Tool Touch-Off
CNC operators discuss their preferred methods for touching off tools. November 12, 2005
Question
What is the best way to touch off tools to the spoil board? We use a piece of paper under the tool and keep lowering it until it doesn't move. The problem is we don't have much accuracy between different tools. Is there a better way? We have an Andi Stratos with Fanuc control. This is the method they taught us at training.
Forum Responses
(CNC Forum)
From contributor N:
Without having a machine with a touch off device, you have to set it manually. The paper works, but if you need more accuracy, you can get a XYZ6070 dial indicator. Anderson has them.
From contributor K:
Our Andi Stratos (1 year old) has an automatic touch off device. Maybe it could be added to yours.
From contributor H:
I suggest not using the paper if you have the vacuum turned on, and you should always have the vacuum turned on when touching off tools with a spoilboard in place. The paper sticks, and it is hard to tell if the vacuum is holding or the tool is touching the paper. I feel the best way, unless you have an expensive touch-off mechanism, is to bring the tool over the part of the spoilboard where you are going to touch it off. Then use a black marker and darken an area where the tool will hit the spoilboard. Bring the tool down until you can see very little light between the tool and the spoilboard. You will need to be at eye level with the spoilboard. A flashlight helps. Spin the spindle with one hand, and adjust your z axis with the other - hopefully you have a remote for adjustments. You should be able to see when the tool starts shaving off the black mark. This is what I was taught in grinding class, where .0001" counts, and it has worked for me. I hope it works for you. Have a nice day.
From contributor J:
We set tool length this way: I measure the length with a caliper and enter the value. Then I run the tool over the spoil board set to cut .1mm deep, measure the actual depth of cut, make the adjustment on the screen and I'm done. The whole operation of changing a cutter and setting the new length takes only a few minutes.
From contributor S:
I've used the paper method, the measure and cut, but my favorite is sliding the non-cutting end of a broken tool back and forth under your cutter until it hits. You should always measure the depth of your cut as to variations in material thickness.
From contributor G:
You can do this with a digital tool presetter. With the toolholder in the presetter, put your tool in and you will have your total length. No more tool touch offs.
From contributor M:
Create a program which will cut into a piece of scrap at whatever depth, measure the depth and adjust bit length on the screen. When you want to test a different bit, simply change the tool in the program and run it again. Much faster than manually lowering and raising and it will be accurate first time, every time.
From contributor S:
Materials differ in thickness (3/4 is not necessarily 3/4). So, if I was the operator, I'd start fresh every time.
From contributor J:
Wait a minute. Don't you cut into scrap and measure how much is left over (above 0)? Who cares what thickness the test scrap is?
From contributor S:
You could, if all your tools were the same cutting edge... There's nothing like hitting go and crossing your fingers, hoping you don't slam into the table or a pod. I'll stick to manual touch-offs, thanks.
From contributor M:
The program is set for the same depth regardless of the tool you want to calibrate, say 17mm (of meat leftover). You get close by means of a caliper. The only time you need to mess with this is when you set up a tool, chuck it into a holder and measure it. We cut into our scrap, leaving 17mm. Measure the portion of the board that is left. If it is 17.40, you adjust by .4. It's not like you put the tool in and cross your fingers. You know within 1mm how long the tool is. What you are trying to do is dial it in. Whether your scrap is 18, 19, or 19.5 does not matter because you are measuring the meat leftover. By the way, the route you just ran can also be measured by a caliper for width and you now can make both adjustments at the same time, unless you throw away your bits. The diameter must be calibrated each time you set up a tool as well, which neither the automated method or the paper method do.
From contributor J:
Well said. I didn't have the patience the other night to give such a simple but complete description. Anyone can measure overall tool length with a digital caliper to within 0.5mm - too easy.
Contributor S, how many times have you slammed into a pod? What happened? Did you use a tape measure? My problem is that I'm so busy producing miles of boxes that I can't find the time to turn a cutter change into its own project.
From contributor S:
If all you do is cut thousands of boxes and use the same tools over and over again, you can train a monkey to touch off tools. I'm saying that if you produce for a custom shop and cut materials ranging in thickness from .060" to 3"+, depending on your software/controller, you can't go G43 T1 H1 Z0 and expect the machine to know you just chucked in a 5" tool when H1 was much smaller.
From contributor D:
Contributor S, does your machine have a pc front end? It sounds older, judging by your methods. Perhaps a new machine would require methods similar to the way contributor M explained, no? Maybe the different methods reflect that some people operate new equipment which may be much more simple - tool data bases and all the stuff found on machines with a pc front end - whereas some people are messing with g-code when setting tool length.
From contributor S:
I've programmed and operated quite a few different routers - flow through and PTP. The method contributor M explained would apply to a PTP where you may measure from the bottom to the top (the material left over). I am not sure, but I believe the questioner's machine is a flow through type. I use that method to dial in the cutter where my most important measurement is from the top down.
From contributor S:
My first machine was a Komo Mach III VR512 with Siemens controls (PC front end), and I was also trained with the paper method. A PTP user will not use that one, rather the one contributor M explained... more practical. I believe operators do need to know G and M code (or whatever v. their software spits out) to ensure their machine is moving where it is supposed to.
From contributor P:
I have an older machine without tool changers; every tool change has to be datum-ed (touched off). I use a variant of the paper technique. I nudge the tool down to around 3mm off the bed, then use a box of engineering twist drills as go/no-go gauges. The drills are sized in 0.1mm steps (about 4 thou inch). It's incredibly easy to gauge to this level of precision. If 3.1mm rolls under and 3.2 doesn't, set your Z at 3.15 and zero is set. It's close to being a non-contact method, as the drills either don't touch or touch only the tip of one tip.
