Announcement

Collapse
No announcement yet.

Fast Tool Change Option for Non ATC Machines

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts
  • #16

    Here's how it works:
    Save all toolpaths to one file as with a tool changer.
    When the machine see's a toolpath change in the gcode it will move the spindle to the home position and prompt for a bit change.
    Then it will measure the tool using the bit measure switch that comes with the FTC package.
    Then it moves the spindle back to the home position and prompts to replace the dust boot and continues with the carve.

    It really saves a lot of time compared to loading each toopath individually and resetting z-zero. Unfortunately, the prompt to change the tool does not include the tool name. All of the tools are listed at the top of the gcode file so...
    Last edited by SteveNelson46; 03-22-2024, 12:25 PM.
    Steve
    __________________
    Camaster Stinger 1 with Recoil (2019)
    FTC
    1hp Spindle
    Laser crosshair
    Wireless Pendant
    Aspire 11.5
    Rhino 8
    Fusion 360

    Comment

    • #17

      Originally posted by SteveNelson46 View Post
      It really saves a lot of time compared to loading each toopath individually and resetting z-zero. Unfortunately, the prompt to change the tool does not include the tool name. All of the tools are listed at the top of the gcode file so...
      It’s possible to have the tool name displayed. You just need to change the Vectric post processor: https://forum.vectric.com/viewtopic....224455#p224455

      I also changed the macros to not have the pause on a tool change because the post was doing it with the toolname. It’s possible to just add the tool name, remove the pause, and leave the macros alone.
      Gary
      2018 Stinger II SR-44 with GCnC WinCNC Backplane, ClearPath Servos, 3HP RM30C ATC CNCDepot Spindle, 16 Tool Carousel, Custom Automatic Height Dustboot, Performance Premium, Recoil, Gantry Lift, Cyclone
      Fusion 360
      Aspire

      Comment

      • #18

        Gary, will you please provide an example of what you modified to get the tool name displayed at change prompts? Thanks in advance!
        ---
        Jim Becker

        SR-44 (2018), 1.7kw spindle, Performance Premium, USB, Keypad, T-Slot table (y-axis configuration), WinCNC, VCarve Pro upgraded to Aspire

        Non CNC stuff...

        SCM/Minimax
        Festool "a good collection"
        Stubby - lathe
        Harvey G700 DC
        more...

        Retired from full time work in the telecom industry 9/2017
        Occasional commission work for others, but mostly for me...furniture/tack trunks/signage/guitars
        Located Bucks County PA

        Comment

        • #19

          For what it is worth... Here is my post processor for FTC tool change that is from 2013. It is what I have been using with Aspire since that time. It places the tool name just slightly above the text rows I can view in the WinCNC viewer when I am making a tool change. I just scroll up a couple clicks and I can make sure I am loading the right tool.

          +================================================
          +
          + Block definitions for toolpath output
          +
          +================================================

          +---------------------------------------------------
          + Commands output at the start of the file
          +---------------------------------------------------

          begin HEADER

          "[N] [91][TP_FILENAME][93]"
          "[N] G90"
          "[N] "
          "[N] M5"
          "[N] G53 Z0"
          "[N] "
          "[N] [91][TOOLNAME][93]"
          "[N] T[T] [91] GET TOOL NUMBER [T] [93]"
          "[N] "
          "[N] [S] [91] SET SPINDLE SPEED RPM [93]"
          "[N] M3 [91]SPINDLE ON[93]"

          "[N] "
          "[N] G00 [XH] [YH]"
          "[N] G53 Z0"
          "[N] "


          +---------------------------------------------------
          + Commands output at toolchange
          +---------------------------------------------------

          begin TOOLCHANGE

          "[N] M5"
          "[N] G53 Z0"
          "[N] "
          "[N] [91][TOOLNAME][93]"
          "[N] T[T] [91] GET TOOL NUMBER [T] [93]"
          "[N] "
          "[N] [S] [91] SET SPINDLE SPEED RPM [93]"
          "[N] M3 [91]SPINDLE ON[93]"

          "[N] "
          "[N] G53 Z0"
          "[N] "
          "[N] G00 [XH] [YH]"
          "[N] G00 [ZH]"

          +---------------------------------------------------
          + Commands output for rapid moves
          +---------------------------------------------------
          Charlie L
          Stinger II, 48 by 48, 1.7 kW Spindle, FTC + Laser + Recoil + Vacuum, July 2012
          WinCNC 2.5.03, Aspire, PhotoVCarve, Windows 7 Pro SP1

          Comment

          • #20

            Jim, pretty much what's in the Vectric post. It's similar to what Charlie did above.
            T<tool number> is the command to change to a different tool number.
            [91] is open bracket, [93] is close bracket for the comment after the T* command
            So:
            T[T] [91] GET TOOL [TOOLNAME] [93]"

            Is all you really need. It's similar to Charlie's, except it puts the tool name right at the T command.

