Cutviewer mill user guide v3

CutViewer Mill V3.1
Copyright © 2010 LAMSON GLOBAL CORPORATION
Introduction
What is CutViewer Mill?
CutViewer Mill V3.1 is an easy to use program that graphically displays the
material removal process for milling/drilling operations in 2, 2.5, or 3 axes.
Based on the stock statements and tool definitions, CutViewer will show you
exactly what material will be removed from a raw stock.
What Hardware does CutViewer Require?
CutViewer is a 32 bit application. It runs in Windows 95/98/ME/NT/2000/XP.
The hardware minimums include a Pentium processor, 64 MB of RAM, 100 MB of hard
disk space, and a video graphics card with at least 2 MB of video RAM.
Display Settings
Before running CutViewer, set the Windows Color Palette to 16-bit mode (65535
colors) or higher.
Evaluation Version
The CutViewer download is the full version with a 30 day time limit. After that
time a license serial number is required to continue using the software. To
obtain a license go to http://www.cutviewer.com
CutViewer Features
CutViewer can open and display Standard ISO G-code files. We can also provide
upon request, a special .dll file that enables it to read any control.
CutViewer provides easy real-time manual editing and verification of the
program file, viewing the process from different viewpoints of the part,
measuring the finished part, collision detection, and many other features.
The post reader can be user customized for your specific CNC hardware.
The raw stock can be defined as either a squared block or a cylinder. Stock
and tool data can be included in your CNC program, or defined separately prior
to running the program.
This version supports the following types of tools:
• Ball End Mill
• Bull End Mill
• Flat End Mill
• Tapered Mills
• Chamfer Tools
• Drills
• Center Drills
The ball mill tool can be used with control points on either the ball surface
or on the ball center.
Running CutViewer
When you first open CutViewer it appears as a reduced size window. You can
maximize the main window but take into account that window size affects the run
speed.
Screen layout contains the Edit Window and 1, 2 or 4 Graphics Output Windows
(GOW). The GOW’s are the graphical output areas for simulation, i.e. the views.
Up to four different views can be represented at the same time. The graphic
window with the focus is identified by blue borders.

You can change the number of GOW’s (1, 2, or 4), the orientation of GOW’s
(Vertical or Horizontal) and Edit window position (Top, Bottom, Left, Right)
via Setup mode. The pictures below show some possible screen layouts.
Edit Window Position=Bottom Edit Window Position=Right
Number of views=2 Number of views=1
GOW Orientation=Vertical

Edit Window Position=Left Edit Window Position=Top
Number of views=2 Number of views=2
GOW Orientation=Horizontal GOW Orientation=Vertical
After starting CutViewer only the File-New, File-Open, and Setup items are
available. All windows are empty when they appear. To load a file, select the
Open File button and navigate to the desired directory. Select the appropriate
filter in the «File of types» combo-box to tell CutViewer which configuration
to use to interpret the g-code.
*Important: selecting wrong configuration causes incorrect simulation (e.g. if
you open Fanuc NC file selecting Heidenhain configuration).
If stock and tool information has not been added to the NC post file before
hand, a series of dialogs will prompt you to define them when the NC file is
loaded. CutViewer maintains tool database files in the CutViewer directory for
each type of tool you choose to save there. These tool database files have a
*.db3 extension. You can store and retrieve these tools for use in all of your
simulations.
When finished, the Editor window will display the NC file and a shaded Stock
will be shown in the Graphic Windows.
Each graphic window has its own settings. You can change these settings through
the window popup menu (in order to open this menu the user should click with
the mouse right button somewhere on the window area).

