Here are a few notes I made while learning GCODE. It is written from the perspective of a person who already knows a scripting languages.
I hope it helps. Let me know about any suggested changes at joe@xdobs.com or if you would like some help extending our library for your project.
Most people do not need to learn GCODE because the normal CNC process allows people to use CAD and CAM software to generate the GCODE from their 3D CAD drawing. We encountered problems with the normal process which encouraged us to write CNCUtil, a Ruby library that directly produces the GCODE
GCODE is a language that is so simple that you can learn the basics and do real work in a few hours. Even the more sophisticated things are easy to understand.
GCODE is also one of the worst languages I have ever seen if you have to edit large scripts. All the tools that software engineers use to manage complex systems such as functional decomposition and encapsulation are missing. Sophisticated GCODE scripts are quite often over 10,000 lines and if you have to find one particular line to edit it can require scanning all 10,000 lines. The simulators help but not nearly as much as real engineering tools do.
The reason I wrote our ruby scripting library CNCUtil to Automatically generate GCODE from higher level specifications is that our projects where simply too complex. We could not afford to to sit around writing 10,000 lines of GCODE and then have to edit 3,000 of them to make a simple change. CNCUtil has been quite successful so that 10,000 lines of GCODE can be generated from 10 to 15 lines of ruby script and if I change a dimension it is normally only a one line code change. I often find it is faster to use CNCUtil that it was to draw the part in CAD and then convert it to GCODE. CNCUtil also comes closer to generating ideal GCODE. I also like CNCUtil because it automatically takes care of most of the MATH which consumes a lot of the GCODE programming time.
I do not claim this tutorial is technically correct but it does work with the EMC2 CAM driver software when hooked to a Xylotex controller board.
My mill is a Taig 2019 micro mill. It is one where the milling
head stays stationary on the X and Y axis while the table moves under the head.
The head moves up and down on the Z axis. This means that when the table
moves in one direction the stationary head is actually moving in the opposite
direction relative to the material
It is important to logically think about the head movement relative to the work piece. It is easy to get table movement mixed in and it will cause you to mix up directions every time.
In otherwords pretend that the material was always stationary and that the head is the item moving.
Always think in head movement relative to the material even if it is the table or part moving.
Increasing X will move milling head Right by moving the table left. On my Taig this moves the table to the left. Moving from the extreme right to the extreme left this mill allows 14.5 inches of movement. I always set mine up so that the table marked dead center is X = 0 so that it can move from a X of -7.25 to X+7.25. I try to never use the to allow some room just in case the alignment is off. On larger pieces I use the plus and minus axis but on smaller pieces I tend to work always on the + side.
A decrease in x will move milling head left on my Taig this moves the table towards the back or towards the main support column. From it's most extreme forward position it can move a maximum of 4.5 inches but about 0.6 inches of this is blocked by the bottom of the Z axis gearing which means that if you are milling anything over 1 inch thick you really only have 4 inches of movement. I align mine so that Y is set to 0 at the forward edge of the work piece which allows quick and dirty alignment check by running back and forth on the X axis. I normally configure mine so that I can move up to 4.0 inche on the Y axis and back to -0.5 but generally always work in the + coordinate space.
Decreasing y will move the head back. It actually moves the table towards me if I am standing in front of the mill which moves the part away from the wall but when looked at it relative to the material it is logically moving the head toward the wall which is opposite the table direction.
All milling operations are done relative to X=0, Y=0, Z=0. The EMC2 software allows you to manually move the head and then set each axis to zero. This means your code can be designed to work from any corner of the piece or the center if needed. In practice it is generally a good rule to use the one corner as the of the work material as the 0. There are times when it makes more sense to start in the center for one or more axis. On our parabola project the front edge on the Y axis is 0 but the center of the 15 inch work piece is 0 on the Z axis.
