Use of the Tools Radius Compensation in the Milling Center

• 1
  Use of the tools radius compensation: why the cutter center is offset
• 2
  G41, G42 and G40: left, right, and cancel
• 3
  Lead-in moves and the corner the control cannot cut
• 4
  Rough and finish with one program, and what the register holds
• 5
  Where radius compensation stops being useful
• 6
  When to use compensation, and when to program the center path

A milling cutter is a circle in plan view. When the control drives the tool along a programmed line, it moves the spindle axis, not the cutting edge. On a straight pass the error is invisible. On a corner, the edge that matters is the one touching the wall, and the center sits one radius away from it. Program the center and the part comes out small by one radius on every outside profile. Program the edge and the control has to know where the edge is.

That is the whole problem. The programmed path is the part geometry. The machine moves the tool center. The gap between the two equals the cutter radius, measured normal to the path at every point. On a Ø12 mm end mill the gap is 6 mm. On a 3 mm cutter it is 1.5 mm. Ignore it and a 50 mm square becomes 38 mm with a Ø12 tool.

Tool radius compensation closes the gap in the control, at run time. The programmer writes the part outline. The operator tells the control which tool is in the spindle and what its radius is. The control shifts every motion left or right of the path by that radius, then recomputes the corners where two shifted lines meet. The operator never edits the geometry.

This split is the reason the function exists. Geometry stays in the program. Tool size stays in the offset register. Change a cutter, or regrind one, and only the register changes. The program runs again unchanged, and the part still lands on size. For shops running the same family of parts on several machines, that separation saves real setup time.

Three codes do all the work. G41 is compensation left. G42 is compensation right. G40 cancels it. Left and right are defined by the direction of travel, not by which side of the part you are cutting. Stand behind the tool, look along the feed direction, and G41 puts the offset to your left. G42 puts it to your right.

The practical rule engineers use: for climb milling an outside profile with the tool going counterclockwise around the part, the offset is on the left of travel, so it is G41. Reverse the direction and the same cut becomes G42. Get this backwards and the control offsets the tool into the part. The first move usually snaps the cutter, or gouges the wall by two radii.

G40 must be active before any move where you do not want the offset. Tool changes, rapid moves to a safe plane, and moves to the next feature all belong after a G40. Leaving compensation active across a positioning move is one of the most common crash causes on a vertical mill, because the control keeps applying the radius to the rapid.

The control also needs to know which register holds the radius. That is the D word on most controls, for example G41 D01. D01 points to offset register 1. The value inside the register is the radius, not the diameter, on nearly every Fanuc-style control. Enter 6.0 for a Ø12 mm cutter. Enter 12.0 and the part is undersize by 6 mm per side.

Compensation cannot switch on while the tool sits on the final profile. The control needs at least one move, longer than the radius, to slide the tool from the programmed path to the offset path. That move is the lead-in. A typical lead-in is a straight line or a quarter arc, 1.5 to 2 times the cutter radius long, at a shallow angle to the profile.

A short lead-in is a real failure mode. If the lead-in is shorter than the radius, the control has no room to reach the offset path and alarms out, or it reaches it late and leaves a mark on the wall. On a Ø12 mm cutter, keep the lead-in above 9 mm. On a Ø3 mm cutter, above 5 mm is usually enough.

Inside corners have a second limit. The largest radius the control can place in a sharp internal corner is the cutter radius. A Ø12 mm tool cannot leave a 3 mm inside corner radius, no matter what the offset register says. The tool physically cannot reach it. The drawing has to allow a corner radius at least equal to the cutter radius, or the feature needs a smaller tool. This is a geometry limit, not a control limit.

Outside corners are the reverse case. The control has to insert a corner arc where two offset lines meet, and the arc radius equals the cutter radius. On a sharp outside corner that arc sweeps the tool around the point. If the lead-out crosses the lead-in, the control may alarm or leave a witness mark. Give the exit move clear space, and keep the overlap off the finished wall.

The strongest argument for compensation is roughing and finishing from one program. Write the finish geometry once. For roughing, set the register to the cutter radius plus the stock allowance, say 6.4 mm for a Ø12 mm cutter leaving 0.4 mm. For finishing, set the register back to 6.0 mm. One program, two passes, no geometry edits.

The register value is not always the nominal radius. A reground cutter is smaller, and the wear offset should track that. Measure the cutter, or cut a test feature and measure the result, then adjust the register by half the error per side. This is normal practice on any machine holding ±0.005 mm, especially in 6061-T6, 7075, 17-4PH and Ti-6Al-4V where cutter wear moves faster.

Radial runout matters too. A cutter with 0.02 mm runout cuts oversize on one flute and undersize on the others. Compensation cannot fix an out-of-round cut, only a size error. Check runout at the holder before blaming the offset. On finishing passes, keep runout under 0.01 mm for Ra 0.8–1.6 μm walls.

Keep a written rule for who edits the register. If the operator adjusts the radius to chase a size that drifted for thermal reasons, the next part may come out wrong when the machine cools. Size drift from heat belongs in the wear offset, with a note on the setup sheet, not in the radius field.

Compensation is a 2D tool. It works in the plane selected by G17, G18 or G19. On a 3D contoured surface, the correct offset changes direction from block to block, and a single register value cannot describe it. Most CAM systems handle those paths by posting the compensated center path directly. That is not a shortcoming of the operator. It is the wrong tool for the job.

The same applies to simultaneous 5-axis motion. The tool axis tilts, the contact point moves around the cutter, and a fixed left or right offset has no consistent meaning. Five-axis toolpaths are posted as center paths with the tool vector included in every block. Use compensation on 2.5D features in a 5-axis program, then cancel it before the contoured moves begin.

Look-ahead is the other limit. The control must find the intersection of two offset lines before it can move. If the block after the lead-in is very short, or the geometry has a near-tangent corner, some older controls alarm with an interference error. Modern controls handle this better, but the safe habit is to keep the first compensated move long and simple.

None of this removes the need to check the register before the cycle starts. A wrong D word, a radius entered as a diameter, or a G41 left active from a previous tool will all produce a bad part on the first cut. The offset screen is worth ten seconds of attention on every setup.