What's new
What's new

Need help with Z Offsets on T1 control. Without presetter...

mmurray70

Stainless
Joined
Jan 11, 2003
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?
 
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.)
Tool_Setter_Dims.jpg

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.
 
So you set all your tools with a rule? That gets you close enough? I actually setup an indicator to stick on chuck face and measure tools. See attached pic. Moving to indicator zero and then "tool-set" and "Teach" seemed like it would work. It just saved the machine position when you pressed teach and then as long as you set program Z offset with a touched tool, everything appeared like it would work ok. When changing tools, the right Z values would be displayed relative to a part. Its just the toolchange in auto mode was getting messed up. The controller was applying WAY too much clearance to toolchange when using large numbers for Z offsets.

So I thought about what you do, pushing Teach, keying in a value, then input. And I thought maybe I could add/subtract a constant each time, I could make all the offsets be within a range thats much closer to zero (which toolchanged fine before). I tried this and it it works fine in a simple program with two turning tools and a threading tool. All these have fairly similar offsets anyway. I havent tried it with a drill yet.

So I might have it somewhat working, but Still have no idea how I should be doing this so that the toolchanger clearance is calculated properly. My machine has a weird horizontal turrett too, not alot of room inside. Would be nice if it were figuring out toolchanges properly to avoid a crash.

indicator.jpg
 
So you set all your tools with a rule? That gets you close enough?

Nope. I thought that might be misunderstood.
I use the rule to set the first tool approximately 4" from the chuck face.
I also use the rule to set a piece of bar at 4" out of the chuck face, plus 0.050" extra to clean up the face.

With that first tool set, I face the bar and touch off each tool.

You can zero the indicator based on that first tool, 4" from the chuck.
Now, zero all the other tools to the indicator.

Set your work zero (program file page Z-Offset) as the distance from the tool zero point which is 4" from the chuck face.

If your part Z-Zero is 2.5" closer to the chuck than your tool zero (short part) your Z-Offset for that program is -2.5
If your part Z-Zero is 1.25" farther away from the chuck than your tool zero (long part) your Z-offset for that program is +1.25"


So I might have it somewhat working, but Still have no idea how I should be doing this so that the toolchanger clearance is calculated properly. My machine has a weird horizontal turrett too, not alot of room inside. Would be nice if it were figuring out toolchanges properly to avoid a crash.

The control is setup to be zeroed from the tool-detector position which is shown in the diagram I attached.
The closer you get to that position, the better your life will be. The control calculates all the graphics, tool change position, etc. from that particular point.

If you do it this way, you'll get all of your graphics and all of your barriers working properly, as well as that tool-change position.
Also, you won't have to change tool-offsets for each job and you'll have a known reference for setting your program Z-offsets.

Hopefully I've explained it more clearly...
 
Our QT20 with T1 also doesnt have a presetter. I almost always will take a witness face cut on the material to be machined and teach that as my Z offset. It is usually with my OD roughing tool since it is always in the turret. With the remaining untaught tools I will touch off the witness cut and teach that tool to Z zero (teach+ value of my Z offset position)and immediately go back to my command/position page and verify that the tool reads Z0. Then since I am there already I will take a manual cut on OD/ID and teach the tool for X dia. Once all the tools are taught to your first tool you can use any of them to set your Z offset. The T1 has to be dialed over on Z to move your Z offset where the newer controls have an incremental Z offset feature. One thing to remember is if you set your Z offset with say work #2 first, and then erase that program to make a new part with the same program # your Z offset will be changed and have to be reset. Bad thing is the lathe will still run even though Z offset isn't where you had first established it.
 
Nope. I thought that might be misunderstood.
I use the rule to set the first tool approximately 4" from the chuck face.
I also use the rule to set a piece of bar at 4" out of the chuck face, plus 0.050" extra to clean up the face.

With that first tool set, I face the bar and touch off each tool.

You can zero the indicator based on that first tool, 4" from the chuck.
Now, zero all the other tools to the indicator.

Set your work zero (program file page Z-Offset) as the distance from the tool zero point which is 4" from the chuck face.

If your part Z-Zero is 2.5" closer to the chuck than your tool zero (short part) your Z-Offset for that program is -2.5
If your part Z-Zero is 1.25" farther away from the chuck than your tool zero (long part) your Z-offset for that program is +1.25"




The control is setup to be zeroed from the tool-detector position which is shown in the diagram I attached.
The closer you get to that position, the better your life will be. The control calculates all the graphics, tool change position, etc. from that particular point.

If you do it this way, you'll get all of your graphics and all of your barriers working properly, as well as that tool-change position.
Also, you won't have to change tool-offsets for each job and you'll have a known reference for setting your program Z-offsets.

Hopefully I've explained it more clearly...

Im not sure if my T1 even has a "Tool zero point" like you mention in the diagram. Does a T1 even support a presetter? I dont see anything about it in the manual at all. I just read manual again about setting offsets and it basically says to skim a face and teach that. And when I attempt to do this I get a larger number for my tool offsets (distance from home position), and it messes up toolchange in auto.

If you move close to chuck to Teach a tool without inputing a number what number does it store on your T2? Does it store distance from home or something else? Im guessing on your T2 its probably a distance from that tool setting point in diagram.
 
I just use one of the cheap edgefinders with the led and beep mounted to a magnet. Just sit it on the face of the chuck (I usually put it beside no 1 jaw and set all your tools to that. Then you set your Z zero for whatever program you are running and spot on every time.

Exactly! This is what I was trying to do too, nice and simple and should be very accurate. But some reason its messing up my toolchanges.


Our QT20 with T1 also doesnt have a presetter. I almost always will take a witness face cut on the material to be machined and teach that as my Z offset. It is usually with my OD roughing tool since it is always in the turret. With the remaining untaught tools I will touch off the witness cut and teach that tool to Z zero (teach+ value of my Z offset position)and immediately go back to my command/position page and verify that the tool reads Z0. Then since I am there already I will take a manual cut on OD/ID and teach the tool for X dia. Once all the tools are taught to your first tool you can use any of them to set your Z offset. The T1 has to be dialed over on Z to move your Z offset where the newer controls have an incremental Z offset feature. One thing to remember is if you set your Z offset with say work #2 first, and then erase that program to make a new part with the same program # your Z offset will be changed and have to be reset. Bad thing is the lathe will still run even though Z offset isn't where you had first established it.

Seems like my machine wants to work this way too. Your setting program Z offset with your roughing tool (which has no tool offset) and the other tool offset values will just be the difference from the first tool. My machine runs ok when tools are set like this. But seems like a pain to type in Z offset everytime. And if your depending on previous touched tools to cut a face and set new tools, I can see things drifting off after a while.
 
Exactly! This is what I was trying to do too, nice and simple and should be very accurate. But some reason its messing up my toolchanges.




Seems like my machine wants to work this way too. Your setting program Z offset with your roughing tool (which has no tool offset) and the other tool offset values will just be the difference from the first tool. My machine runs ok when tools are set like this. But seems like a pain to type in Z offset everytime. And if your depending on previous touched tools to cut a face and set new tools, I can see things drifting off after a while.

Just part of the process with a T1. When you do it enough times it becomes less of a PITA.
 
Sorry if I threw in some confusion. I was under the impression that the T2 way would work for T1 also.
Does the T1 lack unique work offsets for each individual program?


Sudsy, the edge-finder is a great idea.
A guy could use that on the turret as a simple work-measuring system too.
 
Sorry if I threw in some confusion. I was under the impression that the T2 way would work for T1 also.
Does the T1 lack unique work offsets for each individual program?


Sudsy, the edge-finder is a great idea.
A guy could use that on the turret as a simple work-measuring system too.

I think the T1 has an individual offset for each program. Not 100% sure. Im using Mazview to store and organize my programs and only download one program to work with at a time.

Thanks to everyone who replied. I did a little more playing around and it seems to be working fine for me to touch off my dial, and add a constant that makes the offset close to zero every time. For example if I touch my roughing tool and teach it and it gives me an offset of -15.162, this tells me most my turning tools are approximately 15" from home. So if I touch ALL my tools off the dial and Teach -15 and then input its gives all the tools an offset value closer to zero and it toolchanges fine. Then you set your work face offset with any measured tool and everythings good to go.

Still not sure if this is the best way, but its fairly quick and accurate so im gonna keep doing this unless I run into a problem down the road or someone points out a better way. Thanks again.
 








 
Back
Top