The popup menu for graphic windows provides the possibility of making window-
related settings.
One of the following views can be selected for each graphic window:
Top
Left
Right
Front
Rear
ISO
The «Show Tool path» menu item activates and deactivates the output of the line
graphics for the toolpath. The «Show Toolpath» command will not take effect
until the simulation has been started or one of the view items has been
selected.
The «Show Tool» menu item activates and deactivates the output of the tool
graphics.
The «Show Program Origin» menu item activates and deactivates the output of the
Program Origin graphics.
The current state of the window settings is indicated by the checkmark at the
appropriate menu item.
Press the «Run» button to start the simulation. To make the on screen cutter
speed slower you can define «Dwell» value (milliseconds) in «Setup» mode and
the process will be suspended for the specified dwell time at every screen
point of the tool motion.
To make the cutter move faster during processing simply press '+' key
and press the '-' key to slow it down. Press «PgUp» key for the fastest cutter
speed.
There are two modes of simulation accessible through Setup:
1. Solid: Graphically simulates the material removal process by updating the
stock solid shape as the tool moves (by default).
2. Turbo: Graphically updates only the toolpath with the tool image (if «Show
Toolpath» and «Show Tool» were activated). The machined part appears only after
reaching the end of NC file or when the user presses «Step Forward», «Pause» or
«Stop» button.
If you want to create new NC program directly in the CutViewer select the
«File-New» menu item, then select the desired CNC type and an empty Noname.nc
file will be loaded to the Edit window. Now you can type the program. To save
new program to the disk select the «File-Save as» menu item. To simulate new
program select the «Run-Rebuild» menu item or simply press Ctrl-F9. If Tool or
Stock info are ommited then CutViewer will initiate the appropriate dialog
prompting for missing info.
The following buttons are available at the Main Toolbar:
Open File
This is for opening NC file from a folder or across network. But make sure you
select the appropriate filter in the «Files of type» combo-box to tell
CutViewer which configuration to use to interpret the g-code.

Reset
Resets the simulation showing the initial Stock at the start position.
Run
Press this button to start the simulation.
Step forward/backward
Switches to step-by-step mode, as this button is pressed repeatedly, the tool
moves incrementally forward or backward. When in Step mode, the line being
executed will be highlighted in the Edit window and a separate dialog will
display the current coordinates and cutting parameters. This helps in
identifying the lines to edit. To cancel the incremental trace mode press the
«Run» button.
Note: you can simply press the «Space» key to switch to step-by-step mode
during execution. Also you can use the «arrow» keys instead of the «Step»
buttons when step-by-step mode is active. The tool will move incrementally
forward if you press «Down» or «Right» key and the tool will move incrementally
backward if you press «Up» or «Left» key. Press «Return» key to cancel the
incremental trace mode and continue execution or Press «Esc» key to stop
execution.
Pause
Suspends execution. While processing is paused, you may apply zooming, measure
the part as well change the Setup parameters and EDIT the code. The «Run»
button will restart simulation from the paused position with provision for new
parameters. You can also edit the file, but you have to select the «Run-
Rebuild» menu item or press Ctrl-F9 in order to implement the changes.
Stop
Stops execution of the simulation. Unlike «Pause», you cannot restart from the
current position after pressing «Stop». Pressing «Run» following «Stop» will
start the simulation from the beginning of the file. Also press «Run» following
«Stop» if you want to restart process after finish of the simulation. The
simulation will be started keeping the latest scale for each graphic window. If
you want to start with the initial scale press the Reset button.
View buttons
Press the appropriate button to set the desired view for the graphic window
that has a focus (this window is identified by blue border).
’Parallel to Axis’ sectioning
Generates a sectioned part slicing it with a plane parallel to the Axis.
‘Through 2 points’ sectioning
Allows you to cut away a portion of the part through any vertical plane defined
by two points.
Unsectioning
Press this button to restore the sectioned part.
Zoom Window

Allows for the zooming by a window or region selection method. To use this
function, click the button and while holding down the left mouse button select
the desired window and then release the mouse button.
Zoom In
Press this button and then press the left mouse button at the desired point to
Zoom in on a part. Press the right mouse button to leave Zoom In mode.
Zoom Out
Press this button and then press the left mouse button to Zoom out on a part.
Press the right mouse button to leave Zoom Out mode.
Zoom Restore
Reverts to the initial zoom view.
Pan
Moves the part within the window. Press the button, and then hold the left
mouse button down while moving the mouse. When the view is in the desired
position release the mouse button. Press the right mouse button to leave Pan
mode.
Rotate
Rotates the view. This mode is available for ISO view only. Press the button,
then hold the left mouse button down while moving the mouse. When the view is
in the desired position release the mouse button. Press the right mouse button
to leave Rotate mode.
Measurements
Displays a tool for making measurements of the part.
Setup
Launches a dialog where you can configure how CutViewer works. If you press the
save button to exit rather than the OK button your settings will be the default
the next time you launch CutViewer.
Tool and stock definition
As CutViewer loads an NC file, it looks for information about the stock size,
tool geometry and program origin placement relative to the stock origin. This
requires the addition of several lines to the NC file. If these lines are
omitted from the NC file, CutViewer will initiate a sequence of dialogs
prompting for the missing information. If you prefer to insert the lines
manually follow the directions below:
Each NC file must contain following additional lines: STOCK, FROM, and TOOL.
Tool, Stock and From definition lines should be prefixed with a semicolon, left
parenthesis or the character your CNC controller uses for a comment line.
The stock shape may be a Block or Cylinder with a bore.

