From: none@none.com99   
      
   On 11/5/2024 6:53 PM, Jim Wilkins wrote:   
   >> So is it a compiler?  ... No I think its best described as a   
   >> specialized interpreter.   
      
      
   > I simply wondered if CAD systems typically generated readable and   
   > editable G code.   
      
   Ready for it?   
      
   No.  Cad generates pretty pictures.  CAM generates g-code (or other code   
   possibly).   
      
   Yes, generally g-code is a simple text file with no hidden characters   
   other than a line break.   I'm not sure that's the correct character.   
   It might be a hard return.  Whatever notepad generates when you hit the   
   enter key is it.  I forget.  Its been a long time since I looked at that   
   stuff.  Anyway a simple text file can be edited in windows notepad.  In   
   fact its my default to open an .nc file in Windows if I click on it.   
   .nc .tap .txt or virtually any other extension will work as long as your   
   control software will show and open the file.  .nc is the default I use.   
     Mach 3 used .tap by default, but I prefer .nc because it says what it   
   is.  A numerical control file.   
      
   Embedded documentation is a mixed bag.  Some CAM programs will document   
   basics automatically if set to do so.  Most probably.  Most modern   
   controllers will just ignore comments, but some (mostly early g-code   
   adopters on under powered processors) will reject anything that is not   
   an executable line of code and not execute at all or throw an error.   
      
   "Well, WELL! WELLL!," you might say.  "What about Fusion360?" you might   
   ask.  There are lots of CAD/CAM programs, but CAD and CAM are two   
   different things.  In Fusion the functions are tied together so a CAD   
   modification will automatically create different code (if it doesn't   
   cause a failure) the next time you generate code.  With no other steps   
   it will generate code based on the new CAD model.  There are a fair   
   number of seemingly commingled CAD/CAM programs these days.  Fusion360,   
   BobCAD/CAM, etc.  Even many purely CAD programs of the past now have   
   plugin's or integrations with CAM programs.  Even FreeCAd now has   
   available a "workbench" that can be used for CAM, and CamBam has many   
   simple CAD tools built in.  Still CAD and CAM are two different things.   
   CAD generates pretty pictures and CAM generates g-code.   
      
   G-Code is just text.  For a programmer its pretty easy to read and   
   understand, but except for a few global settings (work offsets, base   
   scale, velocity mode, and some parameters) each line is standalone.  It   
   executes the current line base on the information you have and the   
   current position and status of the machine.   
      
   If you have a list of simple "G01 X(x) Y(y) F(f)" it will execute each   
   one in order doing what you told it to do.  If you used four of those   
   bracketed by other overhead commands to cut a rectangle it will cut your   
   rectangle one line at a time by going from the current location   
   (whatever it is) to X(x) Y(y) in a straight line at a speed of F(f).  If   
   you decide you need to modify your rectangle you would need to modify   
   TWO (2) lines of code.  This is an over simplification, but it   
   illustrates why some people get in trouble hand editing code.   
   Understanding what a line of code does it a matter of looking up that   
   code and how its executed based on the parameters given, and to a   
   limited extent how the control software implements it.  The number of   
   commands (G Codes and M Codes) is rather small.  There are also   
   parameters for a single code that can be global until changed.  For   
   example drilling operations often will pass on all parameters except the   
   coordinates.  If you are drilling a list holes all the parameters that   
   apply may only be in the first line of code to drill the first hole.  If   
   you decided to change one in the middle of that list by adding   
   parameters every hole after that would have the new parameters.  Maybe   
   that's what you want, and maybe you just blew your part.   
      
   Yes, its readable.  I think any even hack programmer would pick up the   
   basics pretty quickly.  Yes its editable.  You really need to understand   
   the whole string of events before you do.   
      
   I actually started out CNC machining functionally without CAD or CAM.  I   
   wrote out g-code by hand and used a spreadsheet to generate iterative   
   code, and exported the text values of my formulas to copy into a text   
   file.   
      
   An issue I ran into is that often the CAM software does not output   
   parameters or lines of code that it doesn't know (because of something I   
   did) that it needs to.  A tool change macro would be such an example.   
   If I move the machine in order to execute a tool change the CAM software   
   that did its job at most recent minutes ago, and maybe days or years   
   ago, didn't know that was going to happen.  When it starts the next   
   operation it thinks its still in the same place.  I had to go back into   
   my macro (part of the control software), save the current coordinates in   
   the current work offset, execute the rest of the tool change, and then   
   return to those coordinates. Specifically for tool changes I would move   
   the table back out of the way, or on a router I might move the gantry to   
   the front of the table either automatically in the macro or manually   
   with the jog functions of the machine (if it allowed it).  On another   
   machine for tool changes it would just STOP.  On that one I modified my   
   post processor insert a machine coordinate Z height move that brought Z   
   to zero leaving room for the tool change.   
      
   Even if you ONLY have CAM generate code for the program you still may   
   need to write a machine specific macro or modify the post processor of   
   the CAM program to add necessary code.  Even if you never manually edit   
   program code you still may find it beneficial to know how.  On the other   
   hand if you are just an operator then other people will do all of that.   
   You just load the stock and push the start button.  You may not even   
   have to check your parts.  The quality control people will do that.   
   Then somebody will determine if you are running the machine wrong, if   
   its setup wrong, or its designed (CAD/CAM) wrong.   
      
   --   
   Bob La Londe   
   CNC Molds N Stuff   
      
   --   
   This email has been checked for viruses by AVG antivirus software.   
   www.avg.com   
      
   --- SoupGate-Win32 v1.05   
    * Origin: you cannot sedate... all the things you hate (1:229/2)