First, boring legal stuff. I accept no liability for any damage, injury, or loss of life that results from the use of this program or information. I am providing this program and information free of charge. It is the responsibility of the operator to ensure that their machine is used safely, and that it will work correctly with this program.
This is a simple script that handles tool changes for a Tormach mill running in vertical lathe mode with gang tooling mounted to the table. I have tested it in the following scenario. It may work for other configurations too.
Tormach 1100 mill.
Unlocked Mach 3 running a modified Duality configuration.
G-code generated by Sprutcam via the Lathe XY config and Duality post-processor.
Currently, it is necessary to define a work offset for each tool. This takes a lot of time to set up.
You should be able to mount your gang tooling holder to the table, indicate it, and be ready to run. This script makes that possible.
What it does, in plain English.
1. Scan the tool table for tools 1-100.
2. If needed, retract the workpiece above the longest tool.
3. Move to the correct Y value to put the next tool on the spindle's centerline.
4. Move to the correct X value to put the next tool close to the workpiece.
1. You must have an unlocked Mach configuration in order to use this script. If Mach is not unlocked, you won't be able to perform step 3.
2. Use this file to replace your existing M6Start.m1s file. Be sure to back up the old file.
3. Set your tool changer type to Auto Tool Changer. This means that at a tool change, Mach will run this script and not wait for the operator's input.
4. Set up a work offset to a unique point on the gang tooling holder. I recommend picking a corner of the holder and using that as a reference. That will let you quickly find zero on the tool holder when you next install it.
5. Set up your tool table. Enter each tool's X, Y and Z position relative to the unique point. The tool table has fields for X and Z. It does not have a field for Y, so you must enter the Y value into the Turret Angle field. The script will read these values and generate the appropriate moves at a tool change.
Please note that the Y move does not take the form of an offset change. This means that the Y axis DRO will not remain at 0.000 as you would expect. It will show whatever number you have entered in the Turret Angle field of the tool table. And if your program generates any Y axis moves, they will act to move the lathe tool away from the spindle center line.
Mach will accept tool change calls for Tools 1-99, while the script checks heights for Tools 1-100. If you have a fixture on the table that is taller than your tools, enter that fixture's height in the Z offset for Tool 100. The script will retract far enough to avoid the fixture.
[URL="http://www.pure-geometry.com/"]Pure Geometry LLC[/URL]
Vertical Lathe tool holders and more.