Hlep needed to comment G-code

[demonwolf]

Hi
Im doing a masters degree in computer aided mechanical engineering and one of my units is Computer aided manufacture in which i have to learn G-code. For one of