What is spiral milling?

A Spiral Milling Custom Macro Using Constant Contouring Feedrate

Milling a circular pocket is a very common machining center operation. Accepted practices include helical milling (circular XY motion with linear Z motion) and “spiral” milling (XY-circular motion after positioning in the Z-axis). These methods are especially helpful when the circular pocket being machined is quite large — much larger than the milling cutter diameter when multiple XY- and Z-axis passes are required. Chad Kluth of Mid Valley Industries provided suggestions and help with verification.

Features of this spiral milling FANUC Custom Macro include climb or conventional milling, as well as constant contouring feedrate. Additionally, if a prior hole exists that is larger than the milling cutter diameter, the milling cutter will rapid during Z-axis plunging motions. If the surface is solid — or if the hole is smaller than the cutter diameter — the cutter fill feed at half the XY-axes machining feedrate when plunging in the Z-axis.

Figure 1 shows several of the input values.

Figure 1. Photo Credit: CNC Concepts Inc.

Here are all the letter address arguments in the G65 calling command, their local variable representations and brief descriptions of their meanings:

X #24: X-axis center of the hole
Y #25: Y-axis center of the hole
Z #26: Z-axis surface into which to mill
R #18: Z-axis rapid approach distance from surface, default is 0.1 inch
D #7: Depth of pocket
V #22: Z-axis depth per pass
B #2: Big/final diameter
H #11: Hole diameter — if solid, leave H out of the calling command
E #8: XY-axes approach distance when there is a hole
F #9: XY- axes milling feedrate
U #21: Fast feedrate, used when moving back to starting position
C #3: Milling style — C1.0 or leave C out of call for climb, C2.0 for conventional
T #20: Tool diameter
Q #17: XY-axes stock removal per pass
W #23: Constant contouring feedrate, leave out of call or set to 0 for no, set to 1. for yes

This is an example calling program that includes the calling G65 command:

O0001
N005 T01 M06
N010 G54 G90 S600 M03
N015 G00 X0 Y0
N020 G43 H01 Z0.2 M08
N025 G65 P1000 X0 Y0 Z0 D0.5 R0.2 F5.0 U30.0 H4.0 E0.1 C1.0 B6.0 T1.0 Q0.2 V0.2 W1.0
N030 G91 G28 X0 M09
N035 G28 Z0 M19
N040 M30

It will use a 1.0-inch diameter end mill and machine a circular pocket at X0 Y0 from the hole diameter of 4.0 inches to its final diameter of 6.0 inches using a 0.2 XY-axes step-over per pass. The pocket will be machined 0.5-inch deep while taking 0.2-inch depths per pass. The pocket will be climb milled and constant contouring feedrate will be used. Most of the argument descriptions are self-explanatory. But a couple may need further clarification:

If you want only one Z-pass, set the depth per pass (V) to the same value as the circular pocket depth (D).
If constant contouring feedrate is not used (W0), then the XY-machining feedrate (F) will be used for all circular motions. If it is used (W1.0), the feedrate for each circular motion will be reduced to ensure that the milling cutter is not overloaded.

Whenever a milling motion is specified in the X- and/or Y-axes, the specified feedrate will be based upon the milling cutter’s centerline path. For linear motions, this is fine since the milling cutter’s periphery will move the same distance as its centerline. But with circular motions, the centerline path will be different than the milling cutter’s periphery path. For internal arcs, the centerline path will be shorter. It will be longer for external radius milling.

This means the centerline path feedrate must be slowed when making internal circular motions if the programmed feedrate is to be the rate of motion at the milling cutter’s periphery. The bigger the cutter radius, the more slowing will required. See Figure 2 to see how this applies to the spiral milling Custom Macro circular movements.

Figure 2. Photo Credit: CNC Concepts Inc.