            Or were you asking about changes to the FTC toolchange macro?
            Gary
            2018 Stinger II SR-44 with GCnC WinCNC Backplane, ClearPath Servos, 3HP RM30C ATC CNCDepot Spindle, 16 Tool Carousel, Custom Automatic Height Dustboot, Performance Premium, Recoil, Gantry Lift, Cyclone
            Fusion 360
            Aspire

            Comment

            • #21

              What you both posted answers what I was asking. Thanks.
              ---
              Jim Becker

              SR-44 (2018), 1.7kw spindle, Performance Premium, USB, Keypad, T-Slot table (y-axis configuration), WinCNC, VCarve Pro upgraded to Aspire

              Non CNC stuff...

              SCM/Minimax
              Festool "a good collection"
              Stubby - lathe
              Harvey G700 DC
              more...

              Retired from full time work in the telecom industry 9/2017
              Occasional commission work for others, but mostly for me...furniture/tack trunks/signage/guitars
              Located Bucks County PA

              Comment

              • #22

                IMG_9817.png
                Charlie L
                Stinger II, 48 by 48, 1.7 kW Spindle, FTC + Laser + Recoil + Vacuum, July 2012
                WinCNC 2.5.03, Aspire, PhotoVCarve, Windows 7 Pro SP1

                Comment

                • #23

                  I need to clarify something - when I added the tool name AFTER the T command, I'd modified my G37Z.MAC macro to NOT do the pause for the dustboot removal. I'd put that code inside the post processor. So if you don't want to modify your macro, you should just do what Charlie did. My PostP had this:

                  +---------------------------------------------------
                  + Commands output at the start of the file
                  +---------------------------------------------------

                  begin HEADER

                  " [91]VECTRIC CNC OUTPUT FOR CAMASTER TOOLCHANGE [93]"
                  " [91]MACHINES WITH WINCNC CONTROL ONLY[93]"
                  " "
                  " [91]FILENAME: [TP_FILENAME][93]"
                  " [91][TIME], [DATE][93]"
                  " "
                  " [91]MATERIAL size: [XLENGTH][34] x [YLENGTH][34] x [ZLENGTH][34][93]"
                  " [91]Z Zero Position: [Z_ORIGIN][93]"
                  " "
                  " [91]TOOL LIST[93]"
                  " [91][TOOLS_USED][93]"
                  " "
                  " G90 [91]ABSOLUTE MODE[93]"
                  " "
                  " M5 [91]SPINDLE OFF[93]"
                  " G53 Z0 [91]LIFT Z TO TOP[93]"
                  " "
                  " G53 x24 Y8"
                  " [91] REMOVE DUST BOOT AND"
                  " [91] CHANGE TO '[TOOLNAME]' BIT"
                  " [91] FOR TOOLPATH '[TOOLPATH_NAME]'"
                  " [91]THEN PRESS ENTER [93]"
                  " G4"
                  " [91] [TOOLPATH_NAME] [93]"
                  " T[T] [91] GET TOOL [TOOLNAME] [93]"
                  " "
                  " [S] [91] SET SPINDLE SPEED RPM [93]"
                  " M3 [91]SPINDLE ON[93]"
                  " "
                  " G53 Z0 [91]LIFT Z TO TOP[93]"
                  " "
                  " [91]TOOLPATH NAME: [TOOLPATH_NAME][93]"
                  " F[FC] XY [91]SET FEEDRATE FOR X AND Y[93]"
                  " F[FP] Z [91]SET FEEDRATE FOR Z[93]"
                  " "


                  +---------------------------------------------------
                  + Commands output at toolchange
                  +---------------------------------------------------

                  begin TOOLCHANGE

                  " M5"
                  " G53 Z0"
                  " "
                  " G53 x24 Y8"
                  " [91] REMOVE DUST BOOT AND"
                  " [91] CHANGE TO '[TOOLNAME]' BIT"
                  " [91] FOR TOOLPATH '[TOOLPATH_NAME]'"
                  " [91]THEN PRESS ENTER [93]"
                  " G4"
                  " [91] [TOOLPATH_NAME] [93]"
                  " T[T] [91] GET TOOL [TOOLNAME] [93]"
                  " "
                  " M3 [91]SPINDLE ON[93]"
                  " "
                  " G53 Z0"
                  " "

                  Also, because someone asked about details, I assume you've put your frequently used (ie CAMaster) PostP files in a My_PostP directory (as per Vectric instructions). The file you want to modify is CAMaster ToolChange INCH.pp (I think - looking at a backup on network drive, and not on my machine). Don't forget to fix the recoil pp too if you have one and you modify G37Z.MAC. Otherwise bad things will happen...

                  Charlie, if you don't want to have to scroll back, you could use this method. Another option is to modify cncscrn.ini and change the size of the output window to make it a bit bigger. But then you'll probably have to be moving buttons around and probably fix the background bitmap.
                  Gary
                  2018 Stinger II SR-44 with GCnC WinCNC Backplane, ClearPath Servos, 3HP RM30C ATC CNCDepot Spindle, 16 Tool Carousel, Custom Automatic Height Dustboot, Performance Premium, Recoil, Gantry Lift, Cyclone
                  Fusion 360
                  Aspire

                  Comment

                  Working...
                  X