More Details for G69.
Sorry, but I pasted this from a PDF file and it seems to lose some spaces.
Must be a windows thing. There is a programming example at the bottom of
this post. If anyone needs a copy of the manual, They can download it in pdf
at http://www.fagor-automation.com/CNC/manuals.htm The 8040 M manual covers
programming for 8040,8050,8055. Some newer features in the manual may not be
available in your CNC due to Software/Hardware revisions.
Programming format:
G69 G98/G99 X Y Z I B C D H J K L R
G98 The toolwithdrawstothe InitialPlane,oncethe holehasbeendrilled.
G99 The toolwithdrawstothe ReferencePlane,oncethe holehasbeendrilled.
XY±5.5 Theseareoptionaland definethemovementof theaxesofthe
mainplanetoposition
thetool atthemachiningpoint.
This pointcanbeprogrammed inCartesiancoordinatesor inpolarcoordinates,and
thecoordinatesmaybe absoluteorincremental,according towhetherthemachine
isoperating inG90orG91.
Z±5.5 Definesthereferenceplane coordinate.Itcanbe
programmedinabsolutecoordinates
orincremental coordinates,inwhichcase itwillbereferred totheinitialplane.
If thisisnotprogrammed, theCNCwilltake thepositionoccupiedby thetoolatthat
moment asthereferenceplane.
I±5.5 Defines thetotaldrillingdepth. Itcanbeprogrammed
inabsolutecoordinatesor
incremental coordinatesandinthis casewillbereferred tothereferenceplane.
B5.5 Defines the drilling step in the axis longitudinal to the main plane.
C5.5 Defines to what distance from the previous drilling step, the
longitudinal axis will travel in rapid feed (G00) in its approach to the
part to make another drilling step.If this is not programmed, the value of 1
mm (0.040 inch) will be taken. If programmed with a value of 0, the CNC will
display the corresponding error.
D5.5 Defines the distance between the reference plane and the surface of the
part where the drilling is to be done. In the first drilling, this amount
will be added to "B" drilling step. If it is not programmed, a value of 0
will be taken.
H±5.5 Distance or position the longitudinal axis returns to, in rapid (G00),
after each drilling peck. A "J" value other then "0" means the distance and
if "J=0" indicates the relief position or absolute position it returns to.
When not programmed, the longitudinal axis will return to the reference
plane.
J4 Defines after how many drilling pecks the tool returns to the reference
plane in G00. A value between 0 and 9999 may be programmed. When not
programmed or programmed with a "0" value, it returns to the position
indicated by H (relief position) after each drilling peck. With "J >1" it
will return the distance indicated by "H" and every "J" steps to the
reference plane (RP).With J1, it will return to the reference plane (RP)
after each peck .With J0, it will return to the relief position indicated by
H.
K5 Defines the dwell time, in hundredths of a second, after each drilling
step, until the withdrawal begins. Should this not be programmed, the CNC
will take a value of K0.
L5.5 Defines the minimum value which the drilling step can acquire. This
parameter is used with R values other than 1mm (0.040 inch). If this is not
programmed or programmed with a value of 0, a value of 1 will be taken.
R5.5 Factor which reduces the drilling step "B". If this is not programmed
or programmed with a value of 0, a value of 1 will be taken. If R equals 1,
all the drilling steps will be the same and the programmed value "B". If R
is not equal to 1, the first drilling step will be "B", the second, "R B",
the third "R (RB)", and so on, i.e., after the second step, the new step
will be the product of factor R by the previous step. If R is selected with
a value other than 1, the CNC will not allow smaller steps than that
programmed in L.
EXAMPLE:
T1
M6
G0 G90 X0 Y0 Z0 ...................................................... ;
Starting point
G69 G98 G91 X100 Y25 Z-98 I-52 B12 C2 D2
H5 J2 K150 L3 R0.8 F100 S500 M8 ....... ; Canned cycle definition
G80
............................................................................
. ; Canned cycle cancellation
G90 X0 Y0 .................................................................
; Positioning
M30
............................................................................
; End of program
Tom
Post by tmaxG83 is the "Simple Deep Hole drilling cycle" and is set up with a
incremental peck amount and number of pecks. The G69 "Complex Deep Hole
Drilling Cycle" is programmed with an absolute depth, but has many more
parameters for retract amount, chip break, etc. All Fagor mill controls are
like this (8025,8050, 8055,8040) You might want to give the post guy both
options.
Tom Maxwell
Applications Engineer
Fagor Automation Corp.
714-957-9885
Post by JimHello
We have a Motion Master cnc that has a Fagor 8055M control, We mostly do
3axis wood molds and models, however sometimes we need to do some 2 axis
drilling on .250 thick aluminum. When I post out a drill program using a
peck cycle I get an error code on the control (can't think what it is
exactly) It will not do a peck. Even spent an afternoon hand writing some
small programs using the Fagor manual. Still could not get it. Does
anyone
Post by Jimout there have a fagor 8055m that is able to do a peck drill cycle? Could
you send me a little sample program that works on your machine?
Our Cam post guy is working on it, but I have a job to drill this week,
and
Post by JimI'm not sure if I'll get a fix by then. Thanks for any help / suggestions.
Jim