Hello Guest it is October 18, 2019, 10:28:49 AM

Author Topic: Creating an M6 Toolchange in Mach4 (Part 3)  (Read 6743 times)

0 Members and 1 Guest are viewing this topic.

Offline DazTheGas

*
  •  750 750
  • DazTheGas
    • View Profile
Creating an M6 Toolchange in Mach4 (Part 3)
« on: October 13, 2015, 03:50:37 PM »
Yay Finished (with a crashed machine  ???

Although the machine crashed at the end the code has been retested completely and works a treat.

Video https://youtu.be/w1xzYPT27NY

The Final Code

Code: [Select]
function M6()
    local inst = mc.mcGetInstance();
    local selectedtool = mc.mcToolGetSelected(inst)
    local currenttool = mc.mcToolGetCurrent(inst)
    local xstart = mc.mcAxisGetPos(inst,0)
    local ystart = mc.mcAxisGetPos(inst,1)

    if selectedtool == currenttool then
    return
    mc.mcCntlSetLastError(inst, "ToolChange Activated But Not Required")
    else
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0 \n X14 Y30")
    wx.wxMessageBox("Please turn off spindle and click ok to continue") --can be removed if required
    RunProbe(currenttool)
    local toolz = mc.mcAxisGetPos(inst,2)
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0")
    local changetoo = mc.mcToolGetDesc(inst,selectedtool)
    wx.wxMessageBox("Please change to tool number "..selectedtool.." "..changetoo.." and press ok to continue")
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 X14 Y30")
    RunProbe(selectedtool)
    mc.mcAxisSetPos(inst, 2 , toolz)
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0")
    wx.wxMessageBox("Please turn on spindle and click ok to continue") --can be removed if required
    mc.mcCntlGcodeExecuteWait(inst,"G90 G0 X"..xstart.." Y"..ystart)
    mc.mcToolSetCurrent(inst, selectedtool)
    mc.mcCntlSetLastError(inst, "ToolChange Finished")
    end
end

function RunProbe(tool)
    local inst = mc.mcGetInstance()
    toollen = mc.mcToolGetData(inst, mc.MTOOL_MILL_HEIGHT, tool)
    if toollen == 0 then toollen = 40 end -- User Preference
    mc.mcCntlSetLastError(inst, "Changing to Fallback Length")
    local probestart = -60 + toollen
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z"..probestart.."\nG91 G31 Z-15 F25")
end

if (mc.mcInEditor() == 1) then
    M6()
end

now to do a quick vid on that crash!!!!

DazTheGas
Theres always time for a choccy biccy
Re: Creating an M6 Toolchange in Mach4 (Part 3)
« Reply #1 on: November 03, 2015, 11:19:43 AM »
Hey, I wanted to thank you for this post, using your macro as a reference and knowing like, literally no G Code or LUA I was able to get a manual toolchange with automatic touchoff working.

I really appreciate it.

Offline Bx3mE

*
  •  48 48
    • View Profile
Re: Creating an M6 Toolchange in Mach4 (Part 3)
« Reply #2 on: November 28, 2016, 05:50:24 PM »
Just adding a thankyou! :)

I Made some Modifications
- Probemove for approach probe to avoid Crash :) and back off probe before real probing.
- Lots of Variables to tune the script
---Preset for probelocation
---Preset for ToolChange position
---Preset for defaults and speeds


Code: [Select]
function M6()
    local inst = mc.mcGetInstance();
    local changeToTool = 3--mc.mcToolGetSelected(inst)
    local changeFromTool = 2--mc.mcToolGetCurrent(inst)
    local XPositionBeforeToolChange = mc.mcAxisGetPos(inst,0)
    local YPositionBeforeToolChange = mc.mcAxisGetPos(inst,1)
    local XToolProbePosition = "1"
    local YToolProbePosition = "1"
    local XManualToolChangePosition = "2"
    local YManualToolChangePosition = "2"
    local ColletAtProbeZCoordinate = -103 -- Machine Z-coordinate when collet tip touches TouchPlate (Must be more than ProbeOperationDistance - DefaultToolLength
    local ExtraProbeDistance = 5 -- SafetyMargin
    local ProbeOperationDistance = -30 -- Length of Probemove before giving up
    local ProbePrepSpeed = 100
    local ProbeSpeed = 25
    local DefaultToolLength = 70 -- Used if tool info is not found. (Should be a value slightly longer than the longest tool in the shop :D)
        -- QUICK REFERENCE
        -- G90 - Absolute (Go to coordinate)
        -- G91 - Incremental (Godistance along axis from current position)
        -- G53 - Machine Coordinate Move

