Fagor 8065, Error Solving Manual

Page: 102 / 220

Error solving manual.
CNC 8060
CNC 8065
·102·
(R
EF
: 1709)
2000-2999
2000 'Tool radius greater than the arc radius'
DETECTION During execution.
CAUSE The tool radius is greater than the radius of the arc to be machined.
SOLUTION Use a tool with a smaller radius.
2001 'Profile damaged by tool radius compensation'
DETECTION During execution.
CAUSE The tool radius is too large for the programmed profile; the tool will damage the profile.
SOLUTION Use a tool with a smaller radius.
2002 'The first block of the linear compensation must be linear'
DETECTION During execution.
CAUSE 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.
SOLUTION Tool radius compensation must begin in a linear block. Therefore, the motion block
that goes after G41-G42 must be a linear motion block.
2003 'Tool radius too large in consecutive arcs'
DETECTION During execution.
CAUSE 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.
SOLUTION Use a tool with a smaller radius.
2004 'Too many motionless blocks between blocks that have tool radius compensation'
DETECTION During execution.
CAUSE While tool radius compensation is active, there are too many motionless blocks
(parameter assignments P, variables, etc.) between two motion blocks.
SOLUTION Reduce the number of motionless blocks programmed; for example, group several
of these blocks into a single block.
2005 'The last block of the linear compensation must be linear'
DETECTION During execution.
CAUSE After canceling tool radius compensation (G40), the next motion block is a circular
block. Tool radius compensation cannot end in a circular block.
SOLUTION Tool radius compensation must end in a linear block. Therefore, the motion block that
goes after G40 must be a linear motion block.
2006 'Tool radius compensation (G41/G42) must be changed on a linear path'
DETECTION During execution.
CAUSE 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.
SOLUTION 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.
2007 'While G138 is active, G40 is not allowed after the first compensation block'
DETECTION During execution.
CAUSE After activating tool radius compensation with the direct method (G138), a
compensation cancellation has been programmed before the first motion block.
SOLUTION 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.