G-Wizard Editor: Setup Options

The GWE Setup Tool is accessed from the button on the far right, or from the Tools Setup menu choice. It contains a variety of sub-tools accessed by a tab bar along the top:

If you do nothing else with the Setup application, be sure to get your Imperial/Metric Units set, a Machine Profile Configured, and download a pre-defined CNC Controller using the "Browse" button next to the CNC Controller field on the Machine Profile. The rest is fine tuning.

We'll go into a little more depth on each one that's specific or different in GWE below. For Basics, Tool Crib, and Files, refer to G-Wizard Calculator Setup.

From a g-code perspective, be aware that the default for GWE is Mach3, which is very close to Fanuc in most ways. You will want to go through the various settings and change them to match the way your controller operates.

The Basics tab is all about setting the units, as well as selecting and defining machine profiles. Let's talk units first. When you change the units, it changes the units for the controls in the editor and it changes the grid but it does not change how the simulator interprets coordinate values in g-code. To change the coordinate value units, use G20 (inches) or G21 (mm). You can either use these in your program, or you can use them in the Setup G-Code under the post tab. So, for example, if your CNC comes up by default expecting mm, put a G21 in your startup g-code.

Always remember, G20 and G21 don't do unit conversion, they merely change how the numbers are interpreted. With G20, X0Y1 refers to X = 0 inches and Y = 1 inch. After a G21, X0Y1 refers to X = 0 mm and Y = 1 mm.

When we say it changes the units for the controls in the editor, that means it changes the units for the XYZ coordinate display down on the status bar, for the Info tab, for the Simulator information that appears below the backplot, and so on.

You can download a pre-defined CNC Controller configuration from CNCCookbook to save the effort of defining all the Post parameters. If you press "Browse" next to the CNCController field, you will see the following popup:

The Variables tab lets you access the internal variables of your simulated CNC machine. These are variables accessible via programs using a "#" and a number and are primarily of interest to programmers writing macros (sometimes called "Parameterized Programming"). But even if you're not writing macros, you may need to access them to set up your work offsets or other offsets so that your g-code program will run properly.

As you can see, the Variables Tab consists of a scrolling list of all the variables together with a set of controls at the top to help you quickly find the variable you're looking for. If you know its number, you can type that into the "Scroll to #" box and get there immediately. If you only know the general category of the variable, you can filter the list using the following buttons:

Note: At the moment, the Variables Tab doesn't affect program execution at all and GWE doesn't yet understand macros!

The Post Tab is where we really get into the guts of what makes each CNC Controller different. It's called the "Post" tab because its modelled on the "Post-Processor" concept common to CAM programs. They have to be able to cope with controller differences too. Here is the Post Tab:

This is a one-line g-code program that is run to allow you to customize the simulator's initial state.

You may modify these as needed to initialize for your controller's initial state. Before the one line startup g-code is executed, the initial state is equivalent to the following:

You should only execute codes that change these defaults as it would be redundant to reinstitute them (for example by putting an "M9" in the startup g-code). These codes will not appear on the backplot, but they will show up as currently active options in the simulator.

A typical use of the Startup G-Code would be to specify a G18 for a lathe. Many lathe controllers select G18 by default at startup.

These are the options for how I, J, and K are interpreted for G02/03 arcs. Some controllers see these as incremental values, meaning they are relative to the current position. Some see them as absolute values. If you check the box, GWE expects incremental values. Uncheck it for absolute.

If you load a g-code file and see lots of crazy circles that are not what you expect in the backplot, you likely need to change the status of this box to match what your controller expects.

The exact syntax for G51 as well as its capabilities differ from controller to controller. GWE supports 3 styles:

There are lots of differences from one machine to the next in how canned cycles work. GWE offers two options you can change:

This option controls which of the #-Variables are saved to disc when you exit GWE. Two styles are available:

There are a lot of different syntaxes for an M98 subprogram call. Check your controller to see how yours works.

Note: At the moment, GWE doesn't handle M98 at all and most of these options are not implemented.

The Numbers tab under Post is used to set the options for how the numbers found throughout a g-code program are to be interpreted. Each g-code word is a letter such as "G", "M", "F", or "S". Associated with each letter or group of letters is a set of options that determine what kinds of numbers can go with the letter.

To use the Numbers tab, first select the letter you want to customize. Here are your choices:

After selecting the desired letter, the Numbers will show the options associated with numbers for that letter in the left column and some examples on the right.

Option	Purpose
"+" Required	Determines whether a "+" sign is required for positive numbers. Some controllers require one.
"-" Allowed	Determines whether the number can be negative. If so, it requires you to designate negative numbers with the minus sign.
Left of decimal "up to" checkbox	If the "up to" box is checked, it means the number of digits can be any number up to the specified number. If it is not checked, the number of digits must be equal to the number specified, with leading or trailing zeros required to make up any shortfall.
Left of decimal digits	The number of digits left of the decimal point. The whole number part.
Decimal mode
Right of decimal "up to" checkbox	If the "up to" box is checked, it means the number of digits can be any number up to the specified number. If it is not checked, the number of digits must be equal to the number specified, with leading or trailing zeros required to make up any shortfall.
Right of decimal digits	The number of digits right of the decimal point. The fractional number part.
Divisor	After the number has been captured, but before it is used by the controller, it is internally divided by this value.

In the righthand column are some tools designed to help you understand what the options you set are doing. You can enter samples into the "Try" box and see what G-Wizard thinks the value of the number is and whether it has any errors.

Below the "Try" box are a series of examples that show what will happen in various cases.

"Pattern" is a shorthand way of writing out the options that is used by a great many CAM programs as well as by utilities for postprocessing such as Posthaste. If you know the pattern of your number, being able ot see what pattern G-Wizard thinks you have set up should help you to match the two up.

When you've got the options the way you want them, press the "Save" button below. Note that each letter must be individually saved. You can also reset the options to the default letter by letter, or at the top is a button labelled "Reset All Letters" that will go through and change all of them to the original G-Wizard defaults.

Note that there is also a default format, which is chosen at the top right of the screen. When no format is defined for a particular address (letter), the format associated with the default is used.

The purpose of the G/M-Codes tab is to let you tell GWE which g-codes your controller actually implements. You can turn each one on or off in the "Enabled" column. If you turn off a g-code, GWE will do two things. First, it will ignore the code during program execution. Second, it will attach an error to that line to remind you the code is not allowed.