[adidoro]

I have another problem, when tool is longer than previous tool used, when it return to work position from tool change position it stop with error Machine limit reached, when is shorter it have no problem.
The start of changing the tool is from Z0 machine coordinate system because at the end of any toolpath I have a G28 Z0 for safety.

[adidoro]

The solution is to change Safe Height to -50 and Z position of tool change to -50 too. (to allow the differences from tool to tool)
But that is not the way it should work, I think.

Edit: No, this changes not working. It's about Z height when start the tool change. If is Z0 in machine coordinate and the tool is longer than previous it will stop with error.
If Z is lower it return to that position without error.

[PlanetCNC]

Machine limit reached error is displayed if machine tries to move outside its limits.

If your new tool is longer then "previous position" is higher and is probably outside machine limits.

[adidoro]

Machine limit reached error is displayed if machine tries to move outside its limits.

If your new tool is longer then "previous position" is higher and is probably outside machine limits.

I start simulation, Z is at zero, change tool to no.1, measure tool longer than tool no.0, here is a video

https://www.youtube.com/watch?v=w9FaH06te70

[PlanetCNC]

Looks like your tool measuring is changing machine position.
It is possible to handle tool length changes this way but you can not use machine limits in Z direction if you do this.

You should use tool offset to handle tool lengths.

[adidoro]

Looks like your tool measuring is changing machine position.
It is possible to handle tool length changes this way but you can not use machine limits in Z direction if you do this.

You should use tool offset to handle tool lengths.

I did not modify tool change script and I use tool offset.

[adidoro]

If I disable "AutoReturn" then is moving up from fixed tool sensor (at Z zero in machine coordinate) and at that height if I manually command to go to previous position is no error.
So I think may be something wrong there. Maybe does not consider the tool offset when is returning to position.
For now, when I start a g-code I lower Z for first toll measure and for sub tool change I removed the G28 Z0 at the end of every toolpath...

Edit: Have you tested as I did in the video? It is only on my end this error?

[PlanetCNC]

I can not test this because I do not have your profile so I can not give you exact answer, what are you doing wrong.

What I see is, that difference in length between T1 and T0 is 90mm and on auto return machine will try to compensate for this difference but it can't because it is out of machine limits.
I suspect your fixed sensor is not set correctly. How did you set "Sensor position Z" value?
https://planet-cnc.com/measure-tool-...-tng-software/

One other note - auto return should be used with g-codes that do not support tool change. Proper g-code with tool change does not need auto return and should not be enabled.

[adidoro]

I can not test this because I do not have your profile so I can not give you exact answer, what are you doing wrong.

You don't need profile folder, just start to measure a tool that is longer than previous from Z0 machine coordinate system with auto return enabled.

Edit: That will happen on any machine or profile, because the auto return is trying to move the tool tip to previous position and it can't, tool being longer will trigger the limit. In other words can't start measuring a tool length from Z0 absolute if tool is longer than previous with auto return enabled.

Another edit: Auto return should only move the X and Y back to position, not Z. I will modify the script for that.

[PlanetCNC]

You are wrong.
But you can do whatever you want. Just make sure you don't break any tools because tool tip will be too low. If your tool is longer then it should move higher otherwise it will crash into material.

[adidoro]

You are wrong.
But you can do whatever you want. Just make sure you don't break any tools because tool tip will be too low. If your tool is longer then it should move higher otherwise it will crash into material.

No, I'm not wrong. Did you made the test?
Higher than Z0 machine position doesn't exist.

[PlanetCNC]

And that is why you get an error then you want to move higher. .

[adidoro]

And that is why you get an error then you want to move higher. .

The start of changing the tool is from Z0 machine coordinate system because at the end of any toolpath I have a G28 Z0 for safety.

I've said that from the first post. Anyway I've commented the Z move from return in M6 script and problem is solved.

[PlanetCNC]

You are still wrong.

Btw, why do you have G28 Z0 code and do you know what it does?

[adidoro]

You are still wrong.

No, I'm not. I will ask you again, did you made that simple test?
Start to measure a tool that is longer than previous from Z0 machine coordinate system with auto return enabled.
And tell me if you get that error or not.

Btw, why do you have G28 Z0 code and do you know what it does?

Yes, I know.

[PlanetCNC]

Yes, I get an error. And this is correct. You want machine to go to position that is outside machine limits. If you do this with soft limits turned on you get this error because this is not possible.
If you change script like you did, you will crash machine into material.

Perhaps you assume that there is enough room between your start position and material but this is usually not true. Specially not true if you use "return" feature the way it was intended to be used.

[adidoro]

Ok, thank you for confirmation.
I have no choice and I don't see any trouble with not getting to that Z position before it had, because is happening after X and Y arrived at previous position from tool change, so there will not be any issues.
Of course I have in settings Safe Height = 0 and Position Z = 0 for Tool Change.
I talk about this from M6:

o<ar> if [#<_tc_autoreturn>]
  G00 X#<wstartx> Y#<wstarty>
;  G00 Z#<wstartz>
O<ar> endif

The travel from tool change position X and Y will occur before that Z move which give that error.
Correct me if I'm wrong.

Edit: In regard to crushing the tool in material it will happen anyway if it's not enough space. That is not controller software responsibilities but the g-code generated with not enough clearance. If clearance is to large and not fit the machine boundaries, that is controller software responsibilities.

[PlanetCNC]

I just want to explain that "Return" means that tooltip will return to exact same position where previous tooltip was. And if this move is not possible you get an error.

Obviously you want "Return" to do something else. That does not mean that existing implementation is incorrect. After all, because it is scriptable you can change it to match your needs.
Here is video showing how return should work:

[adidoro]

I just want to explain that "Return" means that tooltip will return to exact same position where previous tooltip was. And if this move is not possible you get an error.

I understand that, but I just told you about the fact that that error occur to late anyway if the tool is to long, it is after X and Y will move to previous position from tool change and just after the tool crushed in to material the error will occur when will try to move Z to that position.
By removing that Z move it does nothing wrong about safety for not crushing the tool in material.

Edit: If it was like this:

o<ar> if [#<_tc_autoreturn>]
  G00 Z#<wstartz>
  G00 X#<wstartx> Y#<wstarty>
O<ar> endif

Then that error will prevent the move of X and Y. But this is not a good implementation, just to understand what I mean.

[PlanetCNC]

I've changed default script with this code:

o<ar> if [#<_tc_autoreturn>]
  (print,AutoReturn)
  o<chk> if [#<_z> LT #<wstartz>]
    G00 Z#<wstartz>
  o<chk> endif
  G00 X#<wstartx> Y#<wstarty>
  G00 Z#<wstartz>
o<ar> endif

If tool is too long, machine will try to get higher if possible. Crash will be avoided.