Hi guys I need some help with Z offsets on my old T1 QT10. My machine has no toolsetter. What exactly should I be doing with Z offsets to be most efficient in setting up jobs and switching between jobs?
The first few jobs I did I set Tool 1 with a Z offset of 0, cut a face and measured the difference with other tools and adjusted them to be the same. This worked but its very slow, there has to be a better way.
Today I tried to touch all tools off a common face (lets say chuck face) and use the teach function which stores the machine position for each tool. This seems fine, but when I run a program the machine now thinks the tool is very long and it moves a mile away from the face of part to change tools. It actually wants to go a couple inches past home position and over travels. There is a parameter to change tools at home position but this would waste a lot of time. Any suggestions?
My QT-10N (T2 control) did not come with a tool setter. Presumably someone crashed it and removed it.
So I have been running without the tool setter and have figured out a method that works. It should be similar for the T1 control.
You need to zero your tools with respect to the program zero (Z offset) you entered in the "program file" page.
In the tool-setter manual for the machine, there's a drawing with the location of the tool-eye. Get that number if you can.
With my Hardinge A2-6 collet nose, the tool eye would have been about 100mm (3.937") away from the collet face.
So one of my programs has a Z offset of -.5" (That is, from the tool-eye location to the Z zero of the part).
This part starts with 3.550" of material hanging out of the collet when I start.
Once I have that program set up as described, I manually switch to my first tool (CNMG 432 in a standard holder).
I use a steel rule to manually move that tool to 3.5" from the collet face.
I go to the "tool-set" page and press "Teach". Before pressing input, I key in the program Z offset.
This will correctly zero the tool. For this example, I press "Teach" and key in -.5, then input.
Next, go to "trace" page, or "command" page to verify that the tool Z is actually reading zero.
Now I turn on the spindle and face off that bar using the jog mode in X.
After that, I stop the spindle and touch off each tool for the job on that same face.
I have to press "teach" and key in the program Z offset for each tool before I hit input.
Using this method, you don't have to re-zero tools between jobs unless you change the tool.
The way it works is that you know a program with 4" of bar sticking out of the collet is an offset of zero.
Each inch you subtract from that stickout has to be accounted for in the Z offset for the program (program file page).
Also, each inch you add to that stickout has to be accounted for in the Z offset for the program (program file page).
SO your tools are now zeroed ≈4" (100mm) away from the collet nose or chuck, but this may vary depending on your chuck/collet system.
The diagram below has the correct Z dimension of 336mm from the headstock to the centerline of the tool setter.
This dimension would also be a program Z-offset of zero.
Here's the drawing from the QT-10N manual... This is for the 8D and 6D turret on the universal machines.
(There are actually different dimensions for max tool length and such depending on the turret, etc.)
Hopefully that all makes sense, but if not I'll clarify any questions.
I just purchased a used tool-setter and will have it on the machine soon.
I had planned to build one, however I came across a good deal on a complete unit for my machine.
If you can't find one, consider bending or welding up some steel tubing and mounting an indicator on the end.
If you make a taper-socket that bolts to the headstock, you can just leave a dedicated indicator on that "arm" and set it to tool-zero.
You'd have to put it in the taper-socket each time you want to measure a tool, but it would speed things up a bit.