Tool change: Milling cutter pops into the material after the measurement

[tantemay]

I have a problem with the tool change
Following situation:
I insert a milling cutter and drive the tip onto the material surface. Then I set this position as Z zero.
Now if I make a tool change and insert a milling cutter, e.g. 10mm shorter than the previous one, then the machine moves to position Z10 after the measurement. So exactly the length that it is shorter, the machine stops above the material surface.
That wouldn't even be a problem. But when it is 10mm longer, the machine moves to Z-10 and bangs into the valuables.


What am I doing wrong or have I misunderstood something?

Similar Threads:

• Meldas, programs8000 or 9000 for tool change, tool measurement, workpiece measurement
• Video Computer Vision and CNC find material center, material measurement, offse
• Mach3 plunging cutter after tool change
• Auto Tool Zero Sensor & Connection Checker, Cnc, Tool Change / Measurement.
• Need Help!- VF 4 Tool change Pops, loud!

[Kenny Duval]

That's because the machine has no idea you changed the cutter or that the cutter is shorter. You either have to touch that tool off on the same reference surface and reset Z zero to the new tool or you need a tool offset table.

Tool Length Offsets Beginners CNC - CNC Training Centre

[tantemay]

No. The machine measures the tool length. That works too. Nowhere does it move after measuring 0 position. I miss doing that with the "Move To Zero" button.

[Kenny Duval]

Then look at the code. Is it calling a tool offset value after the tool change?

[tantemay]

some Demo:

[Kenny Duval]

That looks like the tool offset is not being applied. When you touch a tool to the ETS is it updating the tool table appropriately. That looks like either the tool offset is not being applied before sending the machine back to zero or the G54 work zero is being moved. You aren't zeroing the axis between tools changes are you?

[tantemay]

1. I do a tool length measurement to get a reference height.
2. I determine the workpiece height and set the position to z0
3. If I then make a tool change, the tool length will be repaired.
That works just fine. Only then does the milling cutter not move back to the old z position. It stands above or below. Depending on whether you have inserted a longer or shorter cutter.
If you then manually move to the old position, everything is correct.
Why doesn't the machine do it independently?

Do I have to do anything else in the settings of the TNGv2 software?

[SeeAnnSee]

Tantamay:

Have you cleared your work position offsets prior to running your new gcode? I suspect that you still have prior material offset (set by your moveable sensor during your previous job) that was not cleared. Try Machine > Work Position > Offset > To Zero. While you are at it, make sure that the tool offset (most likely set using your fixed sensor) has been cleared: Machine > Tool Offset > To Zero. You can also verify that the offset has been cleared by toggling between the "Work" and "Machine" tabs to determine if the coordinates have returned to zero.

As a standard practice, I zero all offsets prior to start of a new project, I measure my material surface offset using my moveable sensor (Z = 0), measure my tool length offset using my fixed sensor, and then once this has been done, I re-measure my material surface offset. I perform the first material surface offset so that I do not encounter a problem with the tool crashing with the material surface once the tool length has been measured. In other words, the first material surface measurement is to prevent crashes, and the second is for the actual measurement for Z=0 offset. Of course, there are icons that can be used to easily perform these offset functions (clearing as well as setting) so that you don't need to fiddle with the drop down Machine menu selections.

Once I starting following the above procedure, I have never had a problem with tool crashes or improper material or tool length offsets. It works flawlessly.

Hope this makes sense, and I hope it helps!

- Tom the SpindleJockey

[tantemay]

Did anyone watch the video?
The tool changes and the measurement function perfectly.
The zero point is also adapted to the newly inserted milling cutter.
Only the milling machine does not move there.
Example of inserted milling cutter is exactly on Work Z0
Then a tool change is made and the new milling cutter is 10mm shorter.
After the measurement, the machine does not move the milling cutter back to Work Z0, but to Z10.
When the new milling cutter is 10mm longer, the machine moves the milling cutter to position Work -10.
You can then move the milling cutter to position Z0, but then it will be too late.

[Kenny Duval]

That can only be a problem with the tool change macro then.

It should always go to a safe Z position...
apply the new tool offset
then return to work zero...

It looks like it isn't applying the offset before returning to zero.

[tantemay]

I set the material surface manually. it doesn't matter. The machine is supposed to move the milling cutter back to where it was before. No matter if he was on z50 or -z50. The controller adjusts the offset, but does not move the machine there

[Kenny Duval]

If you set work zero with the first tool...then put in a tool that is 10mm shorter, probe it and then return to zero and the tool is 10mm above the work then clearly the tool offset is not being updated or applied. Same thing for the 10mm longer tool. The only difference is the longer tool crashes into the work.

The control has to account for the difference in length of each tool. That requires applying an offset.

[tantemay]

Yes, the control takes into account the different tool lengths. It just doesn't move back to the last work position, but to the last machine position.
I'm just asking if this is correct or if it is a bug.

[PlanetCNC]

My first guess is, that "Auto Return" should not be enabled unless "Enable Offset" is also enabled.

[Kenny Duval]

Well that would explain the behavior. Clearly the offset is not being applied when returning to zero.

[tantemay]

My first guess is, that "Auto Return" should not be enabled unless "Enable Offset" is also enabled.

Have a look

[Kenny Duval]

Then that looks like a bug...

[PlanetCNC]

Then offset is applied.
"Autoreturn" returns machine to previous machine position and not to work position. Kind of makes sense assuming that you start tool change procedure from safe height like you should. It then returns machine to same safe height.
Both "Enable Offset" and "Autoreturn" settings are disabled by default. It is not M6 job to call G43 or to move machine anywhere except to tool change position.
For example:
Lets say we have simple g-code:

%
G21 G90
G00 X0 Y0 
G01 Z0
G01 X30
G01 Y30
G01 X0
G01 Y0
%

Lets change some tool changes:

%
G21 G90
G00 X0 Y0 
T1 M6
G01 Z0 
G01 X30 
T2 M6
G01 Y30 
T3 M6
G01 X0 
T4 M6
G01 Y0 
%

Will this work. No. Not unless "Enable Offset" and "AutoReturn" are used. But this G-code is not correct.
Lets do it correctly:

%
G21 G90
G00 X0 Y0 

G49
G00 Z100 (safe height)
T1 M6
G00 X0 Y0 
G43
G01 Z0
G01 X30 

G49
G00 Z100 (safe height)
T2 M6
G00 X30 Y0 
G43
G01 Z0
G01 Y30 

G49
G00 Z100 (safe height)
T3 M6
G00 X30 Y30 
G43
G01 Z0
G01 X0 

G49
G00 Z100 (safe height)
T4 M6
G00 X00 Y30 
G43
G01 Z0
G01 Y0 

G49
G00 Z100 (safe height)
%

It is not so simple anymore. That is where two settings are useful. To help create simple g-code for simple things..

[tantemay]

Then I should write in the PP that the machine moves before changing to machine position Z-5.
Respectively, I have now written this in the M6 script.

[PlanetCNC]

Yes, safe heights and positions should be part of PP.