Flip cards are pretty graphic...When i first got my FP4NC it had German cards and i was able to get the idea just looking critically at the graphics....
What you really need is the operators manual for your machine /control....gives lots of programming examples, easy to follow for each of the commands....invaluable.
Not up to speed as to the exact differences but a Contour3 is roughly equivalent to a Dialog4 control as to programming.
Some general notes:
Dialog must have a speed code (S+/S-) programmed in order to allow any feed moves (G01/G02)
Any called linear move (target point) is assumed by the control to be a feed move, you do not need to have a G01 or G02 programmed in the move code. But you must have previously
programmed a feed rate ...
Once a feed rate is programmed it will stay in effect till it is overridden with a different feed rate or a rapid move....Must then recall a feed rate to continue with an linear move....
If you are doing a drawing using a pen in the spindle and don't wish it to be rotating while running the program "proof" you can use speed code S+0...Control believes the spindle is in motion so the
program will run, but the spindle will not rotate.
Rapid moves must be called every time they are needed (in every block where desired)
Canned cycles almost include a call fro feed rate within the cycle....
Canned cycles with depth moves use incremental (G91) valuers for all depths within that cycle...even if you are programming in absolute (G90).
Cutter comp has more "rules" that have to be followed in order for it to function...
Establish a routine as to how to start every program ! This will simplify the program writing and eliminate errors...
As example, i always start every program by moving rapid to the tool change point...Somewhere off the part surface and at the datum (zero point) of the program...
I also set the direction for length comp right off. as well as the spindle speed...
Example in inches:
N1 G0 X0.0 Y0.0 Z4.0
N2 G17 T1
N3 S+1000
N4 G0 X1.0 Y2.4 Z.1.
.................................................
Block 1 sets the tool change point and moves there.
Block 2 calls the length comp for a vertical tool and defines the first tool (T1) Must have a tool 1 defined in the tool store (mode 10)
Block 3 starts the spindle at 1000 RPM rotating to the right (forward)
Block 4 moves the tool at rapid to a clearance height off the part and at the start point of the cut....Note trailing zeros (to the right of the decimal point) are not needed....But i always write them in my
paper copy (Manuscript) as i am creating the program....
Cheers Ross