Applying offsets when changing tools manually.

[Alexanders]

When you manually select the tool ID in the tool menu, the offsets from the offset table are applied and work.
In the G code program, after the Tn M06 line, the tool number changes in the Tool ID menu, but the coordinates do not change and in fact offset does not occur.
I don't understand what I'm doing wrong...

[TomKerekes]

Hi Alexanders,

G Code allows the Tool Length/Offset to be applied independently of the selected tool as well enabled/disabled independently. In some machines this can be useful when the next tool is pre-loaded while the previous tool is still in use.

To select which Tool's offset is to be used for Length/Offset compensation use the Hxxxx command. To enable Tool Length/Offset compensation use G43. To disable G49.

Whether or not the Tool Dropdown automatically selects and enables the Tool Length/Offset Compensation can be configured in the Tool Setup here.

[Alexanders]

Do I understand correctly that the string T2 M6 will not use the offset of tool 2 under any circumstances?
The offset of tool 2 will only apply either a manual selection from the ID list or the string G43 H2 , correct?
Then in the case of a manual tool change, the string T2 M6 will not perform any actions and does not make sense?

[TomKerekes]

Hi Alexanders,

Do I understand correctly that the string T2 M6 will not use the offset of tool 2 under any circumstances?

Well not exactly. It doesn't have any effect on whether Tool 2 Length/Offset is in use or not.

The offset of tool 2 will only apply either a manual selection from the ID list or the string G43 H2 , correct?

yes. The manual selection from the ID list will apply the Length/Offset if Tool Length/Offset Immediately is enabled.

Then in the case of a manual tool change, the string T2 M6 will not perform any actions and does not make sense?

It makes sense if you want to use it to request the Operator to change the Tool. It also effects which Tool image is used in the G Code Viewer.

[Alexanders]

After determining the tool offset, I have to manually enter the height value in the tool table. This is inconvenient and can lead to errors.
Can you give an example of assigning a user button to automatically insert coordinates into the table of the current tool?

[TomKerekes]

Hi Alexanders,

See the ToolTableSet.c example.

[Alexanders]

Thanks! It would be useful to add all the above information to the manual. The current manual does not give a complete understanding of these nuances.
There is another question. I am currently setting up the generation of G codes in SolidCAM 2022.
When applying G41/G42 compensation, KMotionCNC always returns the error "Cutter gouging with cutter radius comp". I have tried different options and tool inlet/outlet distances related to G41/G42. The error is always repeated. Under what conditions does this error occur? And where can I find a list and description of KMotionCNC errors?

[TomKerekes]

You might read this wiki article:
Internal/concave Path Tool Radius Compensation Example G41/G42

[larryjamessmith]

Hello,
I have just spent two days trying to figure out why my custom program to execute an M6 tool change was no longer working correctly and causing my tool to end up positioned at the wrong height, sometimes diving into the workpiece (once into my expensive vise!). I finally figured it out. It was due to the option being set in Trajectory Planner to "Apply tool length/offset immediately". I don't know which release this appeared in, but it is dangerous!

When using a custom program to execute an M-code it is best to leave it up to the programmer to perform all functions required. In this case, that option being checked results in the initial tool tip height not being determined correctly.

If the option is provided to automatically perform a G43, it should be performed AFTER the custom M6 program is finished. This would reference the currently mounted tool after it is mounted and any clamping errors have already been accounted for. This is also where it is typically sequenced in gcode by CAD system post processors.

Thank you,
Larry Smith

[TomKerekes]

Hi Larry,

Sorry to hear of your troubles. That option should only apply to tool changes via the dropdown list. Not M6 ran from GCode. It was added years ago and defaults to off. Other Users are equally adamant it should be applied automatically. Hence the option.