The line format for a Block is described below:
a) ;STOCK/BLOCK, Length, Width, Height, Origin X, Origin Y, Origin Z
The first three variables are the stock size, given in positive numbers
representing the actual measurements of the material. The stock reference point
(origin) is the lower left corner in the isometric view (the point with the
minimal X,Y,Z coordinates) . The Stock origin also can be identified by the
intersection of the yellow, blue and red axes when the rotate (view) button is
pushed. The last three numbers indicate the x,y,z position of the program
origin relative to the stock origin. This definition provides more control than
assigning z=0 at the top surface of the block, it also requires more attention.
For example, if the stock has a length of 100 mm, a width of 70 mm, a height of
30 mm and the program origin is at center of the top face:
;STOCK/BLOCK,100,70,30,50,35,30
Similarly, a 6»x4»x1» stock with a program origin at the center of the top
surface is written as:
;STOCK/BLOCK,6,4,1,3,2,1
If the stock shape is a Cylinder with a bore:
;STOCK/CYLINDER, D1, D2, Height, Origin X, Origin Y, Origin Z
D1 is Outer Diameter
D2 is Inner Diameter
The inner diamter D2 may be 0. Diameters and Height represent the actual
measurements of the cylinder. The stock reference point (origin) is the center
of the cylinder bottom.

For example, if the cylinder has a diameter of 100 mm, a height of 30mm and the
program origin is at center of the bottom face:
;STOCK/CYLINDER,100,0,30,0,0,0
If the program origin is at center of the top face:
if the cylinder has a bore diameter 40 mm:
If you start the program with the wrong Stock parameters you can re-deine the
stock selecting the «Redefine a Stock» menu item from the Edit window popup
menu or simply pressing Alt+S and the Stock definition dialog will appear.
b) ;FROM/X start, Y start, Z start
The FROM line denotes the starting or home position of the tool relative to the
program origin. In this example using the stock above and the initial position
of the tool 10 mm above the top face:
;FROM/0,0,10
The inch example, if the first tool position is .1» above the origin:
;FROM/0,0,.1
c) The TOOL line denotes the tool geometry.
The line format for Mills is described below:
;TOOL/MILL, Diameter, Corner radius, Height, Taper Angle
*Note: for Tool/Mill: the Corner Radius will indicate the type of mill used
where 'r' is the corner radius specified and 'D' is the tool Diameter:
r=0 for a flat end mill (Fig.1)
r<D/2 for bull end mill (fig.2)
r=D/2 for ball end mill (if the control point is the tool tip) (Fig.3)
r=-D/2 for ball end mill ( if control point is the center of the ball) (Fig.4)
The following are Examples of various tool settings:
;TOOL/MILL,20,0,80,0 ;TOOL/MILL,1,0,1.5 - flat end mill
;TOOL/MILL,20,10,80,0 ;TOOL/MILL,1,.5,2 - ball mill (control point is the
tool tip)
;TOOL/MILL,20,-10,80,0 ;TOOL/MILL,1,-.5,2 - ball mill (control point is the
center of the ball)
;TOOL/MILL,20,3,80,0 ;TOOL/MILL,1,.125,1 - bull mill
The line format for Chamfer tools is as follows:
;TOOL/CHAMFER, Diameter, Point Angle, Height

or
;TOOL/CHAMFER, Diameter, Point Angle, Height, Chamfer Length
The line format for Drill is described below:
;TOOL/DRILL, Diameter, Point Angle, Height
And the line format for Center Drills is as follows:
;TOOL/CDRILL, D1, A1, L, D2, A2, H (see Fig. below)
*Note: You can insert a new tool into the NC file at the needed position. To
get the Tool definition dialog choose «Insert Tool definition» from the Edit
window context menu. After a Tool line is inserted, you have to select the
«Run»-»Rebuild» menu item or press Ctrl-F9 in order to implement the changes.
You can add a new tool to the tool database. Simply press the «Add tool to DB»
button from the Tool definition dialog. Afterwards you can get the tool from
this database pressing the «Get Tool from DB» button.
If you have the tool database then you can use the following syntax for the
Tool definition command:
;TOOL/ID=……
or

