Need Help!- Funuc oi-tc Alarm #064

[Datech]

064 SHAPE PROGRAM NOT MONOTONOUSLY. What is this meant?


G00 Z.1
X4.51
G71 U0400
G71 P100 Q200 U0100 W0 F.01
N100 G00 X4.224
G01 Z0 F.005
G03 X4.275 Z-.025 R.025 F.002
G01 X4.2725 Z-3.7114 F.004
X4.4934 Z-3.9026
G03 X4.5 Z-3.9151 R.025 F.002
N200 G01 Z-4.1 F.004
G70 P100 Q200

What missing in the program?

[hitachibos]

what is the X and Z position just before you call this routine?

it should be the same X as end point X4.5 and the Z off the face .050 or .1

[dcoupar]

Originally Posted by Datech 064 SHAPE PROGRAM NOT MONOTONOUSLY. What is this meant? G71 U0400 G71 P100 Q200 U0100 W0 F.01 N100 G00 X4.224 <----- Initial X --- try adding W0 to this block G01 Z0 F.005 G03 X4.275 Z-.025 R.025 F.002 <----- Increasing X G01 X4.2725 Z-3.7114 F.004 <----- Decreasing X - not allowed in TYPE I cycle X4.4934 Z-3.9026 <----- Increasing X G03 X4.5 Z-3.9151 R.025 F.002 <----- Increasing X N200 G01 Z-4.1 F.004 G70 P100 Q200 What missing in the program?

If the program above is the correct shape, you can try adding a W0 to N100 to specify a TYPE II (non monotonous) cycle. If your machine has the option, you shouldn't get the alarm.

[Datech]

dcoupar, add w0 to n100 solved the problem. Thank you for your help.