By default all coordinates are in an absolute grid space relative to X=0,Y=0,Z=0, It is possible to change the current state and make movements relative but we normally leave things in the absolute space as it is easier to keep track of. If I was doing a lot of manual GCODE instead of using our library I would probably use the relative space more often.
Note: There is an option in most controller software to reverse the directions of X,Y,Z and A axis movements. I am using the defaults with my Xylotex controller board and EMC2. You will want to test your movement to make sure it is the same.
%
(required)(example gcode box)
G00 Z0.5 (raise bit above work)
G00 X0 Y0 (move bit to starting position)
G01 Z -0.5 F8 (lower bit = inch to allow milling)
G01 X1 Y0 F8 (move to top right corner)
G01 X1 Y1 F8 (move to bottom right corner)
G01 X0 Y1 F8 (move to bottom left corner)
% (required)
This simple example illustrates the how to mill a simple rectangle which has one inch side long sides. As you can see the programmer is responsible for keeping track of current location and walking around perimeter. This has only milled a rectangular line = inch deep. Milling a pocket would require decreasing the radius by a cutting increment and doing it over and over again until you meet in the center.
This seems to be an often confused issue with GCODE because there are custom GCODE editors available. GCODE is a simple text file that can be edited with any text editor such as Notepad which is built in to windows or Kwrite and VI which are built in to Linux.
The GCODE specific editors can make the task a little easier because they remember some of the syntax but I dont find them worth the hassle because they are neither as fast or as feature rich as free programming editors such as Anyedit at http://www.anyedit.org/
I seldom have to write GCODE directly because I use our Ruby library but when I do I use EditPlusfrom http://www.editplus.com/ because it is easy to produce a syntax file for EditPlus that show the GCODE in color.
It is a really good idea test gcode before risking your expensive cnc bits or material. It is very easy to miss single command that causes the bit to make a cut right where you do not want it. I currently use> Microtech CNC Simulator from http://www.cncsimulator.com/ but there are many available and are documented in our CNC overview document. and in the links portion of our CNC site.
The final test should always be ran with the head raised on the milling machine it self. This allows you to see exactly where the cuts will go before investing material and bits. Easy errors in GCODE can cause the machine to run up against its limits and try to run past the end of one or more axis so I keep my hand on the power switch to the controller so that if it looks like this will happen I can stop the movement. I can do the same thing with the abort command from the screen but by turning off the power seems to be easier to do in a hurry than positioning and clicking the mouse.
Comments in GCODE are inserted inside of (parenthesis) These can be on a line by them selfs or following a command on the line. They can actually be on the front of a line but we consider that bad style.
Comments can not be nested so do not use ( or ) inside a comment and where possible avoid the use of all punctuation because I have found bugs that cause some drivers to crash on some comments. Use comments judiciously because they do slow down the interpreter.
I generally use CNC util that allows me to write my scripts at a higher level and then it generates the GCODE so I add most of my comments to the ruby script rater than the GCODE
Be aware that if you specify a combination of moves that the interpreter will operate on all of them at once so for example if the head is currently located at X=0, Y=0, Z=0 and you specify in a single move to move to X=1, Y=1, Z=-1 then you will be drawing a diagonal line in three dimensions at a 45 degree angle in each one. This is fine if you are doing 3D profiling but if you really wanted to move the Y=1, X=1 and then plung then it has to be done in two separate commands.
Most moves are completed with the G01 op code. It can accept 1 or more dimensions and requires a speed wich is specified with F. Several of the combinations are shown below.
The range of F values is F0 to F20 but EMC seems to treat all values above F15 as the same. These can be decimal values. For milling Styrofoam with a 1 deep pass at = the bit radius F12 seems to produce good clean edges but F8 is better. I plunge at F5 in Styrofoam because F8 plunges sometimes caused cracks. In contrast most milling of aluminum will be done between F1 and F1.9 and stainless steel could be as low as F0.1.
