Even though I’m running a Centroid Acorn controller, I’m 100% sure I can get more helpful answers here than on the Centroid forum, where they rarely give you a direct answer to a question. I believe the basic workflow and code should be about the same across different controller platforms.
I have a toolsetter that is functioning just fine for my basic Z probe.
Per normal operation of the toolsetter, how would I go about addressing subsequent manual tool changes to utilize the toolsetter in the fixed position. I emphasize manual, because the tool changes may not be called up in a program, per my preferred ‘one program per tool’ method of operation. I want to manually change tools based on the original Z ref from the workpiece.
I believe I can use a modified version of @Aiph5u’s Tool Change Routine, but I’m not sure how to be able to manually call this program up as a subroutine.
As usual, thanks for any input!
Shown out of locating dock, where I can use it for normal top-of-workpiece Z probing.
you know from my private e-mail that I have so much to do at the moment, however what you try to do is on my list for the buildbotics-derived Onefinity controller: To implement a g-code tool setter algorithm for recording bit length on tool change events on the buildbotics-derived controller. It should not be difficult, it is just required to use a variable (variables are called “parameters” in g-code) and to store a value from the last tool change in a user parameter, and there would be an initial tool change required, even if the tool is already in the spindle, just to record the initial tool length of the first tool. Unfortunately unlike other CNC controllers (like the Masso controller), the Buildbotics does not remember values over a power down or an estop.
Unfortunately I did not yet find the time to analyze Makermatt’s tool change routine but he reports that it works for his RapidChange tool change system, but should work for manual tool change also, with popup windows requesting the correct bit by number.
A script like this would use entries both in the ‘program-start’ and the ‘tool-change’ input fields of the SETTINGS page. You may have a look
If you have the tool setter in a fixed position, the most simplest way would be to always set the workpiece zero on the bottom of your virtual 3D model. If you do this, you would just be required to record the tool setter’s height of triggering point just like with the XYZ touch plate so that it is substracted automatically on every use. This is done in the line with the G92 command. I have a variation in my Aiph5u’s tool change routine for workpiece zero on machine bed at the end of the posting there (you just need to comment a line out for probing on machine bed).
I almost emailed you, but didn’t really want to bother you with this since you have other stuff going on. As usual, I appreciate your helpful input!
I did actually manage to get a helpful and direct answer on FB that pointed to a document on the Centroid forum that gives a full explanation in detail on how to set this up. I hope to make some headway on this tomorrow.
Just wanted to chime in here that I have been updating and improving the code significantly since that thread and have had good luck with the tool setting portion of the code. I have moved everything to a subroutine (O program as they are called) to ensure that it is only called when I want it to be called and not triggered by the Macros function which runs the program start code each time a macro is run.
You can can simply create a subroutine with the “o” word and a name and “sub” after it, followed by your code and then end with a “endsub”
To run the subprogram you use “o [name of program] call”. The word “call” is what actually runs it whether that be in your program start, on tool change, end program or in a macro. Below is a snippet of the code I am using which youl can see has one program calling other sub programs.
o<rc_measure_tool> sub ; this is a subprogram called <rc_measure_tool>
o190 if [#<_rc_measure> EQ 1] ;if statement to see if a parameter called # is equal to 1
o<rc_measure_tool_auto> call; this is where the subprogram <rc_measure_tool_auto> is called
o190 elseif [#<_rc_measure> EQ 0]
o<rc_measure_tool_disabled> call; this is another program called if the parameter above is 0
o190 endif
o<rc_measure_tool> endsub
o<rc_measure_tool_auto> sub; this is a second program which is called from above
o<rc_calc_set_dist> call
G53 G90 G0 X[#<_rc_x_measure>] Y[#<_rc_y_measure>]
G53 G90 G0 Z[#<_rc_z_seek_start>]
G38.2 G91 Z[#<_rc_seek_dist> * -1] F[#<_rc_feed_seek>]
G0 G91 Z[#<_rc_retract_dist>]
G38.2 G91 Z[#<_rc_set_distance> * -1]
o<rc_set_tlo> call
G53 G90 G0 Z[#<_rc_z_safe>]
o<rc_measure_tool_auto> endsub
