GRBL post processor

[10bulls]

GRBL has certainly become popular in recent years.

I haven't yet tested this post processor on a GRBL, but if anyone would like to test and make suggestions for improvements, I would be very grateful.

The main change to this post from the default post processor is the replacement of drilling canned cycles with G0/G1 moves.

The 'Drill' post processor property is:

Code:

{$g0} {$_x} {$_y}
{$g0} Z{$mop.retractheight}
{$g1} {$_z} {$_f}
{$g0} Z{$mop.clearanceplane}

and 'Drill Dwell' is:

Code:

{$g0} {$_x} {$_y}
{$g0} Z{$mop.retractheight}
{$g1} {$_z} {$_f}
G4 {$p}
{$g0} Z{$mop.clearanceplane}

Peck drilling is currently not supported as this would require the post processor definitions to be able to handle more complex loops or scripts.
A post build command could be created to handle this.

I hope this post is useful starting point.

[gerritv]

I am evaluating CamBam for use with a 3D router based on Velmex positioners and Grbl. So far all is well but there were a few items to tinker with on the Post.
Attached is an updated version.

I will look at creating a custom post script for peck drilling, probably in vbs as opposed to Python

Gerrit

[gerritv]

Still chipping away at actual testing on a machine. As a result of my dissatisfaction with the available GUI's for Grbl I wrote my own. It is more machinist-friendly and in the process shows off Grbl's real capabilities quite well.

https://github.com/gerritv/Grbl-Panel/wiki

Gerrit

[BR52]

Hello Gerrit,

Seeing your GrblPanel the present project written in Visual Basic.
I converted for my Visual Studio 2010 and only changed the RepeatButton component.
The source code you presented, is changed and lack RepeatButton on "GrblGui.vb"
The main window is not the same here:
http://www.cambam.co.uk/forum/index.php?topic=4274.msg31530#msg31530

Please put the correct source code.
Place your EXE here on the forum.

   Armando

[gerritv]

The source code on Github compiles, works and is current. The exe is part of the zip file in the Release notes there.

I used VS 2103 Express. In your conversion to VS2010 you removed the Custom project (RepeatButton) but that has nothing to do with the button you pointed at. (The Solution has 2 projects, not 1)

Please raise questions/discussion on this at https://github.com/gerritv/Grbl-Panel/

Gerrit

[BR52]

I will not argue with you Gerrit.

What is important you put the file "GrblPanel.exe"

People do not have the compiler to generate the "GrblPanel.exe"

   Armando

[gerritv]

That is why on the github site there is a Release page that has a .zip file (bottom left side) that contains the program and its files. Ignore the .zip and .gz with the source code.

Again, go here https://github.com/gerritv/Grbl-Panel/releases

I will not post the code in multiple places, and certainly not on the CamBam site.

Gerrit

[MrJTJinx]

How do i use the drill profile.
I have this postprocessor loaded and have selected the drill profile and tried to enter as many variables as i can.
when i view the gcode i still get the code as if i were using the canned cycle only the canned cycle instruction is missing.
what i expected was that the code would replace the canned cycle with a list of G0/G1 instructions that GRBL would understand as it doesn't have canned cycles in its firmware library.

[pixelmaker]

GRBL doesn't support the drilling/pecking G-Codes natively.
Supported G-Codes in v1.1
G0, G1: Linear Motions
G2, G3: Arc and Helical Motions
G4: Dwell
G10 L2, G10 L20: Set Work Coordinate Offsets
G17, G18, G19: Plane Selection
G20, G21: Units
G28, G30: Go to Pre-Defined Position
G28.1, G30.1: Set Pre-Defined Position
G38.2: Probing
G38.3, G38.4, G38.5: Probing
G40: Cutter Radius Compensation Modes OFF (Only)
G43.1, G49: Dynamic Tool Length Offsets
G53: Move in Absolute Coordinates
G54, G55, G56, G57, G58, G59: Work Coordinate Systems
G61: Path Control Modes
G80: Motion Mode Cancel
G90, G91: Distance Modes
G91.1: Arc IJK Distance Modes
G92: Coordinate Offset
G92.1: Clear Coordinate System Offsets
G93, G94: Feedrate Modes
M0, M2, M30: Program Pause and End
M3, M4, M5: Spindle Control
M7* , M8, M9: Coolant Control
M56* : Parking Motion Override Control

Be careful, G80 is used by GRBL as "Motion mode cancel". In G code, G80 is the "Cancel canned cycle".

ralf

[MrJTJinx]

Thanks Ralf.

Unfortunately I am aware of the codes grbl uses.  this post starts with 10Bulls grbl post processor with a work around for grbl drilling but unfortunately I either don't know how to get it to work or it isn't working properly
please can you advise

[dh42]

Hello

what i expected was that the code would replace the canned cycle with a list of G0/G1 instructions that GRBL would understand as it doesn't have canned cycles in its firmware library.

This is the case, but only for G81 and G82 (drilling and drilling with a break at the bottom) ; G83 (Peck drill) is not yet handled because there is currently no way to make math and loops with the post processor.

Remember that GRBL was not designed to drive a milling machine but it was developed for engraving machine (laser), so no needs for canned cycle or toolchange on this kind of CNC.

On the example file, if I use the Mach3 PP I get this Gcode for a hole of 10mm depth (simple drill and drill with 1s break at the end)

T5 M6
( Drill1 )
(  )
G17
S12500
M3
G0 X0.0 Y0.0
G0 Z5.0
G98
G81 Z-10.0 R0.0 F600.0
G80
( Drill2 )
(  )
G0 Z5.0
G0 X19.0
G98
G82 Y0.0 Z-10.0 P1.0 R0.0 F600.0
G80
G0 Z5.0
M5
M30

and if I switch to GRBL PP I get

T5 M6
( Drill1 )
G17
M3 S12500
G0 X0.0 Y0.0
G0 X0.0 Y0.0
G0 Z0.0
G1 Z-10.0 F600.0
G0 Z5.0
( Drill2 )
S12500
G0 X19.0
G0 X19.0 Y0.0
G0 Z0.0
G1 Z-10.0 F600.0
G4 P1.0
G0 Z5.0
M5
M30

++
David