Re: [CAD_CAM_EDM_DRO] Cncpro/Gcode

Taus:

I have been using CncPro for some time now on commercial/industrial machine
retro fits and have not experienced the lack of support at all. Doug has
always been quick to respond unless for some reason he is out of the country.
Now as far as the upgrades go, just go to the "price" site on
www.yeagerautomation.com and download the upgrades or "patches" this will
bring you up to date on the .exe files.

Before getting into the questions, I assume you are VERY new to CNC as the
instruction set he uses is quite common and matches the FANUC set very
closely, by the way the FANUC is the leading CNC controller in the world.
You might want to get some books etc. on CNC just to get an idea of the
basics.

1. F5 - F8 (I/O 1 - I/O 4) are for user input output "M" codes. Also you
can use the "F" keys 5 - 8 to turn these outputs on or off by simply toggling
the "F" keys. These would be used for things like turning on a spindle
motor, activating solenoid valves, etc.

2. V variables are just what they say, variables you can use them as follows:
V1=2.500
V2=3.000
V3=5.000
G1 G91 XV1 YV2 ZV3 F100
By doing this you can assign up to around 100 different variables and when
you have a shape that is the same you can just change the appropriate
variable without having to re-write the whole program

3. The Looping instruction could be considered a "jump" in a way. You can
run a section of your program over and over by "looping" that section.

4. E-Stop does mean EMERGENCY STOP, you can define the input for this as
either a true emergency stop or as a line hold which will simply stop the
program at the line where the program is at when the input for the E-stop is
seen and then you just have to press the appropriate key to continue from
that point

5. Subroutines are a HUGE help as you can write a subroutine for a particular
contour and then just call it up with a one line command to run it over and
over at different locations on the "table". This makes it necessary to write
the code for that contour only once. Let's say you want to make the same
oval shape over and over on a piece of material, say 30 times, all in
different locations. You can write ONE contour subroutine for the oval and
then simply call it up to run after re-positioning the cutter to the correct
starting point instead of writing the code for the oval 30 times. This saves
programming time and programming space/memory.

6. Length compensation is used when you are running a part that requires more
than one tool to make the part. You have a reference point and you know the
difference in the "Z" axis between the reference and the other tools. You
simply put this value into the tool table for those tools and call up the G43
command with the Tool's compensation number and the program automatically
makes the proper "Z" axis adjustment without the necessity of programming
separate "Z" values for each tool.

7. Machine offset co-ordinates G54, G55, etc. are used when you want to have
a new "0" to start from. Let's say that you have enough space on your
"table" to make 4 of a certain part(s), you can put the G54 command at the
beginning of the first program line and the machine will operate as if "0" is
actually located at the offset point you have entered into the offset table.

8. I usually keep the constant contouring turned off until I actually begin
the cutting of the part and then turn it off when I am ready to raise the
cutter out of the material, or turn it on after you have called for the tool
compensation then turn it off before you cancel the tool compensation. I
don't have it turned on at the start of the main program.

I hope this helps you some, if you have any additional questions please
E-mail be directly at cnc002@...

Randy A.