Help for CopyCat Router Wizard

<title> Help for CopyCat</title>
<h1>Help for CopyCat Router Wizard</h1>
This wizard will allow you to jog a machine around and create a Gcode file from the movement.
This would be usefull for copying an existing part instead of measuring and drawing it.
<p>
This wizard always writes to the same file, C:\Mach3\GCode\teach.tap This allows you to add
to an existing file. If you want to start a new file be sure to click the 'NewTeach File'
button. 
<p>
Inside the wizard you are free to move the machine around with the normal jog commands,
as well as by entering commands into an MDI box. Your movements are only saved
and made part of the G code file when you press one of the action buttons.
<p>
There are several groups of action buttons.
<h2> Control functions</h2>
These simply add control statements, like spindle on or off, tool change, etc. Pressing the 
button will add that code into the Gcode file.
<p>
Note the button labeled 'Insert Comment' You may use it to add any comment into the Gcode. 
You might use a comment to indicate a point in the code where you want to insert another
block of code. For example, if you have a long line of holes to drill you might just enter
the first hole
and the last hole, with a comment in between, then use another wizard to generate all
the code for the holes between these points.
<h2>Movement Buttons</h2>
In general, you may move around the machine freely with any of the normal jog functions, then when you are at the desired point
you press a movement button when you are at a point you want in your program.
<h3>Radid Move</h3>
A rapid move will create a G00 code to the current point. X and Y values are used. Be cautious
if you rapid to a Zvalue below the surface of the part!
<h3>Feed Move</h3>
Create a G01 command to the current position. The current Feed rate will be used.
<h3>Zup Zdown</h3>
Generally while probing a part you will not want to make Z moves, as that would move your probe above
or below the part. When you have moved to an XY point and then want to either move the tool up or down
enter the appropriate button. Code will be entered into your tech file, but the Z axis will
not make an actual move.
<h3>Arc Move</h3>
An Arc, or a full circle move may be generated. To enter an arc you must first move to
a point that defines the start of the arc with either a Rapid or Feed move. Press "Start 
Arc' to remember this point. Next move to
a point on the arc, and press "2nd Point". Finally move to the end of the arc and press "end Arc".
If the 'Full Circle' button has been pressed, and its LED is on, then a full circle will be generated.
Otherwise an arc from the start to end points is generated. 
<p>
You may cancel the Arc entry before completing it with the Cancel button. This resets all the
entrys and does not add any Gcode to the file.
<p>
For best results place the 3 points around the Arc about equally. 
<h3>Holes</h3>
Move to the center of any hole and select a Rapid or Feed move. Note that this move should
be above the work at a safe height. Then select the kind of hole.
<p>
<b>Hole</b> will mill a hole by making a circular cut.
The tool will spiral down to the requested depth, then make a full circle at that depth to
fully clear the hole. Be sure you are using a cutter that can be 
plunged! 
<p>
<b>Drill Hole G81</b> will make a plunge drill operation to the selected depth.
<p>
<b>Peck Drill G83</b> will make a peck drill cycle to the selected depth in steps of Zinc.
<H2>Probe Screen</h2>
A second screen has probe functions. The left side of the screen uses a tool probe and the G31
command to actually probe the edge of a part or to find the center of a circle. 
<p>
Generally, when you have found the edge or center, you will want to raise the probe tip above the work, then 
click the 'GoTo Probed Value' button. You may then return to the main screen and select a move button.
<p>
The right side of the screen finds the center of a circle by the 3 point method. Thanks to
German Bravo for his original circle center wizard, which was used in the screen. Note you may
use the 3 point method, but find the poits with the probe functions.
<h2>Probes</h2>
In the simplest case you may probe your part with just a pointer- a tothpick can work, and doesnt hurt when
you break it! Simplly jog around the part looking for the important points, and enter them into movement
commads as needed. You might consider a simple round rod as a probe, of the same diameter as you intend to cut the
finished part. This will automatically build in the needed tool offset.
<p>
A video probe is useful if you have one, simply open the video window and elect your points. 
Note you might want to turn on the tool circle and use it to build a program that offsets for tool diameter.