Surfacing Macro
-
@cthulhulabs wow, thats really nice.
how is the cutter diameter set so each movement in Y isn't too large/too small? -
@jay_s_uk you just adjust the step over. So if you were using a 1/4in end mill you'd set the step over to like 2mm. I'm using a 1" surfacing bit so I set it to 10mm. Seems to leave a nice finish.
-
@cthulhulabs fantastic! I look forward to trying this when I next need it
-
@cthulhulabs This is really impressive! Thanks for sharing. I plan on trying it out soon myself!
-
@sindarius / @jay_s_uk
Get a chance to try this out? Trying to see if there are any ways to improve it. -
@cthulhulabs It's been too cold in my garage to want to do any woodworking at the moment
I do have the macro copied over to my machine once it warms up enough to be in there.
-
It would be nice if this macro could be made into a plugin. Then you wouldn't have to edit the macro to change parameters. Something like the CNC touchprobe plugin by @raymondstone
-
damn that would be another reason for me to update my old duet2w from RRF2.1 to 3.3
no build another cnc first -
I tested this macro today. Works nicely, had to edit some parameters for my Ooznest touchprobe input. Thanks a lot
; Adjust probe for low speed probing M558 K0 P8 C"!e0stop" H20 F120 T300 ; Z probe number - Z probe switch type - probe recovery 1s probe speed and travel speed
-
@cthulhulabs i like this macro! I am trying ot use it by I am encountering a couple of hiccups. I know this is an older thread, but I am hoping you might see this reply.
-
Are you using a PanelDue in conjunction with your machine?
-
Where/how are you controlling your spindle?
-
I am getting funny outputs with the move command prompts on PanelDue. I get the first one for probing Z. but not for any of the other ones. M291 Syntax looks correct. I am trying to get a PC near the machine to see what the console looks like.
M291 P"Insert your surfacing bit into your spindle and position it above the probe plate" R"Probing" S3 X1 Y1 Z1 ; Set bit above center of probe G91 ; relative positioning ; Probe Z component G38.2 Z{move.axes[2].userPosition - (var.ProbeThickness + 2.25)} ; seek until the probe circuit is closed Z-axis 25 mm G0 Z{var.ZClearanceHeight} ; rapid move Z axis 5 mm G10 P1 L{var.CoordSystem} Z{var.ProbeThickness + var.ZClearanceHeight} ; store relative probe offset for coordinates system 1 G90 ; Absolute positioning M291 P"Move to the starting X Y position for surfacing" R"Start Position" S3 X1 Y1 Z0 set var.StartX = move.axes[0].userPosition; set var.StartY = move.axes[1].userPosition; if var.Debug M118 P0 S{"StartX = " ^ var.StartX} L2 M118 P0 S{"StartY = " ^ var.StartY} L2 M291 P"Move to the ending X Y position for surfacing" R"End Position" S3 X1 Y1 Z0 set var.EndX = move.axes[0].userPosition; set var.EndY = move.axes[1].userPosition;
- How or where are you turning your spindle on? As mine is controlled through RRF, I need to insert the tokens to turn off/on. I am thjnking before and after the while loop?
T1 G90 M03 S5000 G04 S1 G0 X0.0000 Y0.0000 Z3.0000 ; Begin surfacing loop while true ... ... M291 P"Surface another layer?" S3 X0 Y0 Z0 ; then prompt the user if they want to do another layer M03 S3500 ; ramp spindle speed down G04 S1 M03 S1500 G04 S1 M05 G04 S1 G90 G0 X0.0000 Y0.0000 Z3.0000
-
-
@sinned6915 I have modified the macro for an Ooznest Workbee with their latest Firmware (RRF3.3). M3 starts the router and M5 stops it.
