1. CNC Codes and Letters
NOTE: The following will be a listing and description of Computer Numerical Control (CNC) Codes and Letter designations. We will try to stick with only “generic” codes that will work on most machines. Some examples may be specifically for the machines we have at South Adams / Area 18 Machine Trades. Please contact the instructor if you find any errors, missing items, or anything you would like to see added.

2. Code
Meaning
Letter
G00
Positioning (Rapid Traverse) A
Rotary indexing axis around the "X" axis
G01
Linear Interpolation (Feed) B
Rotary indexing axis around the "Y" axis
G02
Circular Interpolation CW C
Rotary indexing axis around the "Z" axis
G03
Circular Interpolation CCW D
Cutter Radius / Diameter offset number
G04
Dwell E
Feedrate in inches per revolution (Lathe)
G17
X,Y Plane of Interpolation F
Feedrate in inches per minute (can be used on lathes)
G18
X,Z Plane of Interpolation G
Preparatory commands
G19
Y,Z Plane of Interpolation H
Offset Number (Mill - tool length)(Lathe - Position offset)
G20
Input in Inch I
Arc center location in the "X" axis
G21
Input in MM J
Arc center location in the "Y" axis
G28
Return to Machine zero (reference point) K
Arc center location in the "Z" axis
G40
Cutter Compensation cancel L
Fixed Cycle repetion count / subprogram repetition count
G41
Cutter Compensation left M
Miscellaneous function
G42
Cutter Compensation right N
Block / Sequence number
G43
Tool length compensation + O
Program Number
G44
Tool length compensation - P
Subprogram / Macro Number call
G54-G59
Set Local Coordinate Systems (Datum Shifts)
Dwell time in milliseconds
G80
Canned Cycle cancel
Block number in main program when used with M99
G81
Spot Drilling Cycle (no dwell) Q
Depth of peck in fixed cycles (G73and G83)
G82
Drill/Counterbore (with dwell)
Shift amount in fixed cycle (G76 and G87)
G83
Peck Drilling Cycle R
Retract point in fixed cycles
G85
Bore
Arc Radius designation
G90
Absolute Programming S
Spindle speed in RPMs
G91
Incremental Programming T
Tool function
G92
Set Program Zero U
Incremental move in "X" axis
G94
IPM Programming V
Incremental move in "Y" axis
G95
IPR Programming W
Incremental move in "Z" axis
M00
Program stop X
"X" axis coordinate value designation
M01
Optional stop Y
"Y" axis coordinate value designation
M02
End of Program Z
"Z" axis coordinate value designation
M03
Start Spindle (Clockwise)
M04
Start Spindle (Counterclockwise)
M05
Spindle off
M06
Tool change
M08
Coolant on
M09
Coolant off
M30
Program reset/tape rewind
M98
Sub-Program call
M99
Return to previous program
You should already have a list of G&M Codes and CNC Letters as shown. If you do not have one, see your instructor, or download one off of the South Adams / Area 18 Machine Trades

3. “G” Codes
- “G” Codes are known as Preparatory Commands which means they are preparing the CNC machine to do something.
- Normally there should only be one “G” code per line, one exception is in the “Safety Line” at the beginning of the program.
- “G” Codes are to be at the start of the “Block” of Program.
Safety Line Example: G17 G20 G40 G80 G90

4. G00 Positioning Rapid Traverse
First of all notice that it is “G” “Zero” “Zero” all of the G&M Codes use Zero and not the letter “O”.
“G00” means the tool is going to move from where ever it currently is to the next position in a straight line as fast as the machine will go.
Think of “G00” as a dragster, something that will go from point A to point B in a straight line as fast as possible
Example: G00 X2.00 Y3.00

5. G01 Linear Interpolation
- “G01” means the tool is going to move from where ever it currently is to the next position in a straight line but this time with a given feedrate.
Think of “G01” as a truck driving on highway 218 or 124 through Adams County, Indiana, these highways are straight AND they have a speed limit.
On Milling Machines, the feedrate will typically be in IPM (inches per minute) and labeled with an “F”.
On Turning Machines, the feedrate will typically be in IPR (inches per revolution) and labeled with an “E or F”
Example: G01 X2.00 Y3.00 F6.00

