PyDNC - Python DNC script for CNC controls

Latest version, 2025 Jun 25, gzip'd tarball - cam_macros.py updated to have SPLIT_G53 and NO_SPLIT_G53 for Fadal G code. Fadal does not allow G0 and G53 in the same block, because reasons.

2025 Jun 5, gzip'd tarball

2025 May 30, gzip'd tarball

2025 May 21, gzip'd tarball

2025 May 7 version, gzip'd tarball

2024 Apr 22 version, gzip'd tarball

2024 Jan 4 version, gzip'd tarball

2023 Aug 4 version, gzip'd tarball

Fadal CNC88HS Post Processor for FreeCAD 1.0 CAM workbench

Yasnac MX3 Post Processor for FreeCAD 1.0 CAM workbench

Introduction

PyDNC is a Python script to send and receive files from CNC controls over a serial line. It uses the PySerial library for the serial port interface, so it should work fine on Windows, Unix, OS X, etc. It has been tested with USB to RS232 converters with Haas, Yasnac, and Fadal controls with no problems at up to 38400 bps. Provision is made for various data bit options, stop bit options, parity, and baud rates.

Of particular use is that when sending data to the control, the script checks for an XOFF code every character to prevent RS232 overrun problems in the ancient controls. Note that most current Linux serial drivers for USB converters do NOT implement software (XON/XOFF) flow control in the driver!

Other Scripts

From the README file in the archive:

These programs are useful for making, sending, and receiving CAM files to and from a CNC control. Particularly ancient controls without macros, subroutines, or general math processing. There are also programs for modifying g-code files, extracting the travel limits from a g-code file, and removing dis-allowed code from a g-code file.

dnc_renumber.py

Process a g-code file, renumbering the lines as it goes. Drops existing line numbers, and renumbers ALL g-code lines, except O-word and "%" lines. Set the line number offset, and the roll-over point for those controls with maximum line numbers.

dnc_stats.py

Compute various statistics of a g-code file. Mostly, find the min and max X, Y, Z values for each tool, in order. Reports the max and min coordinates for each tool, so an operator can work out if tools stick out far enough _before_ running the code.

dnc_strip.py

Strip all comments, line numbers, etc. from a g-code file for those controls that can't handle such stuff in a DNC file. Specifically, note that Fadal controls won't accept O-words, line numbers, or comments in a program being drip-fed to the control.

dnc_xform.py

Offset or scale all the X, Y, and/or Z values in a g-code file. Can also swap spindle speed and feed rate commands. The spindle and feed replacements are matching the spindle and feed rate, not the tool number! Can be very helpful for modifying a g-code file from one machine to another (different max spindle, max feed, etc.). Can also be used to mirror or offset code.

plot_gcode.py

Convert g-code file to positions for plotting with gnuplot. Input is a g-code file, output is a long series of x,y,z,mode lines for each move in the g-code file. The mode is taken from the currently active motion mode (0, 1, 2, 3) for each move. The mode number has 1 added to the number for plotting in gnuplot, as line color 0 is special.

cam_macros.py

Python pre-processor to make a DNC-ready g-code-only file from a source file with g-code, macros, and setup comments. The macros allow a higher level of cam programming than straight hand-coding the coordinates. With a CAD program that can provide a consistent set of x, y, z coordinates for corners, the macros can be used as a CAM programming language for 2.5-D cutting.

Fadal CNC88HS Post

The Fadal post-processor, fadal_post.py, is for the FreeCAD Path workbench, and produces g code that conforms to the Format 2 Fadal specification, which is closer to Fanuc dialect. The post does not currently handle tapping jobs correctly, although that may be partly due to issues with the Fadal mill being used for testing.

Improvements welcome, as they will only be made here as problems have to be overcome.

Yasnac MX3 Post

The MX3 post-processor, fadal_post.py, is for the FreeCAD Path workbench, and produces g code that conforms to the MX3 minimal dialext. The development controller does not have most of the options, but does include arcs! The post does not currently handle tapping jobs correctly, although that may be partly due to issues with the Fadal mill being used for testing.

Improvements welcome, as they will only be made here as problems have to be overcome.

---

cam_macros.py Macro Commands

Python pre-processor to make a DNC-ready g-code-only file from a source file with g-code, macros, and setup comments. The macros allow a higher level of cam programming than straight hand-coding the coordinates. With a CAD program that can provide a consistent set of x, y, z coordinates for corners, the macros can be used as a CAM programming language for 2.5-D cutting.

Create the source file with embedded setup comments starting with "#" - these comments must be the whole line! Embedded g-code does not have any particular marker - just enter g-code as it should be used. Macros start a line, and are the only item on a line - do not try to mix g-code or macros on the same line. Macro tokens take a list of parameters or other specific format; see below for the format for each token.

Recursion is supported in the subroutines and included files; lines are processed for macros at output. Macro expansion happens after coordinate replacement (in the subroutine).