    if changeToTool == changeFromTool then
    return
    mc.mcCntlSetLastError(inst, "ToolChange Activated But Not Required")
    else
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0\nM5" )
    RunProbe(inst,changeFromTool,XToolProbePosition,YToolProbePosition,DefaultToolLength,ColletAtProbeZCoordinate,ExtraProbeDistance,ProbePrepSpeed,ProbeSpeed)
    local ToolZCoordinate = mc.mcAxisGetPos(inst,2)
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0 \n X"..XManualToolChangePosition.." Y"..YManualToolChangePosition)
    local changeToToolDescription = mc.mcToolGetDesc(inst,changeToTool)
    wx.wxMessageBox("Please change to tool number "..changeToTool.." "..changeToToolDescription.." and press ok to continue")
    RunProbe(inst,changeToTool,XToolProbePosition,YToolProbePosition,DefaultToolLength,ColletAtProbeZCoordinate,ExtraProbeDistance,ProbePrepSpeed,ProbeSpeed)
    mc.mcAxisSetPos(inst, 2 , ToolZCoordinate)
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0")
    mc.mcCntlGcodeExecuteWait(inst,"G90 G0 X"..XPositionBeforeToolChange.." Y"..YPositionBeforeToolChange)
    mc.mcToolSetCurrent(inst, changeToTool)
    wx.wxMessageBox("If Toolchange was Sucessful - click ok to continue")
    mc.mcCntlSetLastError(inst, "ToolChange Finished")
    end
end

function RunProbe(finst,ftool,fXToolProbePosition,fYToolProbePosition,fDefaultToolLength,fColletAtProbeZCoordinate,fExtraProbeDistance,fProbePrepSpeed,fProbeSpeed)
    mc.mcCntlGcodeExecuteWait(finst, "G90 G53 G0 X"..fXToolProbePosition.." Y"..fYToolProbePosition)
    local toollen = mc.mcToolGetData(finst, mc.MTOOL_MILL_HEIGHT, ftool)
    if toollen == 0 then toollen = fDefaultToolLength end
    mc.mcCntlSetLastError(finst, "Tool length not found - using Default Length")
    local probestart = fColletAtProbeZCoordinate + fExtraProbeDistance + toollen
    local GCODE = "G90 G53 G31 G0 Z"..probestart.." F"..fProbePrepSpeed
    GCODE = ""..GCODE.." \n G91 G0 Z5 F"..fProbePrepSpeed.." \n G91 G31 Z-15 F"..fProbeSpeed
    mc.mcCntlGcodeExecuteWait(finst,GCODE)
end

if (mc.mcInEditor() == 1) then
    M6()
end

Offline Bx3mE

*
  •  48 48
    • View Profile
Re: Creating an M6 Toolchange in Mach4 (Part 3)
« Reply #3 on: November 29, 2016, 08:08:14 AM »
The change i made to avoid Crash on approach did not behave as expected ( NOT WORKING AT ALL ;D)
So fixed now...And Some other stuff :P

I have not done any rigorus testing but tried some stupid stuff and the script still behaves...

New Version:

Code: [Select]
function M6()
    local inst = mc.mcGetInstance();
    local changeToTool = mc.mcToolGetSelected(inst)
    local changeFromTool = mc.mcToolGetCurrent(inst)
    local XPositionBeforeToolChange = mc.mcAxisGetPos(inst,0)
    local YPositionBeforeToolChange = mc.mcAxisGetPos(inst,1)
    local XToolProbePosition = "1"
    local YToolProbePosition = "1"
    local XManualToolChangePosition = "2"
    local YManualToolChangePosition = "2"
    local ColletAtProbeZCoordinate = -105 -- Machine Z-coordinate when collet tip touches TouchPlate (Must be more than ProbeOperationDistance - DefaultToolLength
    local ExtraProbeDistance = 5 -- SafetyMargin
    local ProbeOperationDistance = -30 -- Length of Probemove before giving up
    local ProbePrepSpeed = 100
    local ProbeSpeed = 25
    local DefaultToolLength = 70 -- Used if tool info is not found. (Should be a value slightly longer than the longest tool in the shop :D)
        -- QUICK REFERENCE
        -- G90 - Absolute (Go to coordinate)
        -- G91 - Incremental (Godistance along axis from current position)
        -- G53 - Machine Coordinate Move

