Content Preview
TB128 Rev1 Gang Tooling
Overview
Setup for Gang Tooling use With these settings you will not have to press cycle start after each tool change and the spindle will stay
running at speed during the tool change Â
Software Version
It is recommended to use the latest version of operating and programming software available so that you can make use of the latest
time saving features V 8 11 has added specific changes to the Tool library which improve the ease of use for Gang tooling We
recommend 8 11 or higher Â
Procedure
To set the control configuration up for gang tooling
Update your control software to the latest version If the control software is not at Version 8 11 or higher update the system Note to
find out what version you have press F1 Setup from the main screen and the version number will be displayed Â
Once the control software is at 8 11 or higher set the parameters below to the following values in the control config parameter screen
To get to the parameter screen F1 Setup F3 config F3 parameters Â
Set Parameter # 163 = 1
This turns on the gang tooling function in the tool library Â
Parameter #1
Parameter 1 tells the control from which direction the reference tool is approaching the work from and changes the
graphical displays to show if the reference tool is front or rear mount If the reference tool is approaching from the front then Parameter
#1 should be set to 1 If your reference tool is approaching from the back then set Parameter #1 to 0 See "Configuration" Chapter 14
of the Lathe Manual for more information about Parameter #1 Â
Set Parameter #6 = 1
This makes ATC F7 key available for tool changes and when running a program it will NOT stop and ask the
operator to press CYCLE START to continue when a new tool is called out in the program The Auto Tool Changer unlock code #203
has to be unlocked when parameter #6 = 1 Â
Create a file CNC7 TCH
in the c \CNC7T directory in CNC7 software Â
 or CNC10 TCH
in the /cncroot/c/cnc10t directory in CNC10 software
 or CNCTCH MAC
in the /cncroot/c/cnct directory in CNC11 software that consist of this one line
M99 Â
Use the DOS editor or the built in editor in the control software or you can create the file on another computer and copy it into c \cnc7
directory Â
When using INTERCON to program parts go to "F10" Setup from the main screen of Intercon and select Â
"Use G28 for tool change" = NO Â
This tells INTERCON not to use the G28 command when programming a tool change G28 is a clearance point used for a position to
retract to when using a turret style automatic tool changer Since with gang tooling a "safe" return point will be different for each tool
you do not want to use the G28 return point with a gang tooling setup It is up to the programmer to program in the clearance moves for
each tool before the tool change takes place Â
Now you are ready to set up tools
Go to the tool library and you will see a column where you can select whether or not a particular tool is coming into the work from the
Front or the Back
Set each tool to its proper approach from "Front" or "Back" setting Â
EXAMPLE Tool Library
Tool Coolant Station Approach Description
T01 Flood 01 Back
T02 Flood 02 Front
T03 Flood 03 Front
T04 Flood 04 Back
T05 Flood 05 Front
T06 Flood 06 Back
T07 Flood 07 Back
T08 Flood 08 Front
T09 Flood 09 Back
T10 Flood 10 Front Â
Now set the Nose Vectors for each tool Look at the nose vector diagram in the tool library and pick the number that matches the
direction that the tool will be approaching the work piece See "Setting the Nose Vector" in Chapter 3 of the Lathe Manual for more
information about setting nose vectors Â
EXAMPLE #1 Reference tool is Rear Mounted Parameter #1 = 0 OD straight in with back approach is Vector #8 and OD straight in
with front approach is Vector #6 ID straight in with back approach is Vector #6 and ID straight in with front approach is Vector #8 Â
For more information on selecting nose vectors see "Setting the Nose Vector" in Chapter 3Â
Set the tool offsets like the lathe manual describes in Chapter 3 Â
While programming parts using gang tooling it is up to the operator to "clear" the current tool before changing to the next tool For
instance after a canned turning cycle the end point of the cycle is the same as the start point in other words the tool starts and stops
at the same location Before changing to another tool the next step in programming would be to add a few lines to clear this and
other tools away from the work piece Once the tools are clear and away in a position ready to change tools then the tool change can
be programmed to take place Â
Advice Study the graph carefully before cutting a part to verify that you have set up the tools properly and have programmed it
correctly You may want to cut a few parts in plastic to verify your offsets and programming Â
If using Intercon v7 13 or earlier to program a part by default Intercon will command a G28 Return to Reference Point for each tool
change You will have to edit the g code to remove this G28 if you are using Gang tooling On version 7 14 and later use of the G28
command is user selectable in Intercon and can be turned on or off To turn off G28 go into Intercon select F7 Setup scroll down and
toggle the G28 command to "off" Â
Intercon verisions prior to V8 10 did NOT support cycles approaching on the negative side of the part If the program was written
manually in G Code or posted using third party software it will work Â
The Auto Tool Changer unlock code #203 has to be unlocked for a gang tooling setup Call your dealer to purchase the ATC unlock
code if you don't have it already
Document History
Rev1 Created on 0000 00 00
by #240