ProbeApp for Centroid CNC12
ProbeApp for Mill & Routers that integrates with Centroid CNC12
Project maintained by swissi2000 Hosted on GitHub Pages — Theme by mattgraham
Universal Tool Setter
Description
These Tool Setter Cycles are for machines with spindles that have no fixed tool holders and can be used to set the machines WCS 0 for each tool by measuring the Tools Height Offset and are designed to be integrated with a M6 Tool Change Macro.
Adding a simple M58 command into the mfunc6.mac Tool Change Macro will bring up the Tool Setter screen for every tool change:
These Probing Cycles require that all tools are configured in the CNC12 Tool Offset Library with a Height Offset of 0. The ProbeApp will issue a Warning if this is not the case. It is recommended that you run the ProbeApp Tool Offsetter first as it will make sure that all Tool Height Offsets in the CNNC12 Tool Offset Library are reset to 0 for the Tool Setter cycles to work properly.
Before these probing cycles can be used for the first time, the Configuration Button needs to be pressed to confirm Probe settings and probing options. See the Configuration chapter for each Method below for details.
The Universal Tool Setter Cycles support 3 different Tool Setting Methods.
Click the links below for details on each Method:
Integration Options
By default the ProbeApp does integrate with CNC12 via M58 by installing a customized mfunc58.mac file into the C:\cncm folder.
Pressing the Probe Button on the VCP or commanding a M58 command will bring up the ProbeApp Main screen by default. This behavior can be customized in the mfunc58.mac file:
;--------------------------------------------------------------------------------
; Filename: mfunc58.mac
; M58 macro
; Description: Provides Probing Routines when used with program ProbeApp.exe
; Author: swissi
;---------------------------------------------------------------------------------
If #50001 ;Prevent lookahead from parsing past here
If #4201 || #4202 Then GOTO 1000 ;Skip macro if graphing or searching
.
.
;---------------------------------------------------------------------------------
;Possible ProbeApp Startup Options to directly open a specific Probing Cycle
;---------------------------------------------------------------------------------
;M130 "C:\cncm\probing\ProbeApp.exe" ;Startup ProbeApp Main Screen
M130 "C:\cncm\probing\ProbeApp.exe -ToolSetter" ;Startup ProbeApp directly with Universal Tool Setter Screen
;M130 "C:\cncm\probing\ProbeApp.exe -CornerPlate" ;Startup ProbeApp directly with Corner Plate Screen
;M130 "C:\cncm\probing\ProbeApp.exe -InCorPlate" ;Startup ProbeApp directly with Square Plate Screen
;M130 "C:\cncm\probing\ProbeApp.exe -BorePlate" ;Startup ProbeApp directly with Bore Plate Screen
.
.
If it is preferred that the Probe Button on the VCP or a M58 command will directly open the Tool Setter screen instead of the Main screen, modify the mfunc58.mac file as shown above.
Version 2 of the ProbeApp now offers a new method to temporarely overwrite the default ProbeApp Cycle screen by setting the CNC12 variable #29500 bevore calling the M58 command.
These are the possible values:
#29500 = 0 ; Main Menu (Default)
#29500 = 1 ; Angle
#29500 = 2 ; Bore
#29500 = 3 ; BorePlate
#29500 = 4 ; Boss
#29500 = 5 ; CornerPlate
#29500 = 6 ; Cube
#29500 = 7 ; InCor
#29500 = 8 ; InCorPlate
#29500 = 9 : OutCor
#29500 = 10 ; Single
#29500 = 11 ; Slot
#29500 = 12 ; ToolOffsetter
#29500 = 13 ; ToolSetter
#29500 = 14 ; TripleCorner
#29500 = 15 ; Web
Use the #29500 to temporarely overwrite the default opening Probing Cycle specified in the mfunc58.mac macro file.
Here’s an Example of a minimalistic mfunc6.mac file that will open the ProbeApp-Tool Setter at every M6 Tool Change:
;------------------------------------------------------------------------------
; File : mfunc6.mac
; Purpose : Minimalistic Tool change macro for Acorn CNC12 with ProbeApp integration
;------------------------------------------------------------------------------
IF #50001 ;Force lookahead to stop processing
IF #4201 || #4202 THEN GOTO 1000 ;Skip when graphing or searching
;------------------------------------------------------------------------------
; Turn Off Spindle
;------------------------------------------------------------------------------
M5
;------------------------------------------------------------------------------
; Retract Z to preferred Tool Change Position (uncomment your selection below)
;------------------------------------------------------------------------------
IF #50001 ;Force lookahead to stop processing
G53 Z0 ;Default
;G28 G91 Z0
;G30 G91 Z0
;G30 P3 G91 Z0
;G30 P4 G91 Z0
;------------------------------------------------------------------------------
; Display Tool Change Message
;------------------------------------------------------------------------------
IF #50001 ;Force lookahead to stop processing
#101 = 0
M225 #101 "#)Insert Tool #%.0f\nD:%.3f H:%.3f\n\nPress Cycle Start to continue" #4120 #[11000 + #4120] #[10000 + #4120]
;------------------------------------------------------------------------------
; ProbeApp Call
;------------------------------------------------------------------------------
#29500 = 13 ;Opens the ProbeApp directly with Tool Setter screen
M58
N1000 ;End of macro
Check out and customize the file mfunc6.mac.customize-for-ProbeApp that has been placed into the C:\cncm folder by the ProbeApp installation process. Rename the file to mfunc6.mac to activate it in CNC12.