    if changeToTool == changeFromTool then
    return
    mc.mcCntlSetLastError(inst, "ToolChange Activated But Not Required")
    else
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0\nM5" )
    RunProbe(inst,changeFromTool,XToolProbePosition,YToolProbePosition,DefaultToolLength,ColletAtProbeZCoordinate,ExtraProbeDistance,ProbePrepSpeed,ProbeSpeed,ProbeOperationDistance)
    local ToolZCoordinate = mc.mcAxisGetPos(inst,2)
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0 \n G90 G53 G0 X"..XManualToolChangePosition.." Y"..YManualToolChangePosition)
    local changeToToolDescription = mc.mcToolGetDesc(inst,changeToTool)
    wx.wxMessageBox("Please change to tool number "..changeToTool.." "..changeToToolDescription.." and press ok to continue")
    RunProbe(inst,changeToTool,XToolProbePosition,YToolProbePosition,DefaultToolLength,ColletAtProbeZCoordinate,ExtraProbeDistance,ProbePrepSpeed,ProbeSpeed,ProbeOperationDistance)
    mc.mcAxisSetPos(inst, 2 , ToolZCoordinate)
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0")
    mc.mcCntlGcodeExecuteWait(inst,"G90 G0 X"..XPositionBeforeToolChange.." Y"..YPositionBeforeToolChange)
    mc.mcToolSetCurrent(inst, changeToTool)
    wx.wxMessageBox("If Toolchange was Sucessful - click ok to continue")
    mc.mcCntlSetLastError(inst, "ToolChange Finished")
    end
end

function RunProbe(finst,ftool,fXToolProbePosition,fYToolProbePosition,fDefaultToolLength,fColletAtProbeZCoordinate,fExtraProbeDistance,fProbePrepSpeed,fProbeSpeed,fProbeOperationDistance)
    mc.mcCntlGcodeExecuteWait(finst, "G90 G53 G0 X"..fXToolProbePosition.." Y"..fYToolProbePosition)
    local toollen = mc.mcToolGetData(finst, mc.MTOOL_MILL_HEIGHT, ftool)
    if toollen == 0 then
        toollen = fDefaultToolLength
        mc.mcCntlSetLastError(finst, "Tool length not found - using Default Length")
    end
    local probestart = fColletAtProbeZCoordinate + fExtraProbeDistance + toollen
    local GCODE = "G91 G31 G0 Z"..probestart.." F"..fProbePrepSpeed
    GCODE = ""..GCODE.." \n G91 G0 Z1 F"..fProbePrepSpeed.." \n G91 G31 Z"..fProbeOperationDistance.." F"..fProbeSpeed
    mc.mcCntlGcodeExecuteWait(finst,GCODE)
end

if (mc.mcInEditor() == 1) then
    M6()
end
Re: Creating an M6 Toolchange in Mach4 (Part 3)
« Reply #4 on: May 01, 2017, 02:05:14 PM »
I have used your tool change code.. after a little set in inch's it works great. One thing I would like to do is have the code turn off the spindle and wait for 12 sec or have the VFD trip a spindle has stopped before it moves. The Post code from Vcarve has the start up of the spindle and is working good.

Big thanks to your help as I have used other code and it always is great. Please keep up your help, there is a lot of us that need it.

Firechief
Stop Drop and Roll

Offline DazTheGas

*
  •  750 750
  • DazTheGas
    • View Profile
Re: Creating an M6 Toolchange in Mach4 (Part 3)
« Reply #5 on: May 01, 2017, 04:03:50 PM »
Thats quite a good point, since creating that script I have moved on to using vfd and spindle etc so it could do with a revamp. I see what I can muster up ;-)

DazTheGas
Theres always time for a choccy biccy
Re: Creating an M6 Toolchange in Mach4 (Part 3)
« Reply #6 on: May 03, 2017, 11:22:30 AM »
Just another point I found in the code you may like to fine tune. when the Z move up to your set point Z0, my Z0 will trip my limit switch. Sounds dumb but it took my some time to find out why it would not run the tool change. reset it to -2 and all was good.  :D
I'am just glad that the code is starting to make some logic to me. [Little]

BIG THANKS
firechief
Stop Drop and Roll
Re: Creating an M6 Toolchange in Mach4 (Part 3)
« Reply #7 on: May 08, 2017, 11:16:26 AM »
All my testing was done in the MDI window this M6 code work great... when I run it in the gcode it would not set the tool to the right height. (way off). What I found was the post Processor was adding a tool offset to the gcode on the next line in the gcode. I mod the post processor and remove it and then all was well. Big thanks for all your code.



Tim Smith


 
Stop Drop and Roll
Re: Creating an M6 Toolchange in Mach4 (Part 3)
« Reply #8 on: August 31, 2017, 03:41:21 PM »
The change i made to avoid Crash on approach did not behave as expected ( NOT WORKING AT ALL ;D)
So fixed now...And Some other stuff :P

I have not done any rigorus testing but tried some stupid stuff and the script still behaves...

