Fadal G Codes


Fadal G Codes for Fadal VMCs / Fadal Machining Centers

G0 Rapid Travel
G1 Linear Interpolation
G2 Circular Interpolation (Clockwise)
G3 Circular Interpolation (Counter Clockwise)
G4 Dwell P= Time in Milliseconds
Also: Non Modal In-position Check
G5 Non Modal Rapid Travel
G8 Accelerate (No Feed Ramps)
G9 Decelerate (Feed Ramps)
Also: In Position Check
G10 Programmable Data Input
L02= Fixture X, Y, Z, A, B, P= 0, 1-48
L10= Length, P= 1-99, R0= Amount
L12= Diameter, P= 1-99, R0= Amount
L13= Read Fixture, P= 1-24, R0= Z, R1= X, R2= Y
L14= Read Length, P= 1-99, R0= Amount
L15= Read Diameter, P= 1-99, R0= Amount
L100 to L109= R Values, P= Amount
G15 YZ Circular Interpolation with the A Axis
G17 XY Plane Selection
Also: Y Axis Cam Wrapping
Q= A Axis Ratio/ [5p (cam dia. in inches)]
Q= A Axis Ratio/ [(5/25.4p (cam dia. in mm)]
P0= A Axis, P1= B Axis
G17.1 A/B Word Swap On
G17.2 A/B Word Swap Off
G18 ZX Plane
G19 YZ Plane
G20 Check for Inch Parameter Setting
G21 Check for Metric Parameter Setting
G28 Return to Zero
G28.1 Return from Jog Away
G29 Return from Zero
G31 Probe Touch Function
G31.1 Probe No Touch Function
G40 Cutter Radius Compensation Cancel
G41 Cutter Radius Compensation Left (climb)
G42 Cutter Radius Compensation Right (conve.)
G43 Tool Length Compensation Positive
G44 Tool Length Compensation Negative
G45 Tool Length Offset Single Expansion
G46 Tool Length Offset Single Reduction
G47 Tool Length Offset Double Expansion
G48 Tool Length Offset Double Reduction
G49 Tool Length Offset Cancel
G50 Ramp Slope Control Cancel
G50.1 Mirror Image Cancel
G51 Ramp Slope Control
R0= Ramp Speed Value of .5 – 2.
R0+= Z Axis, R0-= XY Axis
G51.1 Mirror Image
G51.2 Tool Load Compensation
State Feed Rate Before the G51.2 Line
R1= Target Spindle Load
R2= Min. Percentage Feed Rate Reduction
R3= Max. Percentage Feed Rate Increase
R4= Time at Min. Feed Rate to Initiate Slide Hold
G51.3 Axis Scaling
R1= Program (All three axes)
R2= X
R3= Y
R4= Z
G52 Coordinate System Shift
G53 Use Machine Coordinate System
G54-59 Fixture Offsets 1-6
G66 Modal Subroutine Call
G67 Modal Subroutine Cancel
G68 Rotation (R0= Angle, XY= Center of Rotation)
G69 Rotation Cancel
G70 Check for Inch Parameter
G71 Check for Metric Parameter
G73 Peck Drill
Q= Peck Size
P= Feed Distance before next Peck (optional)
I= Initial Peck
J= Reducing Value for Subsequent Pecks
K= Minimum Peck Size
G74 Left Hand Tap
Format 1 Q= Thread Lead (1/pitch), F= RPM
Format 2 S= RPM, F= Feed (Lead * RPM)
G74.1 Left Hand Rigid Tap
Format 1 Q= Thread Lead (1/pitch), F= RPM
Format 2 S= RPM, F= Feed (Lead * RPM)
G74.2 Prepare for G74.1
G75 Tapping Head Cycle
Format 1 Q= Thread Lead (1/pitch), F= RPM
Format 2 S= RPM, F= Feed (Lead * RPM)
G76 Fine Boring
Q= Amount of Y+ Shift or
I= Amount & Direction of X Shift
J= Amount & Direction of Y Shift
G80 Fixed Cycle Cancel
G81 Drill, Spot Drill
G82 Center Drill, Counterbore
P= Dwell Time in Milliseconds
180,000/RPM= Dwell time for 3 revolutions
G83 Deep Hole Cycle
Q= Peck Size
P= Feed Distance before next Peck (optional)
I= Initial Peck
J= Reducing Value for Subsequent Pecks
K= Minimum peck Size
G84 Right Hand Tap
Format 1 Q= Thread Lead (1/pitch), F= RPM
Format 2 S= RPM, F= Feed (Lead * RPM)
G84.1 Right Hand Rigid Tap
Format 1 Q= Thread Lead (1/pitch), F= RPM
Format 2 S= RPM, F= Feed (Lead * RPM)
G84.2 Prepare for G84.1
G85 Bore In / Out
G86 Bore In / Spindle Off / Rapid Out
G87 Bore In / Out
G88 Bore In / Dwell / Out, P= Milliseconds
G89 Bore In / Dwell / Out, P= Milliseconds
G90 Absolute Positioning
G91 Incremental Positioning
G91.1 High Speed Execution (-2 System Only)
G91.2 High Speed Execution Cancel
Also: Binary Compress / Analyzer End Point
G91.3 Binary Compress / Analyzer Start Point
G92 Absolute Preset
G93 1/T Feed Rate Specification (Inverse Time)
G94 Feed Rate Specification DPM, IPM
G98 Return to Initial Plane
G99 Return to R0 Clearance Plane

Fadal G Codes