Example 1: TNC Standard Interpolation Modes G01/G02/G03

Classic Control - Lathe Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue

This example of general TNC uses standard interpolation modes G01/G02/G03.

TNC Standard Interpolation G01, G02, and G03

Preparation

  • Turn Setting 33 to FANUC.

  • Set up these tools:

    T1 Insert with .0312 radius, roughing

    T2 Insert with .0312 radius, finishing

    T3 .250 wide grooving tool with .016 radius/same tool for offsets 3 and 13

Tool Offset X Z Radius Tip
T1 01 -8.9650 -12.8470 .0312 3
T2 02 -8.9010 -12.8450 .0312 3
T3 03 -8.8400 -12.8380 .016 3
T3 13 -8.8400 -12.588 .016 4
% O30421 (TNC STANDARD INTERPOLATION G01/G02/G03) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an rough OD tool) ; (T2 is a finish OD tool) ; (T3 is a groove tool) ; (T1 PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS off, Spindle on CW) ; G00 G54 X2.1 Z0.1 (Rapid to position S) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (T1 CUTTING BLOCKS) ; G71 P1 Q2 U0.02 W0.005 D.1 F0.015 (Begin G71) ; N1 G42 G00 X0. Z0.1 F.01 (P1 - TNC on) ; G01 Z0 F.005 (Begin toolpath) ; X0.65 (Linear feed) ; X0.75 Z-0.05 (Linear feed) ; Z-0.75 (Linear feed) ; G02 X1.25 Z-1. R0.25 (Feed CW) ; G01 Z-1.5 (Linear feed to position A) ; G02 X1. Z-1.625 R0.125 (Feed CW) ; G01 Z-2.5 (Linear feed) ; G02 X1.25 Z-2.625 R0.125 (Feed CW to position B) ; G01 Z-3.5 (Linear feed) ; X2. Z-3.75 (End of toolpath) ; N2 G00 G40 X2.1 (Q2 - TNC off) ; (T1 COMPLETION BLOCKS) ; G97 S500 (CSS off) ; G53 X0 M09 (X home, coolant off) ; G53 Z0 (Z home, clear for tool change) ; M01 (Optional program stop) ; (T2 PREPARATION BLOCKS) ; T202 (T2 is a finish OD tool) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS off, Spindle on CW) ; G00 G54 X2.1 Z0.1 (Rapid to position S) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (T2 CUTTING BLOCKS) ; G70 P1 Q2 (Finish P1 - Q2 using T2, G70 and TNC) ; (T2 COMPLETION BLOCKS) ; G97 S500 (CSS off) ; G53 X0 M09 (X home, coolant off) ; G53 Z0 (Z home, clear for tool change) ; M01 (Optional program stop) ; (T3 PREPARATION BLOCKS) ; T303 (T3 is a groove tool) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G97 S500 M03 (CSS off, Spindle on CW) ; G54 G42 X1.5 Z-2.0 (TNC on, rapid to point C) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (T3 CUTTING BLOCKS) ; G01 X1. F0.003 (Linear feed) ; G01 Z-2.5 (Linear feed) ; G02 X1.25 Z-2.625 R0.125 (Feed CW to position B) ; G01 G40 X1.5 (TNC off) ; T313 (Change offset to other side of insert) ; G00 G41 X1.5 Z-2.125 (TNC left on) ; G01 X1. F0.003 (Linear feed) ; G01 Z-1.625 (Linear feed) ; G03 X1.25 Z-1.5 R0.125 (Feed CCW to position A) ; (T3 COMPLETION BLOCKS) ; G00 G40 X1.6 M09 (TNC off, coolant off) ; G97 S500 (CSS off) ; G53 X0 (X home) ; G53 Z0 M05 (Z home, spindle off) ; M30 ; %
note: The suggested template of the previous section for G70 is used. Also note that compensation is enabled in the PQ sequence but is canceled after G70 is completed.

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.

Feedback