Routech - Xilog Basic Programming Instructions

The following information is taken from:
"Basic CNC Router Training Course"
Routech
training SCM Group USA
advanced woodworking products laboratory
Pages 11 - 17

I am currently working on the setup of a Routech Record 240 that uses Xilog3 as the controller. The machine was purchased used and delivered in the described setup below.
The machine originally came with AlphaCAM. It has apparently been replaced with Vectric Aspire. Vector files are post-processed as .xxl files. A program called Winiso.exe converts the .xxl file to a .pgm file. Xilog3 locates the .pgm file on the C:\ Drive.

I am in the process of switching our CAD/CAM from Aspire to VCarve (also a Vectric product). During the set up I am running into a couple of issues with offsets.

H: (Header Instruction)

The header instruction is the most important part of a program; it contains information that is essential for machining and must always be carefully set up. Following an explanation of each of its parameters.

DX = Dimension of the Panel X (usually length). Required.
DY = Dimension of the Panel Y (usually width). Required.
DZ = Dimension of the Panel Z (Usually Height). Required.
- = Working Field. Required.
/ = Tooling File. Denotes the name of the file that contains all information about tools. by default the name is DEF. Required.
R = Number of times that the program will repeat before quitting the program. Required.
* = Units of measurement. Either MM or IN (caps). Required.
C = Continuous execution. DO NOT MODIFY.
T = Raise bars enable variable. This is not the tool number. DO NOT MODIFY.
# = Name of the environmental variables file. DO NOT MODIFY.
V = Intelligent clamping of part variable. This is not the feed rate. DO NOT MODIFY.
BX = Offset of on the X axis. Optional.
BY = Offset on the Y axis. Optional.
BZ = Offset on the Z Axis. Optional.

B: (Boring Command)

This command executes one or a series of holes, depending on the tools selected (list of tools).

X = X Coordinate of the hole. Required.
Y = Y Coordinate of the hole. Required.
Z = Z Depth desired for the hole. Required.
T = Tool list for the operation. The first tool is the REFERENCE tool. Required.
E = Position of the hood. Optional.
V = Boring Feed Rate. Optional.
S = RPM's of the tool. Optional.
G = Number of steps for the boring operation (Pecking). Optional.
D = Out-of-Network dimension. Allows clearance for longer tools or hurdles in the tool path. Optional.

BO: (Optimized Boring Command)

This command executes one or a series of holes, depending on the DIAMETER and TYPE of tools.

X = X Coordinate of the hole. Required.
Y = Y Coordinate of the hole. Required.
Z = Depth desired for the hole. Required.
D = Diameter of the hole. The first hole will be the REFERENCE hole for the successive holes. Required.
N = TYPE of tool that will perform the operation. (Brad=P, Lance=L, Countersink=S). Required.
L = Taper height of the countersink. Required only if N=S.
R = Number of Holes desired.
x = Distance from one hole to another (displacement, step) on the X axis, if more than one repetition is selected. If no step is desired, it is recommended to type 0. Required.
y = Distance from one hole to another (displacement, step) on the Y axis, if more than one repetition is selected. If no step is desired, it is recommended to type 0. Required.
V = Boring Feed Rate. Optional.
G = Number of steps for the boring operation (Pecking). Optional.

< I have to log off for now. I will post more on the subject later tomorrow. Take care and be well. >

G0: (Profile start point)

This command POSITIONS the machine at the desired coordinates and ENABLES the selected tool for ROUTING.

X = X Coordinate where the routing will START. Required.
Y = Y Coordinate where the routing will START. Required.
Z = Depth at which the routing will START. Required.
T = Tool that will execute the machining. Required.
E = Position of the dust extraction hood. (0=highest, 4=Lowest). Optional.
V = Routing Feed Rate. Required.
S = RPM’s of the tool. Optional.
D = Out-of-Work Dimension. Allows clearance for longer tools or hurdles in the tool path. Optional.
N = Profile name. Optional. For use only with the GREP command. < Linux based? >

G1: (Linear cut or Interpolation)

This command cuts in a STRAIGHT LINE, used when ROUTING.

X = X Coordinate where the routing will END. Required.
Y = Y Coordinate where the routing will END. Required.
Z = Depth at which the routing will END. Required.
V = Routing Feed Rate. Optional.

G2: (Circular cut, Clockwise Direction)

This command cuts in a CIRCULAR motion, clockwise fashion. May cut a full circle or portion of it (an arc is a portion of a circle), used when ROUTING.

X = X Coordinate where the routing will END. Required.
Y = Y Coordinate where the routing will END. Required.
Z = Depth at which the routing will END. Required.
I = X Coordinate of the CENTER of the circle. Optional.
J = Y Coordinate of the CENTER of the circle. Optional.
r = Radius of the circle. If we use the r parameter, we do not require the (I, J) coordinates, but if left blank (I, J) must be inputted. Optional.
V = Routing Feed Rate. Optional.

G3: (Circular cut, Counter-clockwise Direction)

This command cuts in a CIRCULAR motion, COUNTER-CLOCKWISE fashion. May cut a full circle or portion of it (an arc is a portion of a circle), used when ROUTING.

X = X Coordinate where the routing will END. Required.
Y = Y Coordinate where the routing will END. Required.
Z = Depth at which the routing will END. Required.
I = X Coordinate of the CENTER of the circle. Optional.
J = Y Coordinate of the CENTER of the circle. Optional.
r = Radius of the circle. If we use the r parameter, we do not require the (I, J) coordinates, but if left blank (I, J) must be inputted. Optional.
V = Routing Feed Rate. Optional.

C: ( Tool Compensation)

This command is used when we wish to apply compensation to a routing.

C = 0 No compensation selected.
C = 1 Compensation selected to the Right Hand side of the path.
C = 2 Compensation selected to the Left Hand side of the path.
C = 3 Length of radius Compensation. Used only when routing with a saw.
S = Machining allowance. This is a tolerance that enables us to fine-tune adjustments such as those needed because of tool sharpening, incorrect sizing/squareness of the part, etc.

N: (Null Command)

This command allows us to position the machine at a desired coordinate AT MAXIMUM SPEED. It is very useful when we need to move the machine out of the way for any reason. Traveling will occur with the electro spindle Out of work position.

X = Desired X coordinate where we want the machine to move. Required.
Y = Desired Y coordinate where we want the machine to move. Required.
V = Speed of displacement. If left blank, machine will move at MAXIMUM speed for the given axis. Optional.
S = RPM,s of the tool. As an option, a tool may be selected and the RPM’s defined. Optional.
T = Tool that will execute the NEXT machining. Optional.

SX / SY: (Mirror Commands)

These two commands will automatically MIRROR any coordinate inputted AFTER the command. They are “flags” that need to be turned either on (1) or off (2) hence, it is more important to remember to turn the OFF after we used them.

H DX = 600 DY = 400 DZ = 20 -A R99 /DEF
1. BO X = 9.525 Y = 75 Z = 11 D = 8 N = P R = 4 x = 0 y = 150
2. SX = 1
3. BO X = 9.525 Y = 75 Z = 11 D = 8 N = P R = 4 x = 0 y = 150
4. SX = 0

Note that the number lines 2 and 4 are identical, nonetheless, the software is producing the MIRROR image of such holes.

IX / IY: (Incremental Machining)

These parameters toggle ON and OFF the INCREMENTAL machining mode. This means that all actual coordinate is referenced FROM THE LAST coordinate that was written. As with the MIRROR command, it is advisable to always return it to it’s OFF position after use.

Considering the panel above:

H DX = 600 DY = 400 DZ = 20 -A R99 /DEF
1. IY = 1
2. B X = 9.525 Y = 75
3. B Y = 150
4. B Y = 150
5. B Y = 150
6. B X = 590.475 Y = 0
7. B Y = -150
8. B Y = -150
9. B Y = -150
10. IY = 0

Notice how the Y coordinate depends on the accumulated coordinate before it, so that each instruction is relative to the preceding one. Furthermore, since the IX = 1 IS NOT selected, the coordinate on the X is still ABSOLUTE and referenced from the LEFT EDGE of the Panel.

Just wondering how you are coming along with your machine? Vectric VCarve is not targeted for the commercial machine space, such as with SCM routers, but it works fine. Most folks using SCM Routers commercially, use AlphaCAM or CabinetVision, but both requiring a fairly hefty investment.

As you've likely found out, there are basically one or two post processor files for SCM equipment in the Vectric VCarve post processor dropdown in the toolpath section. Vectric does not support a drill head, so you will need to write your own code if you plan to do much with it i.e. the boring command "BO." The other issue you may run into with Xilog3 is that it was written so long ago that the table / array space is limited to 32k, thus you will have to break up large programs or output you code into multiple cut paths in VCarve Pro so you don't run out of memory space when loading the program. (I did testing on my machine some time back, so I was able to pin point the 32,000 line count limitation and confirm it with SCM.)

The Vectric people are really nice and helped me a ton when I was starting out. They don't know much about commercial machines like the SCM's, but they will try to help.

I've only used offsets at run time in Xilog3. You can input the X,Y,Z offsets for the material just before you run the program. I know there is also a X and Y offset on the material setup tab in VCarve, but I haven't needed to use that as most of my work is panel processing / sheets and I typically start at the lower left corner or work x=0 y=0. I have a SCM Routech Record 130 and use VCarvePro.