;TOOL/ Description=………
In this case CutViewer will use the tool from the database with given «ID» or
«Description» value.
d) ;COLOR,R,G,B
You can assign display color to each tool. This must follow the TOOL
Command.
R - specifies the intensity of the red color
G - specifies the intensity of the green color
B - specifies the intensity of the blue color
The intensity for each argument is in the range 0 through 255.
If all three intensities are zero, the result is black.
If all three intensities are 255, the result is white.
For example, you may type the following:
;COLOR,0,255,0 - Display Color is green;
or
;COLOR,255,255,0 - Display Color is yellow;
Note: CutViewer inserts Color line automatically if you use Tool definition
dialog. You can change Display Color for each tool pressing the color
assignment button in «Setup» mode or directly using a simple key-combination
«Ctrl-T». To change the color, simply click on the appropriate cell in the
«Color» column.
Note: Any leading symbols are permitted, provided they do not interfere with
program execution.
For example, you may type the following:
;FROM/120,0,0
or
$FROM/120,0,0
Stock / Tool selection in CLS and APT CLDATA (ASCII) files:
Each file must contain information about stock in following format:
PPRINT/BLOCK,d1,d2,d3,d4,d5,d6
or
PPRINT/CYLINDER,d1,d2,d3,d4,d5,d6
d1,d2,d3,d4,d5,d6 - see G code section
For example:
PPRINT/BLOCK,100.,70.,30.,50.,35.,30.
Information about tool for CLS files:
TLDATA/MILL,D,r.... = mill
TLDATA/DRILL....... = drill
Information about tools for CLDATA (ASCII) files:
CUTTER/D,r
D-tool diameter
r- corner radius
for flat end mill r=0
for ball mill r=D/2
To assign display color to each tool use command:
PPRINT/COLOR,R,G,B

Refer to the demo files for more examples.
Editing
You can modify an NC program in the Edit window, as you would edit a file. All
changes will be accepted only after you select the «Run-Rebuild» menu item or
press Ctrl-F9 for program rerunning.
For program debugging you can select the menu item «Run to Cursor» or simply
press F4 key. The «Run to Cursor» command runs your program from the current
point to the line the cursor is on in the edit window and then switches to the
Step-by-Step mode. For example, if you are checking a large NC file you may
select fast Turbo mode of operation then select the desired line in the edit
window and press F4. When the program stops at selected line you can switch to
the Solid mode and continue processing. You can also use Ctrl-F4 after
modifying the program. This would be the same as «Rebuild» and «Run to
Cursor».
You may also set breakpoints on lines in the NC file where you want the program
execution to pause during a run. Running to a breakpoint is similar to Running
to a cursor position in that the program runs until it reaches a certain line.
However, unlike «Run To Cursor», you can have multiple breakpoints in your
file. To set a breakpoint, select the line in the file where you want the
breakpoint set, then do one of the following:
a) Press F5
b) Choose Toggle Breakpoint from the Run menu
c) Choose Toggle Breakpoint from the Edit window context menu.
When you set a breakpoint, the line on which the breakpoint is set becomes
highlighted.
*Note: you can select Edit commands through popup menu. In order to open this
menu the user should click with the mouse right button somewhere on the Edit
window area.
Zooming
Use one from the following buttons for zooming:
Zoom Window
Allows for the zooming by a window or region selection method. To use this
functions click the button and while holding down the left mouse button select
the desired window and then release the mouse button.
*Note: The resulting part will be sectioned because of memory restrictions and
for faster processing.
Zoom In
Press this button and then press the left mouse button at the desired point to
Zoom in on a part. Press the right mouse button to leave Zoom In mode.
Zoom Out
Press this button and then press the left mouse button to Zoom out on a part.
Press the right mouse button to leave Zoom Out mode.
Zoom Restore
Reverts to the initial zoom view.

