Here's an attached DXF and NC file. See if it's something you can use, but remember, try it at your own risk!!

[Billet Boyz]

You coulsd also program it by hand like this and save lots of memory....

O0000 (PATTERN)
N100 G00 G17 G20 G40 G49 G80 G90
N102 T2 M06 (UNDEFINED)
N104 G00 G90 G54 X-.0469 Y0. C0. S2139 M03
N106 G43 H3 Z.6
N108 G99 G81 Z.49 R.6 F4.11
N110 G91 C9. L39 (RUN CANNED CYCLE AT 9 DEG INC 39 MORE TIMES)
N112 G90 X-.125 C4.5
N114 G91 C9. L39
N116 G90 X-.2031 C0.
N118 G91 C9. L39
ETC
THIS WILL ONLY WORK IF YOUR MACHINE IS SET UP TO READ L COMMANDS

[Fryzss]

Thanks for all your responses to this question. I'm going to work with each of your suggestions in order to better understand each approach. It looks like defining the tool and feedrate and adding my z axis should get me started. My grandfather was a machinist in southern California and I got some exposure to it there as a teenager. I hope this guy I'm helping can provide this information.
I may have to get a combo lathe milling machine just to play with. I already fab and repair as much as I can now at home.
Thanks again,
Jeff