This script takes input from stdin, and outputs to stdout and stderr. G-code output is on stdout, and notifications and setup comments (those lines starting with "#") are on stderr. Typical use:

[gungnir.local] cam_macros.py < source_file > dnc_gcode 2> setup_notes

Current tokens recognized as macros-
• NIBBLE_X
  

  NIBBLE_X Xxs,xe Yys,ye Sdelta

  
  

  NIBBLE_X X-8.0,-3.942 Y-0.2765,+0.2765 d0.100

  
  Nibble along X axis, from xs to xe in steps of at most delta. Each nibble runs from ys to ye. Use careful choice of start and end to implement climb or conventional milling.
• NIBBLE_Y
  

  NIBBLE_Y Xxs,xe Yys,ye Sdelta

  
  

  NIBBLE_Y X-12.410,-11.660 Y+0.2765,+0.5290 d0.100

  
  Nibble along Y axis, from ys to ye in steps of at most delta. Each nibble runs from xs to xe. Use careful choice of start and end to implement climb or conventional milling.
• PERIMETER
  

  PERIMETER Ddiameter L
      xxxx,yyyy[,zzzz]
      nan for coordinate means skip....
      END

  
  

  Run around a perimeter, in order. Code with individual points on each line (1 per line), ending with "END" on a line. Profile is only closed if start point added at end of list. Any coordinate entered as "nan" will be treated as the same as the last used coordinate. Z values optional on all lines, but only added if entered. X and Y coordinates needed for each line, even if Y is nan.

  If present, the D token specifies a tool diameter, and the perimeter coordinates are offset by the tool radius (diameter/2). The "L" token flips the side of compensation to the left, as viewed moving along the coordinates. Without the "L" token, compensation moves the tool to the right. Compensation should be correct for any angles and radius, although small areas which do not fit the tool may cause unexpected results. A perimeter which cannot fit the tool could cause incorrect or unusable tool paths!

• SUB
  

  SUB Xxs,xe Yys,ye Zzs,ze Sdelta
      g-code
      g-code
      .
      .
      .
      END

  
  

  Repeat a chunk of g-code once for each x,y,z value between zs and ze, tepping down by no more than delta. The entire chunk of code until END is repeated at each Z level, with a G1 Z move to each new depth at the start of each repetition. This is very similar to calling a subroutine in most controls, but can be used in those crippled controls without subroutines or macros. No provision for expanding macros inside the subroutine!

  Note that all listed axes will be stepped each repetition. This is helpful for turning the OD on a typical lathe. Also, if SET RAMP is active the axis changes will be done on the first line of the subroutine, rather than on a generated G1 move.

• INCLUDE
  

  INCLUDE filename

  
  Include the named file at this point. Lines are processed for macros, and expanded. This allows recursion of the macro expansion. Note that settings are global, and thus carry over from the enclosing file.
• HELIX
  

  HELIX Xx.xxxx Yy.yyyy Zz_start,z_end Sdelta Ddiameter Rradius N

  
  

  HELIX X-7.9000 Y0. Z0.00,-0.500 d0.0625 r0.1

  
  Radius is OUTER radius of helix, diameter is for tool offset (to inside). Delta is max step in Z per revolution. Adds extra revolution at end at final depth. If flag "N" set, does NOT end with a move to the center of the helix. Default is to end with a move to the center, like a hole is being cut.
• SLOT
  

  SLOT Xxs,xe Yys,ye Zzs,ze Rradius Sz_step C

  
  C is a flag for climb milling, CCW around slot Cut a slot from xs,ys to xe,ye at Z levels zs to ze in steps no larger than z_step. Slot cut with radius; if radius is 0 the slot will only move back and forth at constant Z.
• RAMP
  

  RAMP Xxs,xe Yys,ye Zzs,ze Rradius Sz_step C

  
  C is a flag for climb milling, CCW around slot Cut a slot from xs,ys to xe,ye at Z levels zs to ze in steps no larger than z_step. Slot cut with radius; if radius is 0 the slot will only move back and forth. This different from slot that Z move is done over first straight leg of the slot, then around arc, back leg, second arc at constant Z. Thus, ramps down into material then cuts around rest of perimeter of slot. If used with radius 0, ramps down to xe,ye and then cuts back to xs,ys at constant z, then ramps down again.
• TOOL
  

  TOOL number

  
  Tool change to tool "number". If g43 set, adds move to ztool with G43 H after tool change for setting tool offset. If g53 set, adds G0 G53 Z0. before M6 to move head.
• SET
  

        SET G43 - add g43 with z move after tool change
        SET G53 - add g53 Z0. before tool change
        SET ZTOOL - set Z-position for G43 move after tool change
        SET SPLIT_G53 - Split the G0 from the G53 Z0. before a tool
          change. Outputs a block with just "G0", then a block with
          "G53 Z0."
        SET NO_SPLIT_G53 - Use G0 G53 Z0. before a tool change, with the
          G0 and G53 Z0. in one block.
        SET NOC - turn off _all_ comments; strips comments from g-code
          and suppress macro comments
        SET COMMENT - turn on _all comments; leave g-code comments, and
          add macro expansion comments
        SET ARC2LINE - convert G2, G3 moves into G1 with line segments
        SET ARCP - set precision for converting arcs to lines
        SET ARCS - stop converting arcs to line segments
        SET NBLOCKS - output computed Nxxxx at the start of non-comment lines
        SET NONBLOCKS - turn off all Nxxx at the start of all lines
        SET NMAX - maximum line number; resets when reached
        SET NSTEP - increment Nxxxx line numbers by this much each time
        SET RAMP - In subroutines (SUB ...... END), change iterating axes on
          first line of subroutine, rather than direct G1 move added to
          subroutine.
        SET NORAMP - In subroutines (SUB .... END), change iterating axes
          at the start of each repetition on an added G1 move; then repeat the
          subroutine lines.
  

  Each set flag remains until explicitly cancelled.