G43 G44 and G49 tool length compensation

G-Code G43, G44 and G49 (TOOL LENGTH COMPENSATION)

 In an CNC Programming Tool length compensation Code is used to adjust for differences in length between different tools, without worrying about those differences in your part program.

This standard length is the Reference Tool. In general, you load the Reference Tool, jog the Z axis down until that tool touches some surface, and set the Z Reference position there. The control memorizes this position of its Z axis. You then load each other tool, bring that tool down until it touches the same surface, and tell the control to measure the tool. The control compares the Z axis position with this tool touching the surface to the previously stored Z Reference position. The difference in Z axis positions is stored as the length offset for the tool.

Clearly, to touch the same surface with a shorter tool, you have to move the Z axis down further. This results in a negative offset. The shorter the tool, the more the negative offset.  To touch the same surface with a longer tool, you don't have to move the Z axis down as far. This results in a positive offset. The longer the tool, the larger (or less negative) the offset.

Listed below are the Three G-Code used only for the tool length compensation,

G43 Tool Length Compensation + (plus)

G44 Tool Length Compensation - (Minus)

G49 Cancel Tool length Comp G43 and G44

G43 Tool Length Compensation + (plus):

This code selects tool length compensation in a positive direction. The tool length offsets are added to the commanded axis positions. An Hnn must be programmed to select the correct offset register from the offset display for that tool being used. During the setup process, each tool point was touched-off to the part zero surface. From this position a Tool length distance offset was recorded for that tool with the Tool offset measure key. This Tool length is referred to as the "Z" axis origin move to the part zero surfaces.

G44 TOOL LENGTH COMPENSATION - (MINUS)

This code selects tool length compensation in a negative direction. The tool length offsets are subtracted from the commanded axis positions. A Hnn must be programmed to select the correct entry from offsets memory. G44 is a rarely-used alternative to G43. It tells the control to begin applying tool length compensation, by subtracting the current length offset from all Z axis positions. In this scheme, larger length offset numbers identify shorter tools (as if they were measured from the table up rather than from the spindle down).

G49 CANCELS G43/G44

This G code cancels tool length compensation. Putting in a H00 will also cancel tool length compensation. M30 and RESET will also cancel tool length comp.

Example for G43 and G44 Programs:

O1234

N170 T02 M06

N171 G90 G54 G00 X50 Y50 Z50 S800

N172 G43 H02 Z5 M08 (or G44 and H value will not be changed)

N172 G01 Z20 F50.

G40 G41 and G42 Cuttercompensation

G-Code G40, G41 and G42 (Cutter compensation):

Understanding cutter compensation can be very simple if one has a basic understanding of manual machining. There are two common types of cutting conditions associated with milling machines. They are CLIMB and CONVENTIONAL cutting. Two common rules for these types of cuts are:

If the programmed cutter path needs to mill CLIMB cutting, and it's a standard right handed tool, it will then be programmed with G41 cutter LEFT of the programmed path. If the programmed cutter path needs to mill with CONVENTIONAL cutting, and it's a standard right handed tool, it will then be programmed with G42 cutter RIGHT of the programmed path.

Listed below are the Three G-Code used only for the Cutter compensation,

G41 Cutter Compensation Left

G42 Cutter Compensation Right

G40 Cancel Cutter Comp G41 and G42

G41 Cutter Compensation Left:

G41 will select cutter compensation left; that is the tool is moved to the left of the programmed path to compensate for the radius of the tool. A Dnn must also be programmed to select the correct tool size from the DIAMETER/RADIUS offset display register.

G42 Cutter Compensation Right:

G42 will select cutter compensation right; that is the tool is moved to the right of the programmed path to compensate for the size of the tool. A Dnn must also be programmed to select the correct tool size from the DIAMETER/RADIUS offset display register.

G40 Cutter Comp Cancel:

G40 will cancel the G41 or G42 cutter compensation commands. A tool using cutter compensation will change from a compensated position to an uncompensated position. Programming in a D00 will also cancel cutter compensation. Be sure to cancel cutter compensation, when you're done with each milling cut series that's using compensation.

The Active Cutter compensation should satisfy the following points:

1) A G41 or G42 code must be contained with a G01 X, Y, or X and Y move is specified in the same block.

2) The distance of the linear move must be greater than the tool radius.

3) The tool radius value, "R", entered into the tool offsets table must not be 00.

4) A G02 or G03 circular interpolation command cannot be specified in the start-up block.

NOTE: The codes G4Ø, G41 and G42 are modal, belonging to the same modal family. They are incompatible with each other on the same block.

NOTE: The machine controller enters compensation cancel mode automatically when:

1) The machine power is first switched on.

2) The reset button on the CRT/MDI controller panel is pressed.

3) A program is forced to end by performing an M02 or M30 command.

Example for cutter compensation programming:

O 1234

N171 G00 X-15 Y-15 Z50;

N172 G01 Z0;

N172 G41 X0 Y0 F100; (Start-Up Move)

N173 Y40;

N174 X30 Y80;

N175 X60;

N176 G02 X100 Y40 R40;

N177 G01 Y30;

N178 G03 X70 Y0 R30;

N179 G01X0;

N180 G40 X-15 Y-15; (Cancellation Move)

N190 G00 Z50

ADVANTAGES OF CUTTER COMPENSATION:

1. The mathematical computations for determining a tool path are greatly simplified.

2. Because the geometry and not the tool center are programmed, the same program can be used for a variety of different cutter diameters.

3. When using cutter compensation you are then able to control and adjust for part dimensions using your cutter diameter/radius offsets register.

4. The same program path can be used for the roughing passes as well as finishing cuts by using different cutter offset numbers.

DIS ADVANTAGES WITH CUTTER COMPENSATION

1.      A cutter compensation command (G41, G42 or G40) must be on the same block with an X and/or Y linear command when moving onto or off of the part using cutter comp.

2.      You cannot turn on or off cutter compensation with a Z axis move.

3.   You can use cutter comp. in the G18 (X, Z) or G19 (Y, Z) planes using G141.

4.   You cannot turn ON or OFF cutter compensation in a G02 or G03 circular move, it must be in a linear G00 or G01 straight line move.

WHEN ACTIVATING CUTTER COMPENSATION, CARE MUST BE TAKEN TO:

1. Select a clearance point, without cutter compensation, to a start point in the X and Y axis at least half the cutter diameter off the part before you start initiating cutter compensation.

2. Bring the Z axis down without cutter compensation in effect.

3. Make an X and/or Y axis move with a G41 or G42 call-out on the same line, with a diameter offset Dnn command, which has the cutter diameter value in the offset display register being used.

WHEN DEACTIVATING CUTTER COMPENSATION, CARE MUST BE TAKEN TO:

1. Select a clearance point in X and/or Y axis, at least half the cutter diameter off the part.

2. DO NOT cancel cutter compensation on any line that is still cutting the part.

3. Cancel of cutter compensation (G40) may be a one or two axis move, but you may need values entered for both X and Y axis.

Very Important Note: In Practical the Cutcom should start before the Linear Movement with G01 and should end before the Linear Movement G01.