The interpreter will complete one command before processing the next one. Moving multiple Axis in a single command will produce diagonal lines if the bit is in contact with the work piece. My favorite mistake is to move from one pocket to another and forget to retract the bit with it's own Z move before starting so I get a nice diagonal sloping up from one pocket to the next which isn't what I wanted at all.
The move as fast as possible Op code is G00. It takes the same parameters as G01 but without the F or speed settings. Some interpreters implement this as speed as the equivalent of F15 but others seem to be moving a lot faster. This is normally done used to either move the head home, retract the bit, Move to the start of a pocket. Anything you can do with a G00 command can also be done with a G01 command with a high F value. Here are some examples.
Raise milling headAssuming z = 0 is top of piece then inches will above work piece. This can be accomplished with g00 op code as shown. Change the Z value to one that reflects how you have your mill set up. % |
Lower or Plunge the milling headif you are at and then use the g01 command move to more shallow depth it is actually retract but the GCODE doesn't really care either way. We use the semantics of plunge and retract in our ruby library because it makes the code easier to read. % |
Milling Bit shape will affect plung ratesome milling bits are tips shaped to allow drilling straight down. Other bits can not do this and must have a whole pre-drilled. most machining books show a pictures of different bit configurations some of which can drill and some which can not. One of the cheapest and easiest bits to use when learning are the 1/16" bits made for RotoZip saws which can be purchased in packs of 4 from your local home improvement store. These bits work fine for both drilling and milling. I have not tried them in metal but they work great in wood and Styrofoam their only downside is that their small size requires more passes for pocketing which takes more time but our library automatically generates all the extra gcode so I use these about 80% of the time especially in soft materials where we can take deep cuts. |
Draw a Triangle % |
Draw a Hexagon
On this one I cheated by using our CNCUtil software to calculate the points for milling out the hexagon. It actually produced the all the gcode needed to mill out a hex cavity which is used to hold hex bolts but I only included the part to mill the first outline. Fundamentally what we do is we know that a hexagon will have 6 sizes and six corners and that ultimately they corners must turn 1/6th of a circle or 60 degrees so that they meet back at the beginning so the first thing we do is calculate the center of the hexagon and then calculate a XY coordinate for each of the 6 corners and then we can mill straight lines from corner to corner until we get back to where we started. CNCUTIL does all the calculations for us but the formula to calculate it relatively simple. % |
This one produces an Octagon % |
Mill Pentagon Outline
The only hard part of the polygon is calculating the end points. The way we do this with CNCUtil is to calculate the end point of each vertex using our Geometry functions which allow us to calculate a X,Y coordinate based on an angle of rotation around a point and then we can simply move the from point to point. The only tricky part is adjusting the angle the correct amount to reflect the number of sides. % |
Draw a Letter
Well it is an upside down letter the capital A. Obviously it would be difficult to hand code in a lot of letters and also support scaling but there are a couple of freeware utilities that will produce GCODE from TrueType fonts. There is a Vector Tracer available that I have not had a chance to try http://www.timeguy.com/cradek/truetype It claims to generate GCODE that you can use directly or with our CNCUtil CNC library % |
Drawing two arcs. g02 will go Clockwise The F parameter works to control speed
in the same way it does for G01 % Note: There are also I and J modifiers available for the arc command which change the center of the arc. I have not experimented with these enough to comment. When I am using the CNCUTIL library it hides all this complexity for me and it quite often calculates it's own arcs rather than using the G02 and G03 op codes. This allows us to produce arcs with changing diameters and makes it easier to mill out complex pockets but you can do a lot with the G02 and G03 opcodes |
CirclesThere are many ways to draw a circle but this is one of the easiest.
