I've been converting a Prolight 3000 w/ 8 position turret over the last week, and have a suitably working M6 macro to post and share as an example. This lathe uses a 1-way ratcheting turret driven by a stepper, and has a single home switch near tool 1 (where as I think Emco and Denford used DC motors and multi-switches for a gray-logic position feedback). The turret is run as the 'A Axis', and is calibrated so one rev is 360 degrees, like a rotary table. I'm happy with how easy it was to get the tool changer working, and get the whole lathe converted over to an AXBB from the separate control box with multiple cables. I still wish I could have found a Denford Cyclone, but I gave up and settled
The Prolight is a nice enough little bench machine.This code started as a sample I found on M3 forum for the basic change strategy, and was built upon to add tool number reformatting and return to last position as options. Hopefully this will be of use for someone else's project.
M6 sample (written in VB...
):- Code: Select all
#VB
' M6 Tool Turret macro for an 8 position stepper driven turret on a Prolight 3000 or similar lathe
' Turret is uni-directional rotation, single home switch at tool 1, and reverses to lock
' Need to set A (or chosen) axis to 360 degree / rev of turret, in my case, steps per unit was ~ 124 steps / degree.
' CCW move for locking was set by testing values to ensure lock without to much added stepper screech noise
' Code was ported from sample found on Mach3 forum, with additons for:
' Can accept double Tcode format (such as T0707) for tool 7, and makes it single digit for UCCNC
' User setable booleans to have tool return to position and show/hide messages
' Setable location for tool change in Machine coords.
'E Brust, 7/2021
If exec.IsLoading() Then 'Do Nothing, program loading
Else
' dim Variables
dim Num_Tools As Integer
dim CW_Feed As Integer
dim CCW_Feed As Integer
dim moves as integer
dim total_move as integer
dim CW_Move_Per_Tool as double
dim CCW_Move as double
dim Requested_Tool as string = exec.Getnewtool()
dim Current_Tool as integer = exec.Getcurrenttool()
dim Current_Feed as double = as3.Getfield(867) ' save current feedrate
dim Show_Messages as boolean
dim Return_Pos as boolean
dim Current_Offset as integer = exec.getactualmodalcode(12)
dim Current_AbsIncMode as integer = exec.getactualmodalcode(3)
dim Current_XLoc as double = exec.getXpos
dim Current_ZLoc as double = exec.getZpos
dim Safe_XLoc as double
dim Safe_ZLoc as double
'' Get actual modal code numbers for reference:
' 3: G90/91 INC/Abs
' 12: G54-G59 work offset
' 7: G40/41/42
' 2: G17/18/19
' 5: G93/94
'================= Use RegEx to sort out odd lathe tool formats, such as T0202 for tool 2...
Try
Dim num4 = "([0-9][0-9][0-9][0-9])" ' regex to match a 4 digit number
Dim num3 = "([0-9][0-9][0-9])" ' regex to match a 3 digit number
Dim num2 = "([0-9][0-9])" ' regex to match a 2 digit number
Dim num1 = "([0-9])" ' regex to match a number
Dim tMatch4 = System.Text.RegularExpressions.Regex.Match(Requested_Tool, num4, System.Text.RegularExpressions.RegexOptions.IgnoreCase)
Dim tMatch3 = System.Text.RegularExpressions.Regex.Match(Requested_Tool, num3, System.Text.RegularExpressions.RegexOptions.IgnoreCase)
Dim tMatch2 = System.Text.RegularExpressions.Regex.Match(Requested_Tool, num2, System.Text.RegularExpressions.RegexOptions.IgnoreCase)
Dim tmatch1 = System.Text.RegularExpressions.Regex.Match(Requested_Tool, num1, System.Text.RegularExpressions.RegexOptions.IgnoreCase)
Dim orderedString as string = ""
If tMatch4.Success Then '4 digits found
orderedString = tMatch4.Captures(0).Value
tMatch4 = System.Text.RegularExpressions.Regex.Match(orderedString, num4, System.Text.RegularExpressions.RegexOptions.IgnoreCase)
' Need to take only the first 2 of 4 (last two assumed junk or from lathe tool offset)
orderedString = microsoft.visualbasic.Strings.Left(tMatch2.Captures(0).Value, 2)
ElseIf tMatch3.Success Then ' 3 digits found
orderedString = tMatch3.Captures(0).Value
tMatch3 = System.Text.RegularExpressions.Regex.Match(orderedString, num3, System.Text.RegularExpressions.RegexOptions.IgnoreCase)
' Need to take only the first 1 of 3 (last two assumed junk or from lathe tool offset)
orderedString = microsoft.visualbasic.Strings.Left(tMatch2.Captures(0).Value, 1)
ElseIf tMatch2.Success Then ' 2 digits found
orderedString = tMatch2.Captures(0).Value
tMatch2 = System.Text.RegularExpressions.Regex.Match(orderedString, num2, System.Text.RegularExpressions.RegexOptions.IgnoreCase)
'Use 2 digits as found
orderedString = tMatch2.Captures(0).Value
ElseIf tmatch1.Success Then ' 1 digit found
orderedString = tmatch1.Captures(0).Value
'Use 1 digit as found
tmatch1 = System.Text.RegularExpressions.Regex.Match(orderedString, num1, System.Text.RegularExpressions.RegexOptions.IgnoreCase)
orderedString = tmatch1.Captures(0).Value
Else
orderedString = ""
'MsgBox("word problem getting tool num")
End If
requested_tool = orderedString
'Return orderedString
Catch ex As Exception
End Try
'================
as3.setfield(requested_tool, 2652)
as3.validatefield(2652)
'================
' set up some user set vars, Change these to match your machine needs...
