# Troughs

## 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.

## Single Nest with (4) Troughs [1] and Two Nests: one with (5) Troughs [2] and one with (2) Troughs [3].

A trough can be defined as a change in direction which creates a concave surface in the material being cut. There can be no more than 10 troughs per cycle. If the part has more than 10 troughs, create another cycle. The following figures illustrate the sequence of roughing cuts (Type 1 and 2) for PQ paths with multiple troughs. All material above the troughs is roughed first, followed by the troughs in the direction of Z.

## Type 1 and 2 Tool Retractions: [1] Type 1, [2] Type 2, [3] Setting 73.

note: An effect of using a Z finish or roughing allowance is the limit between the two cuts on one side of a trough and the corresponding point on the other side of the trough. This distance must be greater than double the sum of the roughing and finish allowances.

For example, if G71 Type 2 path contains the following:

... X-5. Z-5. ; X-5.1 Z-5.1 ; X-3.1 Z-8.1 ; ...

The greatest allowance that can be specified is 0.999, since the horizontal distance from the start of cut 2 to the same point on cut 3 is 0.2. If a larger allowance is specified, over-cutting will occur.

Cutter compensation is approximated by adjusting the roughing allowance according to the radius and tip type of the tool. Therefore, the limitations that apply to the allowance also apply to the sum of the allowance and the tool radius.

caution: If the last cut in the P-Q path is a non-monotonic curve (using a finish allowance), add a short retraction cut; do not use W.

Monotonic curves are curves that tend to move in only one direction as x increases. A monotonic increasing curve always increases as x increases, i.e. f(a)>f(b) for all a>b. A monotonic decreasing curve always decreases as x increases, i.e. f(a)b. The same sort of restrictions are also made for the monotonic non-decreasing and monotonic non-increasing curves.

## G71 Basic G-code Example: [S] Start Point, [P] Starting block, [Q] Ending block.

% O60711(G71 ROUGHING CYCLE) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an OD cutting tool) ; (BEGIN 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 X6. Z0.1 (S - Rapid to 1st position) ; M08 (Coolant on) ; G96 S750 (CSS on) ; (BEGIN CUTTING BLOCKS) ; G71 P1 Q2 D0.15 U0.01 W0.005 F0.014 (Begin G71); (Stock removal cycle leaving stock allowance) ; N1 G00 X2. (P - Begin toolpath) ; G01 Z-3. F0.006 (Linear feed to Z-3.) ; X3.5 (Linear feed to X3.5) ; G03 X4. Z-3.25 R0.25 (CCW arc) ; G01 Z-6. (Linear feed to Z-6.) ; N2 X6. (Q - End of toolpath) ; G70 P1 Q2 (Finish pass) ; (BEGIN COMPLETION BLOCKS) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

## G71 Type 1 Stock Removal Example

% O60712(G71 FANUC TYPE 1 EXAMPLE) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an OD cutting tool) ; (BEGIN 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 X6.6 Z0.1 (Rapid to 1st position) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (BEGIN CUTTING BLOCKS) ; G71 P1 Q2 D0.15 U0.01 W0.005 F0.012 (Begin G71); (Stock removal cycle leaving stock allowance) ; N1 G00 X0.6634 (P1 - Begin toolpath) ; G01 X1. Z-0.1183 F0.004 (Linear feed chamfer) ; Z-1. (Linear feed) ; X1.9376 (Linear feed) ; G03 X2.5 Z-1.2812 R0.2812 (CCW arc round) ; G01 Z-3.0312 (Linear feed) ; G02 X2.9376 Z-3.25 R0.2188 (CW arc round) ; G01 X3.9634 (Linear feed) ; X4.5 Z-3.5183 (Linear feed chamfer) ; Z-6.5 (Linear feed) ; N2 X6.0 (Q2 - End of toolpath) ; G70 P1 Q2 (Finish pass) ; (BEGIN COMPLETION BLOCKS) ; G97 S500 (CSS off) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

## G71 Type 2 O.D./I.D. Stock Removal Example: [1] Start position, [P] Starting block, [Q] Ending block, [2] Finish allowance, [3] Programmed path.

% O0125 (FANUC G71 TYPE 2 EXAMPLE) ; T101 (Tool change and apply tool offset) ; G54 (Select coordinate system) ; G50 S3000 (Spindle rpm will not exceed 3000 rpm); G96 S1500 M03 (Constant surface cutting speed) ; G00 X1. Z0.05 (Rapid move to approach starting position) ; G71 P1 Q9 D0.05 U0.015 W0.010 F0.01 (Define PQ block path) ; N1 G00 X0. Z0.05 (P1 block) ; N2 G01 Z0. ; N3 G01 X0.75 ; N4 G01 Z-0.5 ; N5 G01 X0.625 Z-0.75 ; N6 G01 Z-1.25 ; N7 G01 X0.875 ; N8 G01 Z-1.75 ; N9 G01 X1. (Q9 block) ; G53 G00 X0 (Rapid move to x machine home) ; G53 G00 Z0 (Rapid move to z machine home) ; T202 (Tool change and apply tool offset) ; G96 S1500 M03 (Constant surface cutting speed) ; G70 P1 Q9 F0.005 (Finish path defined by PQ block) ; G53 G00 X0 (Rapid move to x machine home) ; G53 G00 Z0 (Rapid move to z machine home) ; M30 ; %

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.