[popspipes]

I can get the basics to work now g53 z0
x18.25 y-4.125
z-6 (I have to use negative numbers for Z and Y)

The little program runs fine, now to get it to select tool 0 and proceed to the toolsetter then back up to z0

[mountaindew]

Trying to understand what the difference is in using g53 and x,y,z values and using the preset values Used in g37. for the ets
Can anyone explain what your doing and why you dont get same results?

[soofle616]

Assuming G37 is set up to measure a tool length as it should be, that will position the spindle's axis directly above the axis of the tool setter. That's correct for checking tool lengths but if the goal is to check T0, the spindle axis needs to be offset in X and/or Y so that the edge of the spindle bore contacts the ETS. Using G53 allows for that offset.

[popspipes]

Yes the g53 position is slightly different, I have it working as long as I set tool 0 right after referencing the axes and set all to 0 it works.
If I reference then set up for a program and set 0,s for that it doesnt work for some reason if I try to set tool 0 again.

[mountaindew]

Assuming G37 is set up to measure a tool length as it should be, that will position the spindle's axis directly above the axis of the tool setter. That's correct for checking tool lengths but if the goal is to check T0, the spindle axis needs to be offset in X and/or Y so that the edge of the spindle bore contacts the ETS. Using G53 allows for that offset.

Ok thanks for the explanation. I see what your doing.
This is not required for router / collet tool changes. The z tool offsets are relative to the ets touch off surface and set on the fly
Spindle nose is touched off only the one time during ets setup to calibrate its height.

[soofle616]

The same is true for the mills. I ran for a few months without ever touching off the spindle nose except for when I first installed the ets and really didn't have a problem. Decided one day to re-reference and saw the position change by about 5-6 tenths so I decided to start touching off every time I started the machine. I rarely see it move by even a full .001 but it does move around a bit since it's position is based on machine zero and machine zero changes slightly with every power cycle. The biggest difference that it has made is keeping things consistent when adding new tools along with previously measured ones. For instance, I keep a 1/4" 3 flute always ready to go since it's my goto for aluminum. It never comes out of the tool holder unless I am replacing it. Used to be that I would have it's length set and that was it. Problem was when I added a new tool to the mix and measured it, the change in machine zero, and thus ets calibration, would lead to the slightest of mismatch if both tools were used on the same surface (like a smaller diameter tool used to finish a tight corner on the floor of a pocket). The basic solution is to remeasure all tools every power cycle so the relative offsets match which I've also done. BUT, when using a probe or haimer, you can't touch those off on an ets so getting their lengths set correctly is a pain. Rather than going through that process every power up, my haimer has a set calibrated length based on a calibrated ets - spindle nose offset. But that puts me back in the same spot where one tool has a length relative to a different calibrated setup. Touching off the spindle nose brings everything back to the same condition. It's a relatively small amount of work to avoid a very small amount of error and for most of what I do, doesn't improve part quality noticeably, but it's become part of the routine and it makes me feel better knowing I'm doing things "the right way"

[mountaindew]

The same is true for the mills. I ran for a few months without ever touching off the spindle nose except for when I first installed the ets and really didn't have a problem. Decided one day to re-reference and saw the position change by about 5-6 tenths so I decided to start touching off every time I started the machine. I rarely see it move by even a full .001 but it does move around a bit since it's position is based on machine zero and machine zero changes slightly with every power cycle. The biggest difference that it has made is keeping things consistent when adding new tools along with previously measured ones. For instance, I keep a 1/4" 3 flute always ready to go since it's my goto for aluminum. It never comes out of the tool holder unless I am replacing it. Used to be that I would have it's length set and that was it. Problem was when I added a new tool to the mix and measured it, the change in machine zero, and thus ets calibration, would lead to the slightest of mismatch if both tools were used on the same surface (like a smaller diameter tool used to finish a tight corner on the floor of a pocket). The basic solution is to remeasure all tools every power cycle so the relative offsets match which I've also done. BUT, when using a probe or haimer, you can't touch those off on an ets so getting their lengths set correctly is a pain. Rather than going through that process every power up, my haimer has a set calibrated length based on a calibrated ets - spindle nose offset. But that puts me back in the same spot where one tool has a length relative to a different calibrated setup. Touching off the spindle nose brings everything back to the same condition. It's a relatively small amount of work to avoid a very small amount of error and for most of what I do, doesn't improve part quality noticeably, but it's become part of the routine and it makes me feel better knowing I'm doing things "the right way"

Well explained,
This is what I pretty much figured was the strategy for using an ets with a mill and using a haimer or e-probe to find z offsets.
On router I mostly start by touching off a chamfer bit then use it to set x,y,z offsets on workpiece. By doing this it moves the machine spindle datum to end of that tool relative to the ets at touch off time.
More or less the same as touching off the spindle only its extended out to the end of a tool.
Then run programs and all tools touch off ets then move to work piece and cut. Tool table on this machine holds only the varied z value for tools. I dont even have descriptions or diameters. its all in cam.

Anyway I use g37 with ets on router all the time and wondered what you guys were up to!

[maker of things]

Shouldn't you be able to touch any tool with defined offsets on the presetter until it trips then change the Z dro (not tool offset) to 0 and be done?

[popspipes]

I will try that thanks! It seems to be a bit of a pain to have to set tool 0 before the offsets can be set, when you have to do a contortion act to get it in the same position each time.

