2000-2999 - Fagor 8065 Error Solving Manual

2000
DETECTION
CAUSE
SOLUTION
2001
DETECTION
CAUSE
SOLUTION
2002
DETECTION
CAUSE
SOLUTION
2003
DETECTION
CAUSE
SOLUTION
2004
DETECTION
CAUSE
SOLUTION
2005
DETECTION
CAUSE
SOLUTION
2006
DETECTION
CAUSE
SOLUTION
CNC 8060
2007
DETECTION
CNC 8065
CAUSE
SOLUTION
(R : 1709)
EF
·102·

2000-2999

'Tool radius greater than the arc radius'
During execution.
The tool radius is greater than the radius of the arc to be machined.
Use a tool with a smaller radius.
'Profile damaged by tool radius compensation'
During execution.
The tool radius is too large for the programmed profile; the tool will damage the profile.
Use a tool with a smaller radius.
'The first block of the linear compensation must be linear'
During execution.
After activating tool radius compensation (G41 or G42), the next motion block is a
circular block. Tool radius compensation cannot begin in a circular block.
Tool radius compensation must begin in a linear block. Therefore, the motion block
that goes after G41-G42 must be a linear motion block.
'Tool radius too large in consecutive arcs'
During execution.
When machining two consecutive arcs that form a loop (the two arcs intersect each
other), the tool radius is too large for machining the inside of the loop.
Use a tool with a smaller radius.
'Too many motionless blocks between blocks that have tool radius compensation'
During execution.
While tool radius compensation is active, there are too many motionless blocks
(parameter assignments P, variables, etc.) between two motion blocks.
Reduce the number of motionless blocks programmed; for example, group several
of these blocks into a single block.
'The last block of the linear compensation must be linear'
During execution.
After canceling tool radius compensation (G40), the next motion block is a circular
block. Tool radius compensation cannot end in a circular block.
Tool radius compensation must end in a linear block. Therefore, the motion block that
goes after G40 must be a linear motion block.
'Tool radius compensation (G41/G42) must be changed on a linear path'
During execution.
The program has changed the type of tool radius compensation (from G41 to G42
or vice versa) and the next motion block is a circular block.
The tool radius compensation cannot be changed if the next motion block is an arc.
Change the type of radius compensation on a linear tool path.
'While G138 is active, G40 is not allowed after the first compensation block'
During execution.
After activating tool radius compensation with the direct method (G138), a
compensation cancellation has been programmed before the first motion block.
To activate tool radius compensation with the direct method (G138), the CNC needs
an additional block in the plane besides the activation block. The CNC allows
canceling tool radius compensation after this movement. If this block cannot be
programmed, use the indirect method (G139) to activate tool radius compensation.
E r r o r so l v i n g m a n u a l .