FANUC G51 scaling: why doubling the contour does not double tool compensation or peck depth
Using the 0i-D machining-center manual, calculations around a nonzero scaling center and an internal circular contour distinguish workpiece geometry, tool compensation and peck depth. Enlarging dimensions does not mean multiplying every value by two.
Contents
When scaling a proven program for a similar part, an important distinction is easily missed: the part geometry becomes larger, but the tool installed in the machine does not. The following explains this boundary of G51 on 0i-D / 0i Mate-D machining centers, assuming that scaling is available and correctly configured.
First identify which quantities are scaled
The public mirror of the original B-64304EN-2/01 manual, §6.9, printed pages 215–222 explains that G51 starts scaling and G50 cancels it. Cutter compensation, tool length compensation and tool offset values do not scale with the geometry. The cut-in amount Q and retraction amount d for G83 / G73 are also excluded. This article addresses a uniform positive scale factor, excluding different factors for individual axes and mirroring through negative factors.
A nonzero center prevents simple coordinate doubling
Consider an original two-dimensional geometric example: scaling center C=(10,5) mm, original contour point P=(30,15) mm, and mathematical factor k=2. The formula P′=C+k(P−C) gives (50,25) mm. Directly calculating 2P gives (60,30) mm, which scales about the origin and changes the part position.
If a group of holes shifts together, first compare the scaling center with the workpiece datum. If point-to-point distances have doubled as intended but the whole group is displaced by (10,5) mm, further changes to cutter radius cannot fix that coordinate problem. Here k is a mathematical variable, not the P-word value to enter directly into a program.
Why the same tool needs a different center path
| Ideal internal circular contour | Original part | Double-size part |
|---|---|---|
| Finished contour radius R | 20 mm | 40 mm |
| Actual radius r of the same tool | 5 mm | 5 mm |
| Geometrically required tool-center radius R−r | 15 mm | 35 mm |
The table describes geometry only, ignoring runout, wear and cutting deformation. Simply scaling the original 15 mm tool-center path to 30 mm differs from the 35 mm calculated for the new finished contour and the same tool. First establish whether the CNC receives a finished-part contour or a tool-center path already calculated by CAM. These are different scaling objects.
Peck depth is a process quantity that needs a separate assessment
If the original peck cut-in amount is 3 mm, enlarging the contour alone does not make it 6 mm. When hole depth, drill diameter or chip evacuation conditions change, reassess the appropriate peck depth and then check the actual program data. During validation, compare target contour points, compensated tool-center positions and each cut-in amount separately. All three levels must agree to explain the machining behavior after scaling. More information is available in the OPTION section.