Three Remuneration Methods Used in CNC Treatment

• 1
  Key takeaways
• 2
  What the three remuneration methods actually control
• 3
  Tool length compensation: setting and running it
• 4
  Cutter radius compensation: G41 and G42 in practice
• 5
  Work offset compensation: G54 to G59 and beyond
• 6
  Step by step: setting all three compensations on a new job
• 7
  The three compensation methods compared

A CNC program describes the path of a theoretical point, not the real cutting edge. Compensation is the offset between that point and the metal. The three remuneration methods used in CNC treatment are tool length compensation, cutter radius compensation, and work offset compensation. Each one corrects a different error, and each one is entered in a different place in the control.

Length compensation answers the question: where is the tip of this tool right now? Every tool has a different stick-out from the spindle gauge line. Without length compensation, Z0 would drift by 50 mm or more between tools. The control reads the offset and shifts the whole coordinate system in Z for that tool only.

Radius compensation answers a second question: how wide is this cutter? A 12 mm end mill cannot follow a 12 mm centerline path and produce a 12 mm slot. The offset shifts the path sideways by the cutter radius so the edge, not the center, lands on the profile. On a curved wall, the same offset also controls how the cutter rolls around the corner.

Work offset compensation answers the third question: where is the part? Fixtures move, vises get re-clamped, and a second operation starts from a different face. Work offsets let one program run on several setups without rewriting the coordinates. The part origin moves in the offset table, not in the code.

• 1
  Length = Z position of the tipOne value per tool, stored in the tool offset page.
• 2
  Radius = side shift of the pathOne value per tool, entered as a positive radius.
• 3
  Work offset = position of the partUsually G54 to G59, one per setup or per vise jaw.

Tool length compensation is the offset that puts the tip of the tool at the programmed Z height. In most controls it is stored as a negative value in the geometry column, measured from the spindle gauge line down to the tip. On a 40-taper machine, this value commonly runs from -80 mm to -250 mm depending on holder and tool length.

Touch off is the critical step. Bring the tool down to a known surface at low feed, jog in 0.01 mm increments near contact, and record the machine Z position. Do this on the same surface every time, or on a tool presetter if you have one. A 0.02 mm error in touch-off becomes 0.02 mm on every depth in the program.

During the program, G43 activates the offset with an H number. H01 applies the length from tool offset 01. The value stays active in the control until it is cancelled or replaced. Cancel it with G49 before a tool change, or let the next G43 overwrite it. Cancelling too early drops Z by the full offset length, which is a common crash on older controls.

On a 24-tool turning center or a mill-turn machine, length values often run in the X direction instead of Z. The same logic applies, but the axis changes. Read the control manual before mixing tool types, because a length value stored for a lathe tool will not work on a mill tool and the difference is not always obvious in the offset page.

• 1
  Always touch off at the same referenceA table surface, a fixture pad, or a presetter. Never a random surface.
• 2
  Watch the signNegative values below the gauge line are standard on many controls; positive values exist on others.
• 3
  Re-check after every tool changeA partially seated holder moves the tip by 0.05 mm or more.

Cutter radius compensation shifts the programmed path sideways by the radius of the tool. G41 offsets the cutter to the left of the direction of travel; G42 offsets it to the right. The value comes from the tool radius column in the offset table, not from the part drawing. For a 10 mm end mill, the radius is 5 mm.

Lead-in and lead-out moves matter. The control needs a straight move at least as long as the cutter radius to ramp the offset in. A typical lead-in is 5 mm to 10 mm at a 45 degree angle or along a tangent. If the lead-in is too short, the control alarms out or cuts a gouge at the entry point. This is the most common radius compensation error on first runs.

Use G41 and G42 for walls, pockets, and profiles. For a roughing pass that leaves 0.3 mm of stock, program the centerline path and use a radius offset of the cutter radius plus the finish allowance. Then run a separate finish pass with the true radius. Mixing the two in one pass is how walls come out undersized.

On inside corners, a cutter larger than the corner radius cannot clear the corner. The control has no way to remove material the tool cannot reach. Check the smallest inside radius on the part against the tool radius before you program the path. If the corner is 4 mm and the tool is 10 mm, the corner needs a smaller tool or a different geometry.

• 1
  Left vs rightG41 for climb milling on an outside profile travelling clockwise; G42 for the opposite direction.
• 2
  Lead-in lengthAt least one cutter radius, 5 mm to 10 mm is a safe starting range.
• 3
  Cancel with G40Cancel at the end of the profile, on a straight move, not on an arc.

Work offset compensation sets the origin of the part inside the machine envelope. The standard offsets are G54 through G59, with additional extended offsets on most modern controls. Each offset stores an X, Y, and Z value that shifts the program zero to a new position. A second vise jaw, a second fixture, or a flipped part gets its own offset.

Setting a work offset starts with an edge finder or a probe. Find the X and Y edges of the part or fixture, then find the Z reference surface. Enter the values into the offset page and verify by moving to X0 Y0 in rapid at a safe Z height. Watch the position display: it should read zero at the edge you touched. A 0.01 mm probe error is a 0.01 mm shift on every feature.

On a 5-axis machine, the work offset is not the whole story. The rotary centerline and the trunnion position also affect the part origin. The control combines the work offset with the rotary transformation. If the rotary centerline is off by 0.1 mm, features cut at different angles will be off in different directions. This is why 5-axis setups need a probe and a known centerline, not just a touched-off corner.

For a second operation on a flipped part, use a separate offset and a known datum from the first operation. A common mistake is to re-use G54 for both sides. The program runs, but the second side is off by the amount the part moved in the vise. On parts held to ±0.005 mm, that shift is enough to fail inspection.

• 1
  One offset per setupG54 for the first vise, G55 for the second, G56 for the flip.
• 2
  Probe if you have oneA probe removes the operator's touch-off error, which is often 0.02 mm to 0.05 mm.
• 3
  Record the valuesWrite the offset numbers on the setup sheet so the next run starts from the same place.