I have gotten G02 command to draw the entire circle with a single command buit I couldn't ever get it to perform reliably and the approach shown here works every time. % Note: You could use this to draw = of a circle or a pie segment just as easily The CNCUtil GCODE Library automatically does all the quadrant calculations for you so all you have to do is specify the finished dimensions. CNCUtil can also mill out a circular pocket or a circular pocket which contains an island in the middle all with simple diameter specifications. |
Stoping for clamp or bit changeSometimes it is necessary to drill one or more holes in a part and add bolts to help hold the part down. I find this necessary when the starting clamp positions would interfere with some milling that needs to be done and we needed the holes in the part for another reason so we run the first part of the program that mills the holes and then stops and asks the operator to add the bolts and remove the clams which are no longer needed. I like drilling holes in this fashion because they are always accurately placed and it pretty much guarantees that any elements milled after the part is bolted down with these holes will be accurately placed. M00 (please install | bolts in special hole | just milled and remove side clamps) Some interpreters will popup a dialog box containing the message in the comment section. The |is supposed to cause a linefeed in the displayed message. Other interpreters will pause with the line showing and the next line highlighted until you hit a key. Normally the key required is the space bar. NOTE: Once you add bolts to the internal of the part it is very important to make sure your milling bits do not intersect with these bolt because they are quite hard and can quickly destroy the bit during an impact. M06 is almost the same as M00 but it provides the state change for the new tool which will affect some other commands such as cutter offset commands. Stops with a prompts for change to tool 1 and changes to the tool 1 coordinate offset When using EMC2 The M06 command does not pause for manual bit change. It must Be combined with a M00 to cause the pause. I don't know if this is a bug in EMC2 or if I am using the wrong syntax. Note: When using this with the Micro CNC simulator it just logically changes the bit and but does not prompt even when using M01. |
How Pocketing Works
Pocketing is reasonably easy conceptually. You are simply removing all the material present inside a the outer dimensions of your shape. It gets complex only because of the sheer amount of work that must be done. Of cource CNCutil does the entire thing with one line but it still has to generate a fair amount of GCODE. There are a lot of different bit movement strategies but the one I like the best is starts in the center and spirals outward until it reaches the final dimension. all the internal cuts are taken at our roughing face cutting depth while the last pass will be taken at the more shallow and slower finish cut. The example below illustrates such a spiral. An additional complexity during pocketing is that if the pocket is very deep we have to cut it out in layers so if we where cutting in a harder material this pocket may have required several passes which would have generated that much more GCODE Mill a Hex Pocket% Note the extra plunges to -0.094 really don't do anything. I need to check the library because it is supposed to supress moves that don't actually generate a change. They don't hurt anything but I generates more code which is almost always something to avoid. |
Cutter Tool compensationSee This is a task that many people want to make quite complex but it is almost absurdly simple. Image you are milling out a square pocket that is 4 inches per side and you want it to measure exactly 4 inches across. I like to mill with a 1/2" diameter bit. I place the exact center of the bit on a line it will mill out one of it's diameter which is actually it radius of or 0.025 inches on each side of the center point. If I want a square to be exactly 4 inches wide and 4 inches tall then I have to move the milling head 1 bit radius to the inside to allow for the amount the bit will cut on both sides. Most of the CNCUtil pocketing and shape commands will automatically deduct the proper amount for the bit size you are using but when you resort to more primitive lines using direct GCODE You may have to accommodate this manually. So when using the = inch bit on a 4 inch square pocket rater than moving from 0,0 to 4,0 to 4,4 to 0,4 to 0,0 I have to move in one bit radius or 0.25 inches for each exterior coordinate. Or if I was milling an outside profile I would have to move out the same amount. The dimensions as adjusted are 0.25, 0.25 tov 0.25, 3.75 to 3.75, 3.75 to 0.25, 3.75 to 0.25, 0.25. Obviously adjusting for bit diameters is cumbersome and time consuming so all the CNCUtil pocketing commands automatically take them into account and make the adjustments automatically. The G40, G41 and G42 commands allow the Gcode interpreter to automatically adjust for the bit radius but you have to know when you are cutting left versus right to activate the proper sequence. I general I find it easier or more reliable to manually adjust the coordinates. The CNCUtil package does this automatically. |
Other GCODE training Links
|
