Inverse-Time and Feed-Per-Minute Modes

Introduction

This module tells you:
  1. The fundamental differences between the Inverse-Time and Inch-Per-Minute modes
  2. When to use each of the modes
  3. The benefits of using Inverse Time
  4. Settings and parameters that can improve the performance of Inverse Time.

Fundamentals of Inverse Time and Inch Per Minute

 

G93 Inverse Time

G93, Inverse Time Mode ON, translates the linear (inches/mm) feedrate into a value that takes rotary motion into account. G93 specifies that all F (feedrate) values are interpreted as strokes per minute. In other words, the time (in seconds) to complete the programmed motion using G93 is 60 (seconds) divided by the F value.

G93 is generally used in 4 and 5-axis work when the program is from a CAM system. When you use G93, the F value tells you how many times per minute the stroke (tool move) can repeat.

When G93 is used, feedrate (F) is mandatory for all interpolated motion blocks. Therefore, each non-rapid motion block must have its own feedrate (F) specification.

Program code G93 to start Inverse-Time mode.

G93 was introduced in Mill software version 9.22.

G94 Feed Per Minute

 

To accomplish a feedrate that is adjusted for distance over time while moving a rotary table, the machine must know the diameter of the cut. The Haas control uses Setting 34, 4th AXIS DIAMETER, and Setting 79, 5TH AXIS DIAMETER, to adjust the rotary speed based on the cut diameter.

G93, Inverse Time Mode OFF and G94, Feed Per Minute ON, is used whenever 3-axis milling is needed. Feed Per Minute uses a slower feedrate to cover longer distances.

Use G94 Feed Per Minute

  • When you program a 2D or 3D part
  • When you machine a diameter that does not change on a rotary table
  • When you use the 4th and 5th axes for positioning on 3+2 operations
  • When you invoke G107 Cylindrical Mapping
    • G107 can also be used to set the default diameter of a cylindrical surface, independent of any cylindrical mapping that may be in effect.
    • An A, B, or C address identifies which rotary axis holds the cylindrical surface
    • G107 variables Q and R
      • Q defines the diameter of the cylindrical surface. Sample code:
        G107 B0. X-1. Q2.0
      • R defines the radius of the cylindrical surface. Sample code:
        G107 C0. Y0. R2.
      • When Q or R is used, a rotary axis must also be specified.
      • If neither Q nor R is used, the last G107 diameter is used.
      • If no G107 command has been issued since power-up, or if the last value specified was 0, the diameter is the value in Setting 34 and/or 79 for the rotary axis specified.
      • When Q or R is specified, that value will become the new G107 value for the specified rotary axis.

When to Use G93 Inverse Time

  • When combined linear/rotary motion exists.
    • Each combined linear/rotary move has a different distance. Thus the corresponding time values change for each code block, even if it does not change from the previously programmed feed value.

Invoking Inverse-Time Mode

A G93 is necessary to declare the feed mode on the initial move containing rotary motion.

General Rule: If a G93 is necessary to invoke inverse time mode, a G94 is necessary to cancel it.

This means that the first move of a sequence of normal XYZ linear moves with no rotary A/B/C words must have a G94 and an F that is interpreted in inches per minute.

Benefits of G93 Inverse Time

G93 lets the user follow a more complex tool path when linear/rotary axes are involved.

G93 lets the user have better control of the rotary's motion. This gives a more precise part with a better surface finish.

Settings and Parameters That Improve Inverse-Time Performance

Setting 85, Maximum Corner Rounding

Setting 191, Default Smoothness

Parameter 104, A Axis In Position Limit

Parameter 165, B Axis In Position Limit

Parameter 512, C Axis In Position Limit

Parameters 786, 787, 788, 789, 790, 791, 792, 793, 794, 795, 796, and 797, Command Fir Order

Parameters 884, 885, 886, 887, 888, 889, 890, 891, 892, 893, 894, 895, 896, 897, 898, and 899, Notch Center Frequency

Parameter 900, 901, 902, 903, 904, 905, 906, 907, 908, 909, 910, 911, 912, 913, 914, and 915, Notch Depth Factor

Menu Category: 

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.