G41/G42 cutter radius compensation: telling left from right and writing the start-up and cancel blocks
Explains with a rectangular contour example how to tell G41 (left) from G42 (right) cutter radius compensation on a machining center by the direction of travel, D numbers and offset values, and the overcutting and alarms that occur in start-up and cancel blocks.
A function for programming straight from drawing dimensions
When milling a contour with an end mill, the tool center must travel offset from the machined surface by the tool radius. To mill the outside of a 60 mm wide shape with a Ø10 end mill, the center has to follow a path 5 mm outside on each side, that is, 70 mm wide. If this calculation is built into the program, every coordinate must be recalculated whenever the tool diameter changes.
Cutter radius compensation lets you write the drawing's contour coordinates directly in the program and has the controller calculate the tool-radius offset in real time. When the tool wears or is replaced with one of a different diameter, only the value on the offset screen has to change.
Left and right are relative to the direction of travel
G41 offsets the tool to stand on the left of the direction of travel, and G42 on the right. The reference is not the machine or the drawing but the direction in which the tool advances. Imagine driving a car: if the machined surface is outside the right-hand window, the tool is on the left (G41); if it is outside the left-hand window, the tool is on the right (G42).
When an end mill rotating forward (M03) goes around an outside contour clockwise, the tool is on the left of the contour, that is G41, and the cut is climb milling. Going around the same contour counterclockwise gives G42 and conventional milling. Typical CNC machining centers have little backlash, so climb milling is often used as the default.
| Machining location | Direction of travel | Compensation | Cutting mode (M03) |
|---|---|---|---|
| Outside (island) | Clockwise | G41 | Climb milling |
| Outside (island) | Counterclockwise | G42 | Conventional milling |
| Inside (pocket wall) | Counterclockwise | G41 | Climb milling |
| Inside (pocket wall) | Clockwise | G42 | Conventional milling |
Example contour
The path below is a program going clockwise around the outside of a rectangle from (0,0) to (60,40). The drawing shows the contour coordinates exactly as written in the program; the actual tool center path, pushed outward by the D3 offset, is calculated by the machine from the offset value. A path visualization tool cannot know the values in the machine's offset table.
A contour path climb-milling the outside of a 60×40 rectangle with G41 D3
O3002
T3 M6
G21 G90 G17 G40 G94
G54
S4000 M03
G00 X-20. Y-20. Z50.
Z2.
G01 Z-3. F150
G41 D3 X0. Y-10. F400
Y40.
X60.
Y0.
X-10.
G40 X-20. Y-20.
G00 Z50.
M30The figure above is the CNC Path Analyzer result for this program (rapid 3 segments, linear cutting 7 segments).
The start-up block needs a linear move
Compensation does not take effect the instant it is switched on: during the move of the block containing G41/G42, the tool shifts diagonally to the offset position. This block is called the start-up block and should normally be a linear G00 or G01 move. Many controllers raise an alarm if compensation starts in an arc block.
The start-up move must be longer than the offset value. The example starts compensation while moving about 22 mm from (-20,-20) to (0,-10), so that the tool settles on the extension below the contour start point (0,0) before cutting the first side with Y40.. Starting compensation right on the contour can cause overcutting into the machined surface during the offset move.
The cancel block and the last side
G40 is also written together with a move, so that compensation is released while the tool leaves the contour. The example extends the last side beyond the contour to X-10., then cancels while moving away with G40 X-20. Y-20.. Cancelling right at the end point of the contour can let the diagonal release move cut into the corner.
D numbers and offset values
D3 means use the value stored in line 3 of the tool offset screen. The same number as the tool number is usually used, but this is not required. The offset normally holds the tool radius, and measurement results are entered in the wear column to correct the size. If the outside comes out 0.02 mm larger than the drawing (0.01 mm per side), adjust the radius wear value by -0.01.
There is also a technique of deliberately entering an offset larger than the radius to leave a finishing allowance. Rough with a D value of 5.3 for a Ø10 tool, then change it to 5.0 and run the same program again to remove the 0.3 mm allowance as a finishing pass.
Where to check when a compensation alarm occurs
| Symptom | Common cause |
|---|---|
| Alarm when compensation starts | G41/G42 started in an arc block, or the start-up move is shorter than the offset |
| Overcut at inside corners | Consecutive non-moving blocks during compensation, or an inside arc radius smaller than the tool radius |
| Size wrong on one side only | G41/G42 opposite to the direction of travel, or the wrong D number |
| Corner damaged after cancelling | G40 right at the contour end point, with no extension move |