Show_Messages = false ' Set true to show messages, false to not...
Return_Pos = true ' Set true to have tool moved back to last location after change
Num_Tools = 8 ' Number of tools in changer
CW_Feed = 3000 ' Forward rotration rate, degree/min, for changing
CCW_Feed = 2000 ' Reverse rotration rate, degree/min, for locking
CCW_Move = 7 ' Angle to reverse for locking, in degrees
Safe_XLoc = -.250 ' Machine X coordinate location to change tool at 0 is at top
Safe_ZLoc = -1.250 ' Machine X coordinate location to change tool at 0 is at far right
CW_Move_Per_Tool = 360/Num_Tools ' Do not change this, this is angle per tool based on number of tools
if(Current_Tool=0) then '// If new tool number is 0 means turret homed but did not set home position as tool 1
exec.Setcurrenttool(1) '; //Set the current tool -> the new tool
Current_Tool = exec.Getcurrenttool()
'return
end if
'Check for X, Z, and A axis to be homed. If tool changer is not 'A', change '59' to be for proper axis
if(not exec.GetLED(56) or not exec.GetLED(58) or not exec.GetLED(59)) then ' // If machine was not homed then it is unsafe to move in machine coordinates, stop here...
if Show_Messages Then
MessageBox.Show("The machine was not yet homed, do homeing before executing a tool change!")
end if
exec.Stop()
return
end if
while(exec.IsMoving)
end while
'================= start tool change here!
if Show_Messages Then
Messagebox.show("Requested Tool No=" & Requested_Tool)
end if
If Requested_Tool > Num_Tools Then
'if Show_Messages Then
Messagebox.show("Requested Tool No. too high, program stopped.")
'end if
exec.Code("M30")
return
End If
If Requested_Tool < 1 Then
'if Show_Messages Then
Messagebox.show("Requested Tool No. too low, program stopped.")
'end if
exec.Code("M30")
return
End If
If Requested_Tool = Current_Tool Then
' do nothing
Else
' lets change tools
If Requested_Tool > Current_Tool Then
moves = Requested_Tool - Current_Tool
end if
If Requested_Tool < Current_Tool Then
moves = Num_Tools - Current_Tool + Requested_Tool
end if
total_move = (moves * CW_Move_Per_Tool)+(CCW_Move/2)
'Move to safe position
exec.Code("G0 G53 Z" & Safe_ZLoc & " X" & Safe_Xloc)
'Pause for 1/2 second
exec.Code("G04 P0.5")
exec.Code("G91 G94") 'incremental & Feed per minute
exec.Code("G01 A" & total_move & " F" & CW_Feed)
exec.Code("G01 A-" & CCW_Move & " F" & CCW_Feed)
While exec.IsMoving()
end while
exec.wait(1000) ' Hold for a second so that TurnTable plugin can update offsets
if(not exec.Ismacrostopped()) '// If tool change was not interrupted with a stop only then validate new tool number
exec.Setcurrenttool(Requested_Tool) '; //Set the current tool -> the new tool
if Return_Pos=true
exec.Code("G90") ' back to absolute movement
exec.Code("G" & Current_Offset & "G0 Z" & Current_ZLoc & " X" & Current_XLoc)
While exec.IsMoving()
end while
end if
exec.Code("G" & Current_AbsIncMode) ' back to original abs/inc. mode
exec.Code("F" & Current_Feed) ' reset original feed
if Show_Messages Then
MessageBox.Show("Tool change done.")
end if
else
exec.StopWithDeccel()
'if Show_Messages Then
MessageBox.Show("Tool change was interrupted by user!")
'end if
end if
End If
End If
' end of tool change
Still on my to do list is a short macroloop code so that after A axis is homed, Tool1 will always be set as the 'active tool' in UCCNC. I assume macroloop is best way, as I'm not finding a way to use an axis home event to trigger a macro. If anyone knows different, let me know.
I'll be posting an update to the 'TurnTable' plugin later that adds additional controls to the interface, like initiating a tool change.
regards
Eric
