G94 CNC Code | Feed per Minute | Milling

English CNC Wiki
1

G94 CNC Code: Understanding Feed Per Minute in Machining Centers

Introduction:

In CNC machining, accurately controlling the feed rate (the speed at which the cutting tool moves relative to the workpiece) is fundamental to achieving the desired surface finish, dimensional accuracy, and tool life. The G94 Feed Per Minute command is the most common way to specify feed rates in CNC machining centers. This article provides a detailed explanation of G94, its syntax, how it differs from G95 (Feed Per Revolution) and G93 (Inverse Time Feed), its use across various control systems (Fanuc, Siemens, Haas, Mazatrol, Mitsubishi, Heidenhain, and others), best practices, and programming examples. This guide is designed to be beneficial for both novice and experienced CNC machinists and programmers.

1. What is the G94 (Feed Per Minute) G-code?

G94 is a G-code that sets the CNC control to feed per minute mode. This means that the subsequent F word (feed rate) value will be interpreted as a linear speed:

  • Metric: Millimeters per minute (mm/min)
  • Imperial: Inches per minute (in/min)

When G94 is active, the machine will move the tool at the specified linear speed, regardless of the spindle speed. This is in contrast to G95 (Feed Per Revolution), where the feed rate is tied to the spindle’s rotation.

Key Concepts:

  • Feed Rate (F-word): The numerical value following the F in a G-code block, defining the feed rate.
  • Linear Speed: The speed at which the tool travels along the programmed path.
  • Modal Command: G94 is a modal command. It remains active until canceled by another feed rate command (G93, G95) or a machine reset.
  • Units: The interpretation of mm/min or in/min depends on whether the machine is set to metric (G21) or imperial (G20) units.

Example:

G94 F500 ; Set feed rate to 500 mm/min (or inches/min, depending on units)
G01 X100.0 Y50.0 ; Move to X100.0 Y50.0 at 500 mm/min

2. G94 vs. G95 (Feed Per Revolution) and G93 (Inverse Time Feed)

It’s essential to distinguish G94 from the other common feed rate modes:

  • G95 (Feed Per Revolution):
    • Specifies the feed rate in distance units per spindle revolution (mm/rev or inches/rev).
    • Primarily used in turning operations on lathes. This ensures a constant chip load regardless of spindle speed changes. Also very important in tapping operations.
    • Not generally used on machining centers except for specific operations like tapping with a rigid tapping cycle.
  • G93 (Inverse Time Feed):
    • Specifies the feed rate as the reciprocal of the time (in minutes) it should take to complete the programmed move.
    • Used for complex contouring and multi-axis machining, where maintaining a consistent toolpath speed is critical.
    • Requires more complex calculations than G94.
  • G94(Feed Per Minute):
    • Linear speed is set.
    • Most useful feed method in milling.

Choosing the Right Feed Mode:

Application Recommended Feed Mode (Machining Centers) Recommended Feed Mode (Lathes)
General milling G94 G95
Facing (milling) G94 G95
Contour milling (simple) G94 G95
Contour milling (complex) G94 (or G93 for very complex contours) G95 (or G93 for extreme cases)
Drilling G94 G95
Tapping (rigid tapping cycle) G95 (often implicit in the cycle) G95 (often implicit)
5-axis machining G94 or G93 G95 or G93
Straight Turning - G95
Facing (Turning) - G95

Important Note: While G94 is primarily used on machining centers and G95 is primarily used on lathes, there can be exceptions. For example, some lathe operations can use G94 for linear movements where spindle speed synchronization is not required. However, G95 is almost always preferred for turning because it maintains a consistent chip load.

3. Control System Variations

While the basic function of G94 is consistent across different CNC controls, there can be subtle differences in implementation and associated features.

  • Fanuc and Similar (Haas, Mitsubishi):

    • Syntax: G94 F[feed rate value]; (e.g., G94 F1000;)
    • Default: G94 is typically the default feed mode on Fanuc-style machining centers upon power-up or reset.
    • Modal: Remains active until canceled.
    • Feed Rate Override: The feed rate can be adjusted in real-time using the feed rate override knob on the control panel. The override percentage applies to the programmed F value.

  • Siemens (SINUMERIK):

    • Syntax: G94 F[feed rate value];
    • FGROUP: Similar to G93, Siemens controls offer the FGROUP command to specify which axes are affected by the G94 feed rate. This is useful in complex multi-axis machining.
    • CFTCP (Constant Feed at Tool Center Point): Siemens offers advanced features like CFTCP to maintain a constant feed rate at the tool tip, even when rotary axes are moving. This helps to ensure a consistent surface finish in 5-axis machining.
    • FNORM: Siemens.
    • Feed Rate Optimization: Siemens controls often have built-in feed rate optimization features that can automatically adjust the feed rate based on factors like tool engagement, curvature, and machine dynamics.

  • Mazatrol (Mazak):

    • Conversational Programming: In Mazatrol conversational programming, you would typically select “Feed Per Minute” (or its equivalent) as the feed rate mode within the appropriate machining unit (e.g., MILL, FACE MILL). The system then handles the G94 command internally.
    • EIA/ISO (G-code): Mazak machines can also run standard G-code, and G94 would function as expected.

