This morning, while I was cutting out a sign on my home-built CNC machine when the shop teacher hit the E-Stop switch on a pillar in the woodworking shop at the program for mentally handicapped people for a fire drill. Hitting the E-Stop switch switch caused my computer and my CNC machine to lose power. How do I resume cutting the sign without having to manually jog the spindle to the home position and starting again?

If you had the offsets for you part saved then you can simply start up the machine and reference it, then load your code and click in the code window anduse the arrow keys to scroll down to where your code was interupted. You then choose the Run From Here button and a prep move box will appear asking if its safe to move to that position, if it is then press Start, once the position has been reached you press start again and it should continue with the code.
 If your ofset wasnt saved then you will need to relocate your zero positions and then do the run from here as detailed above.
Hood

Before loading G-Code into Mach3 program, I zero all axises and click on "Ref All Home" button. I repeat to make sure that the DRO display "0" on all axises. If the machine is interrupted, how do I get the machine to move all axises to "0"? I tried "Goto Z" button but I thought that it didn't work. The machine doesn't have limit and home switches.

Without home switches the only way for you to get back is to move manually to where you started your work, edge finder may help locate but that will depend on the workpiece and how accurately you set it up in the first instance
Hood

I move the axises close to home position, press the "TAB" key to call up the jogging control window, set the jogging mode to single step, enter the values shown on the DRO in the "Cycle Jog Step" textbox, and press the arrow keys to move the axises exactly to home position. For example if the "X" axis position on the DRO is "0.1256", I enter "0.1256" in the textbox and I press the left arrow key once to move the "X" axis to "0". I will try installing home switches on my machine but what about the "Z" axis? Should the home switch be installed so that it is hit when the "Z" axis carriage is moved almost all the way to the top?

Yes usually the Z axis is set to home when it is at the furthest distance away from your work. This means 0 is you Z Max and your Z min is always a negative number, this is when in machine coordinates and you can then of course have positive and negative Z values when you have a work offset.
Hood

I installed the home switches with the Z-Axis home switch at the top. After moving the axises to home position, how do I have the Z-Axis move to 3/4" off the table of my CNC router? I tried to use the Part Offset feature but I found out that the router carriage will hit the machine frame. If a piece of wood is 24 inches long and the working area of my CNC router is 20 inches long by 17 inches wide, how do I put the piece of wood in the machine so that one end is two inches to the left of the home position and have the router carriage move to correct position as if the piece of wood is 20 inches long? I designed a sign in Cut2D program and the piece of wood is 24 inches long and the letters to be routed are about 20 inches long.

Not really sure I understand your question but here go's
 Your home position or Reference position is what Mach uses to know where it is. When you load a part it is normal to jog your axis where you want the workpiece zero position to be, when you get there you zero each axis with the zero buttons beside them. That is now your work offset zero position.
 If you have a piece that is longer than your travel and the code has the zero position that is at the corner of your workpiece you can offset the axis by entering the position in the DRO that would correspond to your work. Not really easy to put in words what I am meaning and as it may not be what you are wanting I wont strain the brain trying to make it clearer, if it is what you are meaning then let me know and I will try and make it clearer

Hood

The "Offsets" screen confuses me. If I enter a value other than "0" in the DRO and regenerate the toolpath, the purple cursor moves to the value that's entered in the DRO but doesn't change the "home" position (the red lines starting at the "home" position). For example, I entered "-2" in the "X-Axis" DRO but if I run my CNC router in simulation mode, the purple cursor moves to the left, the router carriage will hit the left side of the router frame. I didn't want to actually run my machine because the stepper motors will make a lot of noise.

Jeff - You may kow a lot of this - but here goes -

Your machine needs to know where it is. The professional way it to have switches fitted on the machine, then you just say to the machine "Ref all home" and it does. It sets all the DRO,s to zero. This position is 0,0,0 in machine co-ordinates and shows on the DROs when the Machine Co-ordinates button is pressed and the button is illuminated. You can only zero machine co-ordinates by using the "Ref all Home button". The button zero,s any DRO that does not have a home switch designated, and it moves any other axis to the switch, and then zero'0 the DRO if it does have a home switch.

This position could be anywhere, and is probably not a convenient poisition from which to start machining, and will probably not be the start position from which your GCode position was written. We will assume that position is in the centre of the table, and you have fitted some studs, poking up from the table, onto which you put your workpiece. (All the other workpieces you are going to machine also have stud holes and will fit in the same position)

The GCode is written to start at the bottom left hand corner of the workpiece - which the program knows as 0,0 (X and Y). Z0 is the top of the workpiece.

To reconcile the two is the job of the "offsets"

You start with your machine and "Ref all Home". This sets the Machine Co-ordinates to 0.0.0. and the machine knows where it is.(If you have limit switches - and your Z is homed to the top of it's run) You then jog your machine to the start position for your work. At this stage note the readings on the DROs. Press the Machine co-ordinates button and the button surround will go out. The DRO,s will not change BUT they are now showing "work co-ordinates or program co-ordinates" and can now be zeroed. If you zero them, they will change to 0,0,0  - in line with your program.

You can now start the machine and away you go. - What have I achieved you ask - well you have the "offsets" which you noted.

You can enter the offsets in the offset table - I don't bother with the offsets page - I put them straight in the table. Offsets are numbered G54 to G59 - and G59 has 255 sub groups so there are plenty. We will assume that you enter the offsets for this program in G56.

When the man presses the Fire Alarm you say "Up your's" and walk out. When you come back you press the button for Machine Co-ordinates and  " Ref all Home" - the machine knows where it is (quite important because E stop sometimes causes missed steps).You then enter the "offset" on the MDI (G56) and switch to program co-ordinates. Tell the machine to go to G0 X0Y0Z0 and the machine will move back to the position that you started machining. Start the program and away you go.

The offsets can be made fully automatic, in that they can be entered in the program. The program can "Ref all Home" and then enter the offsets. You can, at the end of the program, change to "Absolute Co-ordinates" (another name for Machine Co-ordinates) and move your tool out of the way of your work. If you change your workpiece by mounting it on the studs I talked about, then start the program again, the machine will reference itself, move to the work, cut it, and then return, ready for the next one.

To clear up any more problems, have a look at the tutorial on Co-ordinates, which deals with the subject step by step.

The toolpath display on Mach 3 is very good and I find it a great help when writing programs. It does respond to the "program" entered in the GCode - i.e. it takes its 0,0,0 position from that. What you must be careful of, however is the position of your Machine/Program co-ordinates button - and if you press this, then also regenerate the toolpath. There are some errors in the display, however, particularly when dealing with osffsets and sub-programs, so don't take it as gospel.