[maker of things]

I do not have to do any tool zero setting to establish work offsets. Perhaps I am not understanding the situation, or it is related to the ETS which I do not use. I power up the machine, release e stop, reset button and on screen reset button. After referencing all axis, I then insert tool 50 (my haimer) and tell the machine that is the current tool. I then touch off x, y and z with the haimer for any work offset I need and the machine is ready to go. The only time I do what it sounds like you are doing every time is when I add a tool to the library. I use G59.3 insert tool 50 and tell the machine that is the tool in the spindle and put my presetter on the vise back jaw (usually). I jog the haimer down on the gauge block area of the manual presetter till the haimer is zeroed, then hit the zero z axis button (usually within .0005"). I insert the new tool and jog it to the measuring section of the presetter until the pre setter is at zero. I then make sure the machine knows the tool number I am setting up and go to the offsets tab and click the touch z button and the tool is ready. I do not teardown tools unless the tool is worn or broken which may affect the situation.

[popspipes]

I do not have to do any tool zero setting to establish work offsets. Perhaps I am not understanding the situation, or it is related to the ETS which I do not use. I power up the machine, release e stop, reset button and on screen reset button. After referencing all axis, I then insert tool 50 (my haimer) and tell the machine that is the current tool. I then touch off x, y and z with the haimer for any work offset I need and the machine is ready to go. The only time I do what it sounds like you are doing every time is when I add a tool to the library. I use G59.3 insert tool 50 and tell the machine that is the tool in the spindle and put my presetter on the vise back jaw (usually). I jog the haimer down on the gauge block area of the manual presetter till the haimer is zeroed, then hit the zero z axis button (usually within .0005"). I insert the new tool and jog it to the measuring section of the presetter until the pre setter is at zero. I then make sure the machine knows the tool number I am setting up and go to the offsets tab and click the touch z button and the tool is ready. I do not teardown tools unless the tool is worn or broken which may affect the situation.

It has to do with the tool setter, I set mine as you are doing but with the toolsetter it wants you to set tool 0 after a machine reset.
I now power up the machine and reference the axes, then set all axes to 0, then run a small program, g59 z-6 x18.25 y4.125, this puts the spindle in the position to set tool 0 for my machine always in the same position.

I just wanted a reference position that was always the same for tool 0 on startup.

[jttoner]

I now have it set up for G59 (an unused one) this works as long as I reference the machine and set G59 all axes to 0. then run the small program to position the spindle to the tool setter.
edit: I did add a g54 at the end of the program to put it back to g54 as I forget to do that..
I am using 2.8.3 PathPilot. mill Is an 1100 s3.

I will check out the router version for the spindle locate function. Thanks MD

Mike. I'm finally getting in some shop time' still working 7 day weeks. Good to see you're active. Anyway, got question. Did Wild Horse fold? I need a new probe and the Tormach probe is too expensive.

[popspipes]

Good to see you on again John!
I dont know if Wildhorse folded or not. What happened to the Renishaw??

[popspipes]

I am trying to use the built in sequence for setting tools with a tool setter, it wont set the tool length until I set tool Zero (spindle nose), there is no macro for setting the spindle nose position as it varies with individual setup etc.

I only set the spindle nose a few times as I set all tools per the job so that if there is a discrepancy in height due to the machine temp variations etc, it wont make any difference. Maybe I am wrong but thats the way I see it.........

There should be an option to set the spindle nose height or not each time the machine is referenced........??

[popspipes]

It would sure be nice if Tormach would include a check box in settings for the tool zero set, at least where you would have the option to use it or not. I have set this occasionally but not every time the machine is referenced. The small gcode file I wrote will do the position part and makes it easier to do that but all axes need to be set to zero after referencing to make it work other wise it gives an error that one or more of the axes limits are exceeded.

I only know enough about Linux and gcode to be dangerous!!!

any input on this would be welcomed.............

[soofle616]

The issue is that you're using G59 as your coordinate system to locate the spindle over the ets. Use g53 instead as that is the machine's base coordinate system and while it will change slightly each time you reference, it should only be by a couple thou at most (mine is usually .002" or less between power cycles). To figure out what your ets position is in G53, you can command g0 g53 x0 y0 z0 to set a starting point (use caution here, I haven't done this myself in a while but I'm pretty sure this will bring your Z to its upper travel limit). Zero your axes and then jog to wherever you want your spindle to go for your touch off. Your DRO will now show you the position in G53. Use that in your program instead of G59 and the machine will always go to the same spot no matter what wcs you're in or where it's set to.
I've actually set up my warmup program to include that line at the end so after the spindle shuts down the machine positions itself over the ets. All i have to do is push the ets reference button and I'm done.
Note: G53 requires a G0 on the same line or you will get an error message.

[popspipes]

The issue is that you're using G59 as your coordinate system to locate the spindle over the ets. Use g53 instead as that is the machine's base coordinate system and while it will change slightly each time you reference, it should only be by a couple thou at most (mine is usually .002" or less between power cycles). To figure out what your ets position is in G53, you can command g0 g53 x0 y0 z0 to set a starting point (use caution here, I haven't done this myself in a while but I'm pretty sure this will bring your Z to its upper travel limit). Zero your axes and then jog to wherever you want your spindle to go for your touch off. Your DRO will now show you the position in G53. Use that in your program instead of G59 and the machine will always go to the same spot no matter what wcs you're in or where it's set to.
I've actually set up my warmup program to include that line at the end so after the spindle shuts down the machine positions itself over the ets. All i have to do is push the ets reference button and I'm done.
Note: G53 requires a G0 on the same line or you will get an error message.

This file works even after running a part.

G0 G53 Z0 X18.4 Y-4.25
Z6

The code has to be all on the same line to set the spindle position, then line 2, I use Z6 to position the spindle for my particular setup.
This beats trying to do a Houdini act to set the spindle in the proper position each time the machine is referenced.

The hangup for me was not putting everything on the same line to position the spindle.

Thanks for the help, like I said earlier Gcode is not my specialty ha!