View Rotation
For view rotation press the 'Rotate' button. To rotate the view, hold the left
mouse button down while moving the mouse. When the view is in the desired
position, press the right mouse button to leave «Rotation» mode.
*Note: you can enact the «Rotation» command directly using a simple hot key
without pressing a button. Press the Alt key and click-drag with the left mouse
button.
View Panning
For view panning press the «Pan» button. To pan the view, hold the left mouse
button down while moving the mouse. When the view is in the desired position,
press the right mouse button to leave «Pan» mode.
*Note: you can enact the «Panning» command directly using a simple hot key
without pressing a button. Press the Ctrl key and click-drag with the left
mouse button.
Sectioning
The part can be sectioned to see invisible elements. CutViewer supports two
modes of sectioning, «Parallel to Axis» and «Through 2 points».
«Parallel to Axis» generates a sectioned part slicing it with a plane parallel
to the Axis. Press the «Parallel to Axis» button and an outline of the top
edges of the stock will appears. Place the mouse cursor on one of the lines
and drag it to the location where you would like to see the section cut. When
you release the mouse an outline of the section will appear below the line. You
may move the section line again with the mouse. Repeat this for other edges if
necessary. When finally satisfied, press the right mouse button to create the
section.
«Through 2 points section»- allows you to cut away a portion of the part
through any vertical plane defined by two points. This option is available
only on the Top and ISO views. Move the cursor to the first position and press
the left mouse button down. While holding the button pull a «rubber band line»
to the desired position. Release the mouse button and correct the position of
the points as necessary. When you are satisfied with the position of the
section line, move the cursor to the side of part you want to remove and press
the right mouse button.
To restore the sectioned part press the «Unsectioning» button or choose the
menu item «Section», «Unsectioning».
Measurements
A tool has also been supplied for making measurements of the part. For making
measurements press the «Measure» button» and then press the appropriate button.
The most of measurements are available on the Top view only.
To build sections through vertical planes press the «Measure»-»Section» button
and input explicit coordinates of the first and second points and step value or
move the cursor to the first position and press a left mouse button down.
While holding the button pull a «rubber band line» to the desired position.
Release the mouse button and correct the position of points as necessary. When
you are satisfied with the position of the section line, press the right mouse

button and input a step value in the dialog box. The section will appear on
the screen. You can see real coordinates in the X,Y,Z box by clicking at a
point of the section. You may zoom in on a section .You may also choose the
«coordinates» page and save X,Y,Z values in the file.
*Note: The values of PART and REMOVED VOLUMES are approximate and relate to
current display representation of the part (taking into account all sections).
STL Compare» function allows the user to perform a check of the cut model to 3D
CAD model in STL format. For making comparison press the «STL Compare» button.
The STL Compare dialog box appears. Load the STL file. You can see the
following fields and the buttons:
dx,dy,dz and xa,ya,za are used for setting the STL orientation relatively to
the program origin.
dx,dy,dz indicate the STL origin relatively to the program origin.
xa(ya,za) indicates the angle of STL rotation around the X(Y,Z)-axis. Press
the «Show STL» button to show STL model and to make certain of STL position and
orientation.
InTol - the tolerance value for the gouges.
OutTol - the tolerance value for the uncut areas.
Press the «Start» button to begin the comparison.
The process is slow, especially for big STL files. The gouges will be displayed
in Red, uncut ares - in Yellow, and all area's within
tolerance - in Green colour. You can change the colours pressing the
appropriate coloured buttons and choosing desired colour.
Settings
Through the «Setup» button you can change and save the following parameters:
Mode of Simulation
1. Solid: Graphically simulates the material removal process by updating the
stock solid shape as the tool moves (by default).
2. Turbo: Graphically updates only the toolpath with the tool image (if «Show
Toolpath» and «Show Tool» were activated). The machined part appears only after
reaching the end of NC file or when the user presses «Step Forward», «Pause» or
«Stop» button.
Autosave options
specify which options are saved automatically when CutViewer is closed. A check
mark means it is enabled.
- Main window position: if checked then main window size and position are
saved.
- GOW settings: if checked then settings for each graphic windows are saved.
Edit window position: setting position of the Edit window in the main program
window.
Screen layout settings
specify the number of graphical windows(1,2 or 4), edit window position
(left,right,top,bottom) and GOW orientation (Vertical or Horizontal).
Check Rapid Collision
enables or disables the detection of Rapid Collision. If this option is on then
CutViewer graphically simulates any collision the tool has with the stock
material while under Rapid Traverse. Execution of the NC file will stop at the
block of code where the collision occurs and a special dialog box will also
appear that will display the coordinates for the current type of move in a
from-to format and the buttons to define next actions. You may continue
execution, pause or stop it. If you press the «Ignore All» button then
execution will continue but without any Rapid Collison detections or in other
words the option «Check Rapid Collision» will be Off. That’s why don’t forget
to turn «Check Rapid Collision» to On if you want to have this feature beeing
available for further simulations in the same session.

