Xilog Plus - Training for the SCM Record 5 axis CNC Router Wood 482 - 2014
Get Started
After you open the Xilogs Plus program and before you open an existing or create new program you have to decide if you want to use the text or graphical editor to create or review a program.
Ope Open Xil Xilog og Plus Plus Under “Option” choose the “Text” or “Graphical” editor
Get Started
After you open the Xilogs Plus program and before you open an existing or create new program you have to decide if you want to use the text or graphical editor to create or review a program.
Ope Open Xil Xilog og Plus Plus Under “Option” choose the “Text” or “Graphical” editor
New Program
Xilogs - Interface
New Tool Display D isplay
Display Graphic
Mechanical Options Suction Cup Editor
Header – date In Input
Header
The first line of each program
The Header includes the
dimensions of the stock to be machined position of the stock on the machine worktable the “Tool File”, used for the program containing tool specific information number of pieces to be processed
Header
DX – Stock X Dimension (Length) DY – Stock Y Dimension (Width) DZ – Stock Z Dimension (Thickness)
Example: The size of the stock is 600mm in length, 400mm in width, and 20mm thick.
Header
“-” – Machine Worktable - Area By default “AB” – LEFT SIDE OF THE MACHINE
Note, use “AD” processing a full sheet using the 5-axis machine Workpiece reference is on the back, left side of the machine table
Work Area - AD
Work Area - DA
Origin in front right
Mirrored in Y
Work Area - EH Origin in the back – Mirrored in X
Work Area - HE Origin in the back right – Mirrored in X and Y
Header
C – continuous machining flag (must always be “0”) T – lifter, “0” to disable & “1” to enable R – number of repetitions for the same stock (normally “1”) “*” – unit of measurement, MM for millimeters & IN for inches “/” – tools file name User must provide the tool file for the specific CNC machine.
Header
BX – distance in X between the stock zero and the field zero (pins) BY – distance in Y between the stock zero and the field zero (pins) BZ – distance in Z between the stock zero and the field zero (worktable)
Header (BX,BY,BZ for3 axis machine)
Left Side of the CNC
+BY
-BX
+BX
-BY
0,0,0
Front Side of the CNC
Header
V – Work piece locking control setting
V=0 – no control (Caution – Machine will start automatically without checking the vacuum setting – Do not use) V=150 – work piece locking control using vacuum switches (3/5-axis - Suction cups)
XGIN – Automatic Tool Approach
G – type of entry
G=1 – straight line (default) G=2 – arc (see manual for more information)
R – tool radius multiplication factor (default=2) Q – type of approach: 0=vertical (upwards) (default); 1=inclined (downwards) F – machining face (default = 1) Back F=5 Left F=3
Top F=1
Right F=2
XGIN – Automatic Tool Approach
C – tool radius adjustment (Tool Correction)
C=0 – bit on centre of the path (default) C=1 – bit on the right of the path C=2 – bit on the left of the path
Router Bit C=0 Center C=1 Right C=2 Left
XGIN – Automatic Tool Approach
G – type of entry
G=1 – straight line G=2 – arc (see manual for more information)
Q – type of approach: 0=vertical (upwards); 1=inclined (downwards) Ex 1: G=1, Q=0, C=0
Top View
Side View
XGIN – Automatic Tool Approach
G – type of entry
G=1 – straight line G=2 – arc (see manual for more information)
Q – type of approach: 0=vertical (upwards); 1=inclined (downwards) Ex 1: G=2, Q=0, C=0
Top View
Side View
XGIN – Automatic Tool Approach
G – type of entry
G=1 – straight line G=2 – arc (see manual for more information)
Q – type of approach: 0=vertical (upwards); 1=inclined (downwards) Ex 1: G=1, Q=1, C=0
Top View
Side View
XGIN – Automatic Tool Approach
G – type of entry
G=1 – straight line G=2 – arc (see manual for more information)
Q – type of approach: 0=vertical (upwards); 1=inclined (downwards) Ex 1: G=2, Q=1, C=0
Top View
Side View
XGIN – Automatic Tool Approach
K – incremental or absolute
K=0 absolute co-ordinates (Recommended) K=1 incremental X co-ordinate, absolute Y co-ordinate K=2 absolute X co-ordinate, incremental Y co-ordinate K=3 incremental X co-ordinate, incremental Y co-ordinate
P – reference origin
P=0 lower left-hand stock origin (Recommended) P=1 mirrored in X P=2 mirrored in Y P=3 mirrored in XY P=11 as P=1 with arc inversion (clockwise/counter-clockwise) P=12 as P=2 with arc inversion (clockwise/counter-clockwise) P=13 as P=3 with arc inversion (clockwise/counter-clockwise)
XG0 – Start Routing
For F=1 (Top surface)
F=1 Top
XG0 – Start Routing
For F=2 (Right surface)
F=2 Right
For F=3 (Left surface)
F=3 Left
XG0 – Start Routing
For F=4 (Front surface)
For F=5 (Back surface)
F=5 Back F=4 Front
XG0 – Start Routing
V – machining speed (mm/min or m/min) (Not Required) S – tool speed (rpm) (Not Required) D – outside machining dimension (safety Z) (Not Required)
N – profile name for repetitions command ex: GREP or XGREP (Not Required) T – routing tool number (MUST BE PROVIDED)
F, C, K, P,IF, and “;” are same as XGIN
XL2P – Segment Through Two Points
Moves from the last position to the newly defined position
With X, Y, Z input
X – end segment, X co-ordinate Y – end segment, Y co-ordinate Z – end segment, Z co-ordinate
With B & L input
B – segment angle with reference to trigonometric zero (positive counter clockwise) ex: B = 30 L – segment length from the start point to the end point
XA2P – Arc Through Two Points Defines a circular arc passing through two points: Enter the co-ordinates of the end point and the center point of the arc
User must enter parameters XYIJG or X/Y IJB
X – end of arc, X co-ordinate Y – end of arc, Y co-ordinate Z – end of arc, depth A – angle of rotation V – routing speed I – center, X co-ordinate J – center, Y co-ordinate B – arc angle
G – direction of travel (2=clockwise, 3=counter-clockwise) L – arc length (1=smaller, 2=larger)
XAR2 – Arc Given the Radius Defines a circular arc passing through two points: Enter the co-ordinates of the end point and the arc radius. If the circular arc is less than 180 Deg set a positive radius, greater than 180 Deg set a negative radius
User must enter parameters XYZArG
X – end of arc, X co-ordinate Y – end of arc, Y co-ordinate Z – end of arc, depth
r – arc radius G – direction (2 = clockwise, 3 = counter-clockwise)
XGOUT – Automatic Exit from Profile Defines a segment or circular arc, tangent to the profile at the exit point. Effective if the command is written after the last profile command.
G – type of exit (See XGIN) (1=straight line (default), 2=arc) (not required) R – tool radius multiplication factor (default=2) (not required) Q – type of withdrawal (0=down then in, 1=inclined downwards) (not required) L – Overlapping profile (not required) F – machining face (not required) C – tool radius adjustment (not required)
XGREP – Repeat Profile Defines profile repetition from the automatic entry in the profile (XGIN) to the automatic exit (XGOUT)
Q – determines whether X & Y are absolute=0 or offset=1 X – if Q=0, profile starting point X co-ordinate if Q=1, profile starting point offset X relative to previous Y – if Q=0, profile starting point Y co-ordinate if Q=1, profile starting point offset Y relative to previous Z – end of arc dept relative to work piece zero G – inversion of direction relative to previous (G=0 does not invert, G=1 inverts) V – routing speed (not required)
XGREP – Repeat Profile Cont.
Defines profile repetition from the automatic entry in the profile (XGIN) to the automatic exit (XGOUT)
S – tool speed (rpm) (not required) D – outside machining dimension (safety z) (not required) N – name of profile to be repeated (Name used in G0) T – Tool A – angle if rotation about the selected point for parameters x y (only if Q=0) x – point of rotation, X co-ordinate y – point of rotation, Y co-ordinate
XB - Boring Carries out one or more boring cycles To bore one or several holes, users must enter parameters XYZTF To repeat holes, users must enter parameters XYZRxyTF
X – first hole, X co-ordinate Y – first hole, Y co-ordinate Z – hole depth E – Hood position V – boring speed S – tool rpm Q – hole repetition for mirroring:
0 = no 1 = mirror X-axis 2 = mirror Y-axis
R – number of repetitions for holes programmed (excluding original) X – X step of repetition Y – Y step of repetition D – outside machining dimension (safety Z co-ordinate) G – number of steps for boring with shaving discharge T – number of tool or tools for multiple boring with boring machine ex:1 or 1 2 3 4
XB - Boring Ex 1: One Hole
Ex 2: Two Holes with 32mm step
XB - Boring Ex 3: A set of holes with the 32mm step boring machine
Assuming Tool 1, 2, & 3 have the same diameter and are installed.
G-CODE
G1 – Segment Through Two Points
Defines a linear section of routing.
X – end of the segment, X co-ordinate Y – end of the segment, Y co-ordinate Z – end of the segment, depth V – routing speed (expressed in mm/min or m/min)
G2 – Clockwise Circular Routing Defines a circular arc passing through two points: enter the coordinates of the end point and the arc radius or the co-ordinates of the center. * If the center of the circular arc is to the right of the chord, set a negative radius. * If the center of the circular arc is to the left of the chord, set a positive radius
X – end of the segment, X co-ordinate Y – end of the segment, Y co-ordinate Z – end of the segment, depth
I – center, X co-ordinate J – center, Y co-ordinate R – arc radius V – routing speed (expressed in mm/min or m/min)
G3 – Counter-clockwise Circular Routing
Defines a circular arc passing through two points: enter the coordinates of the end point and arc radius or the co-ordinates of the center. * If the center of the circular arc is to the right of the chord, set a negative radius. * If the center of the circular arc is to the left of the chord, set a positive radius
X – end of the segment, X co-ordinate Y – end of the segment, Y co-ordinate Z – end of the segment, depth
I – center, X co-ordinate J – center, Y co-ordinate R – arc radius V – routing speed (expressed in mm/min or m/min)
Crosspiece & Suction Cup Editor
Suction Cup Locations
After the programming is done, Xilog Plus has a function which can calculate
Suction Cup Locations
Crosspiece Bar Material Suction Cup
Tool Path
Location Pin
Suction Cup Locations 3 sizes of Suction Cups 145x145 180x65 145x55
Modify the orientation of the cup
Suction Cup Locations
Move the suction cups up & down
Suction Cup Locations
Once the suction cups are in correct position, press “Anti-Collision Control” in the tool bar.
Suction Cup Locations
Make changes if necessary and repeat the “Anti-collision control” until no more error messages occur. Save the file when the suction cup locating is done.
Tool Data Base
Open Tool Data Base Select “Open File” and select Tooling (.tlg) from the pull down menu. Select the name of the tool file (def) and press “Enter”
Fixed tools are normally drills installed in the drilling unit #1-100
“External Tools” are tools or aggregates that can be loaded into the tool changer
Example of Tool Parameters of a Router Bit
Tool Data Base
Graphic Display for Tools