; Constants var Debug = false; var ProbeThickness = 5; var CoordSystem = 20; var StepOver = 10; var DepthOfCut = 0.2; var FeedRate = 8000; var ZClearanceHeight = 25; ; Variables var StartX = 0; ; The X starting position var StartY = 0; ; The Y starting position var EndX = 0; ; The X ending position var EndY = 0; ; The Y ending position var YDir = 0; ; The direction to go in Y var YDist = 0; ; The distance to go in Y var YPos = 0; ; The position in Y to move to var YDistLeft = 0; ; How much we have left to move in Y var ZDepth = 0; ; How far down we should be in Z var XSorE = "End" ; Whether X should move towards the start or the end position ; If the printer hasn't been homed, home it if !move.axes[0].homed || !move.axes[1].homed || !move.axes[2].homed G28 ; Adjust probe for low speed probing M558 K0 P8 C"!e0stop" H20 F120 T300 ; Z probe number - Z probe switch type - probe recovery 1s probe speed and travel speed G31 K0 P500 X0 Y0 Z0 ; Set trigger value - set offset and trigger height - Z probe number M291 P"Insert your surfacing bit into your spindle and position it above the probe plate" R"Probing" S3 X1 Y1 Z1 ; Set bit above center of probe G91 ; relative positioning ; Probe Z component G38.2 Z{move.axes[2].userPosition - (var.ProbeThickness + 2.25)} ; seek until the probe circuit is closed Z-axis 25 mm G0 Z{var.ZClearanceHeight} ; rapid move Z axis 5 mm G10 P1 L{var.CoordSystem} Z{var.ProbeThickness + var.ZClearanceHeight} ; store relative probe offset for coordinates system 1 G90 ; Absolute positioning M291 P"Move to the starting X Y position for surfacing" R"Start Position" S3 X1 Y1 Z0 set var.StartX = move.axes[0].userPosition; set var.StartY = move.axes[1].userPosition; if var.Debug M118 P0 S{"StartX = " ^ var.StartX} L2 M118 P0 S{"StartY = " ^ var.StartY} L2 M291 P"Move to the ending X Y position for surfacing" R"End Position" S3 X1 Y1 Z0 set var.EndX = move.axes[0].userPosition; set var.EndY = move.axes[1].userPosition; if var.Debug M118 P0 S{"EndX = " ^ var.EndX} L2 M118 P0 S{"EndY = " ^ var.EndY} L2 M291 P"Are you ready to begin surfacing?" S3 X0 Y0 Z0 ; Figure out which direction in Y we are going if var.EndY < var.StartY set var.YDir = -1; elif var.EndY > var.StartY set var.YDir = 1; else set var.YDir = 0; if var.Debug M118 P0 S{"YDir = " ^ var.YDir} L2 set var.YDist = {abs(var.StartY - var.EndY)}; if var.Debug M118 P0 S{"YDist = " ^ var.YDist} L2 ; Begin surfacing loop while true if var.Debug M118 P0 S"Begin Layer Loop" L2; set var.ZDepth = {var.ZDepth - var.DepthOfCut}; set var.YDistLeft = {var.YDist}; ; go to the start X and Y position then down to Z Depth if var.Debug M118 P0 S{"Move to start X" ^ var.StartX ^ ",Y" ^ var.StartY} L2 T1 M3 S17500 ;M42 P1 S1 G0 X{var.StartX} Y{var.StartY} if var.Debug M118 P0 S{"Move to start Z" ^ var.ZDepth} L2 G1 Z{var.ZDepth} ; we should be at the Start X position so move to the End X position if var.Debug M118 P0 S{"Move to X" ^ var.EndX} L2 G1 X{var.EndX} F{var.FeedRate} set var.XSorE = "Start" while var.YDistLeft > var.StepOver if var.Debug M118 P0 S"Begin Y Loop" L2 ; move in Y by StepOver set var.YPos = {move.axes[1].userPosition + (var.StepOver * var.YDir)} if var.Debug M118 P0 S{"Move to Y" ^ var.YPos} L2 G1 Y{var.YPos} F{var.FeedRate} set var.YDistLeft = {var.YDistLeft - var.StepOver} if var.XSorE == "Start" ; move X to the start position if var.Debug M118 P0 S{"Move to X" ^ var.StartX} L2 G1 X{var.StartX} F{var.FeedRate} set var.XSorE = "End" else ; move X to the end position if var.Debug M118 P0 S{"Move to X" ^ var.EndX} L2 G1 X{var.EndX} F{var.FeedRate} set var.XSorE = "Start" ; move in Y the rest of the distance left set var.YPos = {move.axes[1].userPosition + (var.YDistLeft * var.YDir)} if var.Debug M118 P0 S{"Move to Y" ^ var.YPos} L2 G1 Y{var.YPos} F{var.FeedRate} ; one last move in X if var.XSorE == "Start" ; move X to the start position if var.Debug M118 P0 S{"Move to X" ^ var.StartX} L2 G1 X{var.StartX} F{var.FeedRate} set var.XSorE = "End" else ; move X to the end position if var.Debug M118 P0 S{"Move to X" ^ var.EndX} L2 G1 X{var.EndX} F{var.FeedRate} set var.XSorE = "Start" G0 Z{var.ZClearanceHeight} ; get out of the way M400 ; wait for the movement buffer to catch up M5 ;M42 P1 S0 M291 P"Surface another layer?" S3 X0 Y0 Z0 ; then prompt the user if they want to do another layer
-
@chimaeragh thank you. i am downloading now and will try it again.
-
@sinned6915 Line 89 selects the tool (T1). If your spindle is set to tool 0 (T0) change it accordingly. Line 90 sends the M3 command to start the spindle.
-
@sinned6915 sorry for the late reply. Have not been on this forum for a while. No I am not using a PanelDue. I am using a Pi with an HDMI touch screen monitor. As for spindle I am using a Brushless Dewalt Trim Router with the ESC replaced with an ODrive. It currently requires running commands from odrivetool on the Pi.
@chimaeragh what all did you change in your version? I just upgraded to an ODrive Pro and can finally use an ADC input to control my spindle.
-
@cthulhulabs My DeWalt is configured as a spindle and is automated via a relay. So I can use M3 to start it and M5 to stop it. (Already modified my Vectric postprocessor for this)
I added M3 and M5 commands into the surfacing loop at line 89 and line 148 of the macro.T1 ; selects the spindle Tool 1
M3 S17500 ; starts tool
-
@chimaeragh Cool. There is a variable at the top for the spindle RPMs. Now that my spindle RPM can be controlled by the Duet I plan to add it. You should probably use that in your M3 command.
I am thinking of rewriting this Macro to only cut in one direction to give a more uniform surface finish. Basically cut from Left to Right, raise up, rapid to the next cut, lower and repeat. There would be a flag in it to change it between Left to Right and Right to Left. Might also add a flag to go from top to bottom or bottom to top.
-
@CthulhuLabs I use your surfacing.g code on a regular basis. Love it.
But is there any way to modify it so that the Depth of Cut could be adjusted by user input?It would be nice to be able to enter a different value each time I use this macro, without having to edit the code. It would be even nicer if the DOC could be modified on each susbequent pass ("run again"). Perhaps also to limit the input value to between 0.1mm and 3.0mm?
-
I know you can pass parameters to a macro in the macro call itself (e.g. depth of pass)
Manually choosing this value on each run of the macro may be possible now using M291 on 3.5 beta firmware.
-
@HebigT Yes, I did look into the M291 function, but sadly, I am still on the v3.3 (awaiting any update from Ooznest)!!
Does this mean that there is no other way to program in a variable DOC? Apart from setting up numerous versions of the macro, each with a different value for the doc? -
With 3.3 you should still be able to pass a parameter in the macro call. You’ll just have to modify the macro (hopefully only once!) to assign that parameter to the DOC variable (e.g. var DepthOfCut= {param.y} )
It’ll still be a manual process of entering the parameter each time you start the macro, but it should save you the trouble of having to change the DOC variable within the macro each time.See the macro parameter section at this link:
https://docs.duet3d.com/User_manual/Reference/Gcode_meta_commands