6. G02 Circular Interpolation (CW)
“G02” Used anytime you need an arc in the Clockwise direction.
As with any Interpolation (machine movement), the machine already knows where it is, you only need to tell it where you want to go next.
For example: if you are setting at X0,Y0 and you want to put a 1.00” radius to X1.00, Y1.00 the “Block” would look like one of the following:
G02 X1.00 Y1.00 R1.00 F12.0
G02 X1.00 Y1.00 I1.00 J0 F12.0

7. G03 Circular Interpolation (CCW)
Just like with the “G02” preparatory command, the “G03” will move from point A to Point B only this time in a Counter Clockwise direction.
The “Block” of code will look identical to the code for “G02” only the code will change.
G03 X1.00 Y1.00 R1.00 F12.0
G03 X1.00 Y1.00 I1.00 J0 F12.0
- Always keep an eye on the details, the difference between “G02” and “G03” would be devastating if you wanted one and entered the other into a program!

8. CNC Vocab pit stop Antonym = Non-modal Modal [mohd-l]
A Command that is to remain in a certain mode until canceled by another mode
In other words: it keeps going and going and going and going….. Until it is told to stop later in the program
Antonym = Non-modal

9. G04 Dwell
“G04” is used anytime you want to pause or dwell at a position
A common “Block” when “Dwell” is required would be – G04 P500
The “G04” of course specifies Dwell
The “P500” states that it will be for 500 milliseconds
Note: 1 Second equals 1000 milliseconds
Therefore if you need to pause for 4.5 seconds you would program the “Block” as: G04 P4500
Example: G04 P1000

10. G17 X,Y Plane of Interpolation
“G17” is the most common plane to choose for a vertical machining center.
“G17” will normally be one of if not THE first “G” code in a program.
The reason the “G17” is so popular is that it could also refer to the table in front of you, the “X axis” is right and left movements while the “Y axis” would be towards and away from you

11. G18 X,Z Plane of Interpolation
“G18” could best be described as a normal engine lathe because the “Z axis” is the longitudinal travel of the lathe and the “X axis” would be your cross slide.
On a vertical machining center, this plane would be like looking at the screen of the controller since the “X axis” is right and left and the “Z axis” is up and down.

12. G19 Y,Z Plane of Interpolation
On a Vertical milling machine, this would be the plane parallel to the side of the machine.
Once again, just think it through, the “Y axis” is towards and away from you and the “Z axis” is up and down.

13. G20 Inch Input
“G20” will typically be at the beginning of the program, that way the CNC knows right away that every dimension entered will be Inch and not metric.
“G20” is very important to enter into each program you want to be inch, imagine if the program that ran prior to yours was a metric program and you do not switch it to inch, every dimension you enter will be read by the CNC as metric…. OPPS!

14. G21 Metric Input
Many shops have switched over to total metric, so “G21” is becoming more popular in this area.
How you program using “G21” is identical to “G20” the only difference is you are entering Metric dimensions instead of Inch.

15. G28 Return to Machine Zero
AKA: Return to Reference Point
“G28” can be very handy, On a Vertical Machining Center anytime you want the tool as far away from the part vertically as possible you would enter “G28 G91 Z0”. If you want the part to come as close to you as possible for easy part changing you would enter “G28 Y0”
Example: G28 G91 X0 Y0 Z0 Would bring the machine as fast as it can to its home position

16. G40 Cutter Compensation Cancel
Typically found in the “Safety Line” of the program
Just like the description implies, “G40” is used to cancel any cutter compensations whether it is for length (or height) compensation or Diameter Compensation.
Keep in mind that the person operating the machine prior to you could have done something with cutter compensation totally legal BUT different than what you need, cutter compensation cancel will clear everything out and be ready for you to add.