Dwell (milliseconds)
specifies a dwell at the every screen point of tool motion for slowing the on
screen tool speed
Trace step
specifies an amount of the tool motions for the Trace mode when the tool moves
incrementally
Tool View
specifies Solid of Wireframe mode for the tool image
Colors
setting the color palette.
*Note: When CutViewer loads NC file, it creates a record in memory of any tool
size or tool color statements that have been inserted where the tools take
effect. A different color statement can optionally follow each tool definition.
If no color statements are found in the post, CutViewer uses the «Part color»
shown in the Setup dialog. Changes made to tool colors by means of the setup
dialog will persist only if there are no colors assigned in the NC file. A
Ctrl-T key combination will directly launch the tool color dialog.
Reloading the NC file (Rebuild – Ctrl-F9) will cause the program to use any
colors added to the editor buffer and override changes made in memory through
the setup dialog. Once the NC post is loaded into memory the tool colors can be
changed in the setup and seen immediately.
So, for a permanent color update we should add COLOR commands to the NC file.
Customizing
CutViewer uses a simple text file with an *.nci extension to configure
CutViewer for specific style of post. The nci file uses the same format the
common .ini file. These files are kept in the CutViewer install directory. The
*.nci configuration file defines the extension filter and description that
appears in the combo-box in the open file window. The extension filter can be
used to limit viewing only those files for which the configuration file is
correct.
The default configuration file called _gcode.nci may be found in the CutViewer
directory. If you have only one NC machine simply edit this file. If you
start by editing the default file it would be a good idea to save the original
before editing.
Several sample *.nci files are provided with the program and can be used to
view some demo posts. Move any move any of these sample nci files to another
directory to shorten the list of choices in the file open combo-box.
If you have several machines, make copies of _gcode.nci under different names
in the CutViewer directory and edit these files. Notepad or WordPad can be
used to edit them. When saving these files, make sure the file is saved as
FileName.nci and not as FileName.nci.txt (Notepad is notorious for this).
Note: A backup of the default _gcode.nci is also found under the name
_gcode.def.
To load an NC file into CutViewer you must select the correct configuration
file from the «Files of Type» combo-box in the file open dialog when you load a
file.
Creating new NCI files
There are two required sections in this file:
[Common]
[Format]

NCI files are not case sensitive. Only the settings that are used by your
program need to be in the file.
Comments have been added above each setting in a different font to show that
they are not needed in the file.
A sample nci file looks like this:
[Comments]
A description that, when seen in the combo=box, will help describe what kind of
post the configuration is for.
CNC=Fanuc OMC
The extension filter, which is used by the open file window to filter the file
list, should be the same as what appears in you NC post filename.
FileExt=*.nc
Note: multiple extensions are allowed. Example: FileExt=*.nc;*.cnc
The character that the post uses before a line that tells the machine
controller not to interpret that line is,
Comment_chr=(
The word Inch or Metric, depending on which unit scheme will be used in the NC
post file.
Units=metric
[Format]
The next 3 settings define the coordinate symbols
x_addr=X
y_addr=Y
z_addr=Z
The next 3 settings define the ratio X,Y,Z value in NC file to actual
value of X,Y,Z coordinates:
x_scale=1
y_scale=1
z_scale=1
The next two settings define how arc centers are read when either G90 or G91 is
active and only apply to a G02/G03 line that has a center defined with I J K
words but not when X Z R is used.
IJKformat_abs=
IJKformat_incr=
There are exactly 5 different string values that can be used with each:
I and J are absolute
Center.
I and J are incremental from the XY end point of the arc
end-center.
I and J are incremental from the start point of the arc
center-start.
If the control expects that incremental centers are always a positive number an
«abs» is added.
abs(end-center)
abs(start-center)
If G90 active