New Version:

Code: [Select]
function M6()
    local inst = mc.mcGetInstance();
    local changeToTool = mc.mcToolGetSelected(inst)
    local changeFromTool = mc.mcToolGetCurrent(inst)
    local XPositionBeforeToolChange = mc.mcAxisGetPos(inst,0)
    local YPositionBeforeToolChange = mc.mcAxisGetPos(inst,1)
    local XToolProbePosition = "1"
    local YToolProbePosition = "1"
    local XManualToolChangePosition = "2"
    local YManualToolChangePosition = "2"
    local ColletAtProbeZCoordinate = -105 -- Machine Z-coordinate when collet tip touches TouchPlate (Must be more than ProbeOperationDistance - DefaultToolLength
    local ExtraProbeDistance = 5 -- SafetyMargin
    local ProbeOperationDistance = -30 -- Length of Probemove before giving up
    local ProbePrepSpeed = 100
    local ProbeSpeed = 25
    local DefaultToolLength = 70 -- Used if tool info is not found. (Should be a value slightly longer than the longest tool in the shop :D)
        -- QUICK REFERENCE
        -- G90 - Absolute (Go to coordinate)
        -- G91 - Incremental (Godistance along axis from current position)
        -- G53 - Machine Coordinate Move

    if changeToTool == changeFromTool then
    return
    mc.mcCntlSetLastError(inst, "ToolChange Activated But Not Required")
    else
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0\nM5" )
    RunProbe(inst,changeFromTool,XToolProbePosition,YToolProbePosition,DefaultToolLength,ColletAtProbeZCoordinate,ExtraProbeDistance,ProbePrepSpeed,ProbeSpeed,ProbeOperationDistance)
    local ToolZCoordinate = mc.mcAxisGetPos(inst,2)
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0 \n G90 G53 G0 X"..XManualToolChangePosition.." Y"..YManualToolChangePosition)
    local changeToToolDescription = mc.mcToolGetDesc(inst,changeToTool)
    wx.wxMessageBox("Please change to tool number "..changeToTool.." "..changeToToolDescription.." and press ok to continue")
    RunProbe(inst,changeToTool,XToolProbePosition,YToolProbePosition,DefaultToolLength,ColletAtProbeZCoordinate,ExtraProbeDistance,ProbePrepSpeed,ProbeSpeed,ProbeOperationDistance)
    mc.mcAxisSetPos(inst, 2 , ToolZCoordinate)
    mc.mcCntlGcodeExecuteWait(inst,"G90 G53 G0 Z0.0")
    mc.mcCntlGcodeExecuteWait(inst,"G90 G0 X"..XPositionBeforeToolChange.." Y"..YPositionBeforeToolChange)
    mc.mcToolSetCurrent(inst, changeToTool)
    wx.wxMessageBox("If Toolchange was Sucessful - click ok to continue")
    mc.mcCntlSetLastError(inst, "ToolChange Finished")
    end
end

function RunProbe(finst,ftool,fXToolProbePosition,fYToolProbePosition,fDefaultToolLength,fColletAtProbeZCoordinate,fExtraProbeDistance,fProbePrepSpeed,fProbeSpeed,fProbeOperationDistance)
    mc.mcCntlGcodeExecuteWait(finst, "G90 G53 G0 X"..fXToolProbePosition.." Y"..fYToolProbePosition)
    local toollen = mc.mcToolGetData(finst, mc.MTOOL_MILL_HEIGHT, ftool)
    if toollen == 0 then
        toollen = fDefaultToolLength
        mc.mcCntlSetLastError(finst, "Tool length not found - using Default Length")
    end
    local probestart = fColletAtProbeZCoordinate + fExtraProbeDistance + toollen
    local GCODE = "G91 G31 G0 Z"..probestart.." F"..fProbePrepSpeed
    GCODE = ""..GCODE.." \n G91 G0 Z1 F"..fProbePrepSpeed.." \n G91 G31 Z"..fProbeOperationDistance.." F"..fProbeSpeed
    mc.mcCntlGcodeExecuteWait(finst,GCODE)
end

if (mc.mcInEditor() == 1) then
    M6()
end

Hi, where do i set up manual toolchange position and fixed probe position ? Cant locate it in your script
Re: Creating an M6 Toolchange in Mach4 (Part 3)
« Reply #9 on: January 11, 2018, 07:49:50 PM »
Is this post dead? Or can I still get a response to a question?
Gene