Rockwell Automation 8520 9/Series CNC Lathe User Manual

Page 596

Compounding Turning Routines

Chapter 24

24-32

Prevent this invalid cycle profile error by keeping the right portion of the

following equation less than the radius of any arcs in your cycle profile.

(I+U)

+ (K+W)

(tool radius)

The same basic equation can apply to other contours. If the length of a

block in the contour is less than the right portion of the above equation,

you can get an “INVALID CYCLE PROFILE” error depending on your

part contour. For contours with pockets, the width of the pocket must be at

least twice the value of the right hand portion of the above equation. In

general this error is a result of removing metal too far from the original

part profile (I, K, U, or W too large) and reducing this distance typically

resolves the error condition.

The workpiece contour blocks can be at any location within the same

program containing the G75 block (even after an end of program block).

They can not be resident in a subprogram or macro that is called by the

program containing the G75 block. Contour blocks can be either circular

or linear blocks. Any F-, S-, or T-words that are programmed in this set of

contour blocks are ignored when they are executed as workpiece contour

blocks in the G75 mode.

In Example 24.7, the workpiece contour blocks are blocks N11 - N14.

Example 24.7

Typical G75 Block Followed By Blocks Defining Final Contour

N005 G75P11Q14I2.W2.D3.F10.S210;

N010 M30.;

N011 X24.;

N012 X55.Z40.;

N013 X65.Z35.;

N014 X70.Z5.;

The control generates multiple passes each offset from the other by an

amount equal to the total material to be removed (I+K/2) divided by the

number of passes (D) minus 1. The tool paths repeat until (D) tool paths

have been made across the part. Each tool path is shifted sequentially by

the distance obtained in this division to generate roughing paths. If a

finishing allowance (U, W) was programmed in the block, it is left uncut.

After the completion of the roughing routine, the cutting tool returns to the

routines starting point.