  • Heidenhain:

    • Syntax: G94 F[feed rate value]; or L ... F[feed rate value] (Linear move with feed rate)
    • FMAX: Heidenhain allows specifying rapid traverse with FMAX. This overrides G94 for that specific block.
    • Advanced Functions: Heidenhain, like Siemens, has many built-in feed rate optimization.

  • Other Controls: Always consult the programming manual for your specific control.

4. Syntax and Parameters

The basic syntax of the G94 command is simple:

G94 F[feed rate value];

  • G94: The G-code that activates feed per minute mode.
  • F[feed rate value]: The desired feed rate, in mm/min (metric) or inches/min (imperial). The F word must be included in a block after G94 has been activated.

Example (Fanuc, Metric):

G21 ; Set metric units
G90 ; Absolute positioning
G94 ; Activate feed per minute mode
G01 X100.0 Y50.0 F500 ; Move to X100.0, Y50.0 at 500 mm/min
G02 X150.0 Y75.0 I25.0 J0 F800 ; Circular interpolation at 800 mm/min

Explanation:

  1. G21: Sets the machine to metric units (millimeters).
  2. G90: Sets absolute positioning mode.
  3. G94: Activates feed per minute mode.
  4. G01 X100.0 Y50.0 F500: A linear move to coordinates X100.0, Y50.0 at a feed rate of 500 mm/min.
  5. G02 X150.0 Y75.0 I25.0 J0 F800: A clockwise circular interpolation to X150.0, Y75.0 with a center point offset of I25.0, J0 (relative to the starting point of the arc), and a feed rate of 800 mm/min. Note that the F word can be changed within a program, even while G94 is active.

5. Programming Examples

Example 1: Simple Milling (Fanuc)

O0001 (Simple Milling Example)
G21 G90 G40 G80 ; Safety line (metric, absolute, cancel comp, canned cycles)
T01 M06 ; Tool change to Tool 1
G54 ; Select Work Coordinate System
G00 X-10.0 Y-10.0 S1200 M03 ; Rapid to above starting point, spindle on
G00 Z5.0 ; Rapid to clearance plane

G94 ; Activate feed per minute
G01 Z-2.0 F100 ; Feed down to cutting depth at 100 mm/min
G01 X100.0 Y50.0 F500 ; Mill a rectangle at 500 mm/min
G01 X100.0 Y-10.0
G01 X-10.0 Y-10.0
G01 X-10.0 Y50.0

G00 Z100.0 ; Rapid retract
M30 ; Program end

Example 2: Drilling with G94 (Fanuc)

O0002 (Drilling Example)
G21 G90 G40 G80 ; Safety line
T02 M06 ; Select drill (Tool 2)
G54 ; Select Work Coordinate System
G00 X25.0 Y25.0 S1000 M03; Rapid and spindle on
G00 Z5.0 ; Rapid

G94; Feed per Minute
G81 X25.0 Y25.0 Z-15.0 R2.0 F150 ; Drilling canned cycle (G81)
G81 X50.0 Y25.0
G81 X75.0 Y25.0
G80 ; Cancel canned cycle

G00 Z100.0 ; Rapid retract
M30 ; Program end

Explanation:

  • G81 is drill canned cycle.

6. Best Practices for Using G94

  • Calculate Feed Rates Correctly: Use the correct formulas and consider the material, tool type, tool diameter, spindle speed, and desired chip load to calculate the appropriate feed rate. Tool manufacturers often provide recommended cutting speeds and chip loads.
  • Use Recommended Cutting Data: Consult tool manufacturers’ data sheets for recommended cutting speeds (Vc, in m/min or SFM) and chip loads (fz, in mm/tooth or inches/tooth).
  • Adjust Feed Rate for Different Operations: Use a higher feed rate for roughing and a lower feed rate for finishing. Reduce feed when entering the material, when cutting full-width slots, and in corners.
  • Use Feed Rate Override: Utilize the feed rate override knob on the control panel to fine-tune the feed rate during machining. This allows you to adjust for variations in material hardness, tool wear, and other factors.
  • Consider Machine Dynamics: Be aware of your machine’s capabilities. Older or less rigid machines may not be able to handle high feed rates without vibration or chatter.
  • Check Machine’s Manual: Consult it.

7. Troubleshooting Common G94 Problems

  • Poor Surface Finish:
    • Cause: Feed rate too high, tool wear, incorrect spindle speed, or insufficient coolant.
    • Solution: Reduce the feed rate, replace the tool, adjust the spindle speed, and ensure adequate coolant flow.
  • Excessive Tool Wear or Breakage:
    • Cause: Feed rate too high, incorrect cutting speed, material hardness variations, or insufficient coolant.
    • Solution: Reduce the feed rate, adjust the spindle speed, check the material properties, and use appropriate cutting fluids.
  • Chatter:
    • Cause: Feed rate too high, excessive tool overhang, insufficient workpiece rigidity, or worn spindle bearings.
    • Solution: Reduce the feed rate, reduce tool overhang, improve workpiece clamping, and check the machine’s condition.
  • Inconsistent Feed:
    • Cause: Problem with machine.
    • Solution: Check machine’s manual.
  • Unexpected motion:
    • Cause: Using incorrect units (mm/min vs in/min).

8. Conclusion

The G94 Feed Per Minute command is a fundamental and widely used G-code in CNC machining centers. It provides a simple and intuitive way to control the linear speed of the cutting tool. Understanding how G94 differs from G95 and G93, how it’s implemented across different control systems, and following best practices are essential for any CNC machinist or programmer.