17. G41 Cutter Compensation Left
Cutter compensation is used to program a part exactly to size using the dimensions provided on the print…. THEN at the machine, offset that geometry to compensate for the tool you are using
Imagine climb milling around the outside of this picture the cutter would be rotating clockwise and moving around the picture clockwise, now guess which side of the part the cutter is…. Your right, the LEFT side!

18. G42 Cutter Compensation Right
- Just like the “G41” compensation only the opposite. Imagine conventional milling the same outside of this picture, the cutter is still spinning clockwise but this time the cutter is traveling counterclockwise around the outside of the part.
NOW which side of the part is the cutter traveling on? You are right the Right side!

19. G43 Tool Length Compensation +
Tool length compensation allows a machine to adjust for the different lengths of the tools.
Basically it is telling the machine how far it is from its “Z” home position to the position when the part touches the “Z origin” of the part.
The “H” value will be Added (+) to programmed “Z” position
Example: G43 Z1.0 H01

20. G44 Tool Length Compensation -
Tool length compensation allows a machine to adjust for the different lengths of the tools.
Basically it is telling the machine how far it is from its “Z” home position to the position when the part touches the “Z origin” of the part.
The “H” value will be Subtracted (-) from the programmed “Z” position
Example: G44 Z1.0 H01

21. G54-G59 Work Offsets AKA: Datum Shifts
AKA: Set Local Coordinate Systems
Specifies the distance the machine would need to move from its home position to the origin of the part or fixture.
Used mostly when multiple parts / fixtures / Set-ups are on the same table
Example: G55 G90 G00 X0.000 Y0.000

22. G80 Canned Cycle Cancel AKA: Fixed Cycle Cancel
Clears out any “Modal” Canned or Fixed cycles used earlier in a program
Used in the Safety Line to insure that what someone else did before does not affect what you will be doing in your program
Example: G82 X2.00 Y3.00 R.100 Z-.500 F6.0
G80

23. G81 Spot Drill Cycle (no dwell)
Specifies that you want to drill to a given depth
Along with the G81 you will also need to specify the following:
Hole Position
R-Plane
Z Depth
Feedrate
Example: G81 X2.00 Y3.00 R.100 Z-.250 F6.0

24. G82 Spot Drill Cycle (dwell)
Specifies that you want to drill to a given depth
Along with the G82 you will also need to specify the following:
Hole Position
R-Plane
Z Depth
Feedrate
Dwell time
Example: G82 X2.00 Y3.00 R.100 Z-.250 F6.0 P500

25. G83 Peck Drill Cycle Specifies that you want to drill to a given depth
Along with the G83 you will also need to specify the following:
Hole Position
R-Plane
Z Depth
Feedrate
Peck Increment
Example:
G83 X2.00 Y3.00 Z R.100 Q.250 F6.0

26. G83 Peck Drill Cycle Comparison
G83 X2.00 Y3.00 Z R.100 Q.250 F6.0
- OR -
N0110 G00 X2.00 Y3.00
N0120 G00 Z.100
N0130 G01 Z-.150 F6.0
N0140 G00 Z.1
N0150 G00 Z-.150
N0160 G01 Z-.400
N0170 G00 Z.1

27. WE ARE NOT DONE YET… N0180 G00 Z-.400 N0190 G01 Z-.650 N0200 G00 Z.100

28. STILL A COUPLE MORE LINES…
N0270 G00 Z-1.150
N0280 G01 Z-1.250
N0290 G00 Z.100
That is just for one hole! Now imagine doing that for EVERY deep hole!
One line per hole versus 19 Lines… you decide!

29. G73 Peck Drill Cycle (High Speed)
Specifies that you want to drill to a given depth
Does NOT fully retract after each peck depth
Along with the G73 you will also need to specify the following:
Hole Position
R-Plane
Z Depth
Feedrate
Peck Increment
Example:
G73 X2.00 Y3.00 Z R.100 Q.250 F6.0

30. G84 Tapping Cycle (RH)
Specifies that you want to Tap a previously drilled hole
Along with the G85 you will also need to specify the following:
Hole Position
R-Plane
Z Depth
Feedrate = RPM X Lead of the thread
1/4-20 Thread at 800RPM = F40.0
Example: G84 X2.00 Y3.00 R.100 Z-.250 F40.0

31. G85 Boring Cycle Specifies that you want to Bore to a given depth
Along with the G85 you will also need to specify the following:
Hole Position
R-Plane
Z Depth
Feedrate
Example: G85 X2.00 Y3.00 R.100 Z-.250 F6.0

32. CNC Vocab pit stop
Cartesian Coordinate System (kärtē'zhən)   A system in which the location of a point is given by coordinates that represent its distances from perpendicular lines that intersect at a point called the origin.

33. G90 Absolute Programming
The Origin or Datum location of your part does not move.
ALL coordinates are in relationship to one location in space
Example: G90 G00 X2.00 Y3.00 Z1.00

34. G91 Incremental Programming
The Origin or Datum location of your part does moves as your tool moves
ALL coordinates are in relationship to the point the tool is located at
Example: G91 G00 X2.00 Y3.00 Z1.00

35. “M” Codes - “M” Codes are known as Miscellaneous Functions.
- Normally there should only be one “M” code per line. Most machines are really picky about this, more so than with “G” codes.
- “M” Codes are to be at the start of the “Block” of Program.
Example: M03 S1500

36. M00 Program Stop
REMINDER: notice that it is “M” “Zero” “Zero” all of the G&M Codes use Zero and not the letter “O”.
M00 will stop the program without pressing “Feed Hold”
Insert M00 whenever you want to stop the program no matter what the conditions are.
Note: on some machines this will also turn off the spindle and not restart it without a M03
Example: M00

37. M01 Optional Stop
M01 is a conditional stop, it is determined by an operator activated switch on the control panel
If the switch is on, it will stop the program identical to a M00
If the switch is off, it will ignore the M01
Best uses:
Before or After Tool Changes
Anytime you want to inspect, oil or manipulate the part or tool
Example: M01

38. M02 End of Program M02 is used only at the end of the program
Some machines will not start a program unless it knows there is an end
M02 does not rewind the program
Example: M02 %

39. M03 Spindle Rotation Normal
M03 – Mill Clockwise rotation – If you were on top of a vertical milling machine looking down
M03 – Lathe Normal Rotation – the direction the chuck would need to spin if you had a normal right hand helix drill bit
Example: M03 S1200

40. M04 Spindle Rotation Reverse
M04 – Mill Counter-Clockwise rotation – If you were on top of a vertical milling machine looking down
M03 – Lathe Reverse Rotation – the opposite direction the chuck would need to spin if you had a normal right hand helix drill bit
Example: M04 S1200

41. Turns spindle off Example: M05
M05 Spindle Off
Turns spindle off
Example: M05

42. M06 Automatic Tool Changer
AKA: “ATC”
Will put away the tool that is in the spindle and replace it with the tool that is identified on the same line as the M06
Example: M06 T01 or
T01 M06

43. Turns on Mist Coolant Example: M07
M07 Mist Coolant On
Turns on Mist Coolant
Example: M07

44. Turns on Flood Coolant Example: M08
M08 Flood Coolant On
Turns on Flood Coolant
Example: M08

45. Turns Off All Coolant pumps / Soleniods Example: M09
M08 Coolant Off
Turns Off All Coolant pumps / Soleniods
Example: M09

46. M30 End of Program & Rewind
M30 is used only at the end of the program
Some machines will not start a program unless it knows there is an end
M30 does rewind the program
All you have to do is change the part and press cycle start
More common than M02
Especially if more than one part is to be made
Example: M30 %

47. M98 Sub-Program Call
Used in a main program when you want to call up another program while still in the main program.
Example: M98 P1001

48. M99 Sub-Program End
Used in place of an M30 when a program is used as a sub-program
Example: M99 %