# Corner Rounding and Chamfering Example

## 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.

## Corner Rounding and Chamfering

A chamfer block or a corner rounding block can be automatically inserted between two linear interpolation blocks by specifying ,C (chamfering) or ,R (corner rounding).

note: Both of these variables use a comma symbol (,) before the variable.

There must be a terminating linear interpolation block after the beginning block (a G04 pause may intervene). These two linear interpolation blocks specify a theoretical corner of intersection. If the beginning block specifies a ,C (comma C) the value after the C is the distance from the corner of intersection where the chamfer begins and also the distance from that same corner where the chamfer ends. If the beginning block specifies an ,R (comma R) the value after the R is the radius of a circle tangent to the corner at two points: the beginning of the corner rounding arc block that is inserted and the endpoint of that arc. There can be consecutive blocks with chamfer or corner rounding specified. There must be movement on the two axes specified by the selected plane (the active plane X-Y (G17), X-Z (G18) or Y-Z (G19). For chamfering a 90° angle only, an I or K value can be substituted where ,C is used.

## Chamfering

% o60011 (G01 CHAMFERING) ; (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 X0 Z0.25 (Rapid to 1st position) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G01 Z0 F0.005 (Feed to Z0) ; N5 G01 X0.50 K-0.050 (Chamfer 1) ; G01 Z-0.5 (Linear feed to Z-0.5) ; N7 G01 X0.75 K-0.050 (Chamfer 2) ; N8 G01 Z-1.0 I0.050 (Chamfer 3) ; N9 G01 X1.25 K-0.050 (Chamfer 4) ; G01 Z-1.5 (Feed to Z-1.5) ; (BEGIN COMPLETION BLOCKS) ; G00 X1.5 M09 (Rapid Retract, Coolant off) ; G53 X0 (X home) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

This G-code syntax automatically includes a 45° chamfer or corner radius between two blocks of linear interpolation which intersect a right (90 degree) angle.

Chamfering Syntax

G01 X(U) x Kk ; G01 Z(W) z Ii ;

Corner Rounding Syntax

G01 X(U) x Rr ; G01 Z(W) z Rr ;

Addresses:

I = chamfering, Z to X (X axis direction, +/-)

K = chamfering, X to Z (Z axis direction, +/-)

R = corner rounding (X or Z axis direction, +/-, Radius value)

Notes:

1. Incremental programming is possible if U or W is specified in place of X or Z, respectively. So its actions are as follows:

X(current position + i) = Ui

Z(current position + k) = Wk

X(current position + r) = Ur

Z(current position + r) = Wr

2. Current position of X or Z Axis is added to the increment.

3. I, K and R always specify a radius value (radius programming value).

## Corner Rounding Code X to Z: [A] Corner rounding, [B] Code/Example, [C] Movement.

Rules:

1. Use K address only with X(U) address. Use I address only with Z(W) address.

2. Use R address with either X(U) or Z(W), but not both in the same block.

3. Do not use I and K together on the same block. When using R address, do not use I or K.

4. The next block must be another single linear move that is perpendicular to the previous one.

5. Automatic chamfering or corner rounding cannot be used in a threading cycle or in a Canned cycle.

6. Chamfer or corner radius must be small enough to fit between the intersecting lines.

7. Use only a single X or Z-axis move in linear mode (G01) for chamfering or corner rounding.

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.