Re: [CAD_CAM_EDM_DRO] G code Examples (Was RE: Cutviewer program - file renaming

John Murphy wrote:

> I'm trying to first understand how
> the different codes are working (before I let a tool do
> everything) and trying to understand what operational methods people
> typically employ (locating origins, incremental versus absolute
> positions, etc.)

I wrote up some directions for a guy several years ago, but be
forewarned that they reference xemc rather than tkemc, and they also
reflect some specifics of how his desktop environment was set up, so
there might be some differences:

*****
CNC Machine Operation Procedures:

1. Turn POWER ON and wait for the PC to boot up.

Computer Says: You Type:

Mill login: root<Enter>
Password:
<your_password><Enter>

2. The EMC program, which controls the mill, will start up. To get the
mill out of E-STOP and homed you need to:
a. Make sure the red E-STOP switch is pulled out.
b. Press the F1 key (Gets you out of E-STOP)
c. Press the F2 key (Causes the machine to start keeping position)
d. Select (manual) mode & incremental (continuous)
e. Jog each axis in turn to a point near their home position and then
press the Home key to cause the selected axis to go to its home position.

3. Setting Axis Offsets
a. Using an edge finder (.200" diameter) spin off the edge of the part
in the X or Y-axis.
b. Set increments to .100", and jog the Z-axis up so that the edge
finder clears the top of the part.
c. Jog the axis you are working on .100" towards the edge finder so that
the centerline of the edge finder is over the edge of the part.
d. Point at the axis position readout with the mouse and right-click. A
small window will come up. Hit <Enter> at this point to zero the axis
readout.
e. Repeat the procedure for the other axis (X or Y).

4. Setting Tool Offsets (the z-zero)
a. Insert the longest tool and set the knee to allow approximately 1/2"
of clearance over the top of the part with the quill fully retracted.
b. Then insert the shortest tool, jog over the part and jog down
incrementally in the Z-axis until the tool just touches the top of a
1/4" (.250") block.
c. Point at the Z-axis position readout with the mouse and right-click.
A small window will come up. Hit <Enter> to zero the Z-axis readout.
d. Press <Alt> & T simultaneously to bring up the tool setting window.
e. Change the tool number on the first line of the window to the number
of the tool in the spindle. Press <Enter> to close the window.
f. Repeat steps b, d, and e (skip c!) for all the other tools.
g. When all the tool lengths are set take the tool out of the spindle
and jog the Z-axis to -.250.
h. Point at the Z-axis position readout with the mouse and right-click.
A small window will come up. Hit <Enter> to zero the Z-axis readout.

Note: To view the tool offsets select View from the top menu bar and
then select Tools... from the drop down menu.

5. At this point you can load a program and run it (assuming the work
offsets and tool offsets have already been established).
a. Select Auto mode from the Mode block near the upper left hand corner
of the screen.
b. Select File from the top menu bar and then select [O]Open... from the
drop down menu.
c. A window will pop up in the middle of the screen with the prompt Program
Name: /root/Desktop/Programs/
d. Type the program filename after the last / in the window and press
<Enter> to open the file.

6. To run the program, press the Run Button. The program will run up to
the first tool change at which point it will pause waiting for the tool
to be loaded into the spindle.

7. Once the tool is in the spindle press the Resume button to resume
cutting the part.

8. While running a program you can:
a. Press the Pause button to suspend the program and put the machine in
"Feed Hold".
b. When paused you can press the Step button to execute one block at a time.
c. Pressing the Resume button will resume running the program.

9. To start a program in the middle:
a. While in Auto mode select File from the top menu bar and then select
[E]Edit... from the drop down menu.
b. A window will pop up in the middle of the screen with the prompt Program
Name: /root/Desktop/Programs/
c. Type the program filename after the last / in the window and press
<Enter> to open the file.
d. Scroll down through the program and click on the line in the program
you want to start on. If you want to re-run a tool I would suggest you
start on the line that says "NnnnG53G0Z0" just before the program
changes to the tool you want.
e. Press the Set Run Mark button at the bottom of the editing window.
f. A small window will pop up to confirm the line you have selected.
Press the OK button in that small window to acknowledge the message.
g. Press the Close button to close the edit window. Pressing the Run
button will cause the program to start at the marked line. It may take a
few moments for the control to read through the file and set up all the
modal operators.
CAUTION: THE MACHINE WILL START WITH A RAPID MOVE FROM THE PRESENT
POSITION TO THE POSITION THE MACHINE WOULD BE AT HAD THE PROGRAM BEEN
RUN FROM THE BEGINNING! ENSURE THAT THE QUILL IS RETRACTED AND THAT
THERE IS PLENTY OF CLEARANCE AROUND FIXTURES, VISES, ETC... TO MAKE THIS
MOVE BEFORE PRESSING THE RUN BUTTON!

10. When done for the day shut down the machine by:
a. Select File from the top menu bar and then select [End]Quit from the
drop down menu.
b. A small window will pop up to confirm that you really want to quit.
Press the Quit button in that window to quit the EMC program.
c. Press the K button in the lower left hand corner of the screen and
select Logout from the pop up menu.
d. A window will pop up confirming that you wish to logout. Press the
Logout button in that window to finish logging out.
e. At the text (shell) prompt type shutdown -h now<Return> and wait for
the system to print out System Halted on the screen before turning off
the power.

How to Set Work Offsets on the EMC Control

There are 9 work offsets that can be used to shift the origin point of
the coordinate system which all axis motion commands use as a position
reference:
Offset
Command
P Value for G10
---------------------------------------
Machine
G53
Can't be offset
1
G54
1
2
G55
2
3
G56
3
4
G57
4
5
G58
5
6
G59
6
7
G59.1
7
8
G59.2
8

The G54 offset is the default offset which is in effect when the machine
is powered up. G54 through G59.2 are modal, which means that once
invoked they stay in effect until another offset is commanded. G53 is
non-modal and refers to the machine coordinate system. To set the offset
values in MDI mode, use the command:
G10L2P<p_value>X<x_offset>Y<y_offset>Z<z_offset>

There should be a file included with the EMC distribution called
skeleton.txt that is a template for an EMC program.

Matt