Ijkformat_abs=
If G91 active
Ijkformat_incr=
Example:
IJkformat_abs=end-center
IJkformat_incr=abs(end-center)
The feed rate symbol
f_addr=F
The RPM symbol
s_addr=S
The tool symbol
tool_addr=T
The feed rate that above which rapid color is displayed and collision is
expected if the cutter has met material.
f_rapid=5000
Cutter compensation g-codes.
cutcom_left=G41
cutcom_right=G42
cutcom_off=G40
Please note that if your CAM system is posting profiles using the cutter
centerline instead of the part profile, each one of these should be set to
«Gxx» so that they are ignored when encountered.
The end of the main program
prog_end=M30
Sub routine call
sub_call=M98P
Begin sub definition
sub_begin=O
End sub definition
sub_end=M99
Sub repeat character
sub_repeat=L
example of a _gcode.nci file :
[common]
CNC=Standard G-code
fileExt=*.nc
comment_chr=(
units=metric
[format]
x_scale=1
y_scale=1
z_scale=1
f_scale=1
s_scale=1
IJkformat_abs=center-start
IJkformat_incr=center-start
x_addr=X
y_addr=Y
z_addr=Z
f_addr=F
s_addr=S

tool_addr=T
f_rapid=5000
cutcom_left=G41
cutcom_right=G42
cutcom_off=G40
prog_end=M30
sub_call=M98P
sub_begin=O
sub_end=M99
sub_repeat=L
Custom Control Conversion
Some CNC have the canned cycles and special functions that can’t be defined via
variables in NCI-file. In this case the user should develop his own converter.
If there is the following line at [format] section in the nci-file:
user_convert=mycoverter.dll
then first of all CutViewer will try to call the procedure named
User_convert_proc from myconverter.dll file. User_convert_proc procedure has
2 parameters - input file name and output file name. These parameters
CutViewer passes to your procedure. If you write your programs on Delphi the
declaration for the procedure in DLL looks as follows:
Procedure user_convert_proc(infile,outfile:pchar);stdcall;
Input file is NC-file to be converted and output file is a result file with
standard G-codes. In other words CutViewer calls the procedure Procedure
user_convert_proc passing 2 parameters and expects that your procedure will
create output file with the name passed by «outfile» parameter and then
CutViewer handles this file as usual. There is one rule for output file.
Every line in this file should be prefixed by number and «#» symbol.
Example:
.....................
10# G01 X1 Y1
11# G00 Z5
14# T1
15# G01 X1 Y0.5 F2
............................
Number before «#» symbol means that current line in the output file is
corresponding to the line in input file with the index defined by this
number (first line in the input file has the index 1) .
Let me explain.
We should convert NC-file for hypothetical CNC that has the following
format:
TOOLNO, 1
SPINDLE, 500
RAPID
GOTO/X=1,Y=2,Z=5
FEEDRATE, 20
GOTO/X=1,Y=2,Z=1
FINI
This is the input file. Our procedure creates the appropriate output file
with the following standard G-codes:
1# T1
4# G00 X1 Y2 Z5 S500
6# G01 Z1 F20
7# M02

You see that number before # is the appropriate line index for input file.
CutViewer needs this index to provide correct cursor navigation in the edit
window during step-by-step mode because the first file will be loaded into the
edit window but in fact internally CutViewer works with the second file.
The algorithm how to convert input file into output file or in other words
the program code inside the procedure is your responsibility and of course
this file in details can be different for different developers. For example
you can create the following output file in our case:
1# T1
2# S500
4# G00 X1 Y2 Z5
5# F20
6# G01 X1 Y2 Z1
7# M02
You can also create exe file instead of DLL and the line in NCI-file in
this case is as follows:
user_convert=myconverter.exe
In this case at first CutViewer runs myconverter.exe file and passes 2
parameters through command line (input and output file names). Your program
should accept these parameters and create the appropriate output file.
Contact points
For questions and orders please contact:
LAMSON GLOBAL CORPORATION
Web Site: http://www.cutviewer.com
Email Sales: sales@cutviewer.com
Email Support: support@cutviewer.com
About Register
The evaluation version of CutViewer only functions for 30 days.
To purchase CutViewer and deactivate the 30 day limitation contact...
LAMSON GLOBAL CORPORATION
Web Site: http://www.cutviewer.com
Email Sales: sales@cutviewer.com
Email Support: support@cutviewer.com

Cutviewer mill user guide v3

More Related Content

What's hot (20)

Similar to Cutviewer mill user guide v3 (20)

Recently uploaded (20)

Cutviewer mill user guide v3