Tool Table Touch Off

ddmotim wrote: Am I incorrect, or am I doing something wrong?

The Axis GUI rather hides what is happening under the hood. (and it also makes it too easy to get it wrong)

The touch-off button brings up a dialog, and in that you can select a drop-down. What then happens is either G10 L20 PN, where N is the dropped-down coordinate system
www.linuxcnc.org/docs/html/gcode/gcode.html#sec:G10-L20
or a G10 L10 P(current tool)
www.linuxcnc.org/docs/html/gcode/gcode.html#sec:G10-L10

So, basically, Touch-off to G54 (if you are in G54) makes the number you enter "true" by moving the coordinate system, and Touch-off to the Tool Table (T) makes the number you enter true by changing the tool table.

I have two machines and they work in different ways.

The lathe has a "master" tool that is used for facing and turning. That tool always has a zero-offset in it. I actually mess this up by mistake quite often, and then I MDI a G10 L10 X0 Z0 G43 to set things back to normal. It annoys me how easy this is to get wrong, and in fact I just sent an email to the dev list suggesting we spilt the button.
So, I make a test-cut facing to length and touch-of Z in G54, then a test diameter and repeat for X. (Because Z=0 moves for every job, and X moves for material and feed on my rubber lathe)
Then I tend to stop the individual tools a bit short of finish diameter and re-set them with a T touch-off for the current job.

On the mill it is different. Each tool including the probe is defined by its length measured above the table by a height gauge when the tool or probe is in the fixture:
picasaweb.google.com/lh/photo/7v3gpOZHcT...pFm0?feat=directlink

So, On that I touch-off G54 to the work, but never touch-off tools. I either edit the tool table or MDI a G10 L1

If I was defining G-code G10 L1, G10 L2, G10 L10 and G10 L20 would be G10, G11, G12, G13. But it's too late now.

Thanks guys!

John, I found that post last night in another thread, it's exactly what I needed. I wasn't switching back and forth from "touch off to fixture" and "touch off to workpiece"

andypugh wrote: The lathe has a "master" tool that is used for facing and turning. That tool always has a zero-offset in it. I actually mess this up by mistake quite often, and then I MDI a G10 L10 X0 Z0 G43 to set things back to normal. It annoys me how easy this is to get wrong, and in fact I just sent an email to the dev list suggesting we spilt the button.
So, I make a test-cut facing to length and touch-of Z in G54, then a test diameter and repeat for X. (Because Z=0 moves for every job, and X moves for material and feed on my rubber lathe)
Then I tend to stop the individual tools a bit short of finish diameter and re-set them with a T touch-off for the current job.

I second changing the behaviour of the touch off window. I've many times inadvertently changed a tool length (when I've wanted to G54) because I haven't changed the drop down back to G43 from tool table.

Hi Andy.
A couple of quick questions.

When you use your fixture to measure the height of a milling tool in a holder, what dimension do you edit into the Z parameter of the tool table?
Is it the direct reading of the height gauge? Is it that minus some fixed dimension?
Is it entered as a negative number?

Thank you for your help!!

Ray

RayJr wrote: When you use your fixture to measure the height if a milling tool in a holder, what dimension do you edit into the Z parameter of the tool table?

I enter the height above the table of the tool tip.
This works because the probe (my tool 99) is also measured the same way, and I use that to find the top of the work.

It actually works anyway, what matters is the relative length of the tools, not anything absolute.

I don't actually edit the tool table, normally. When I replace a tool I use the Touchy "set tool" which brings up G10 L10 Pnn (and have to edit the L10 to L1)

For this to work well, wouldn't the knee of a Bridgeport need to be set to the same position (height) each time you need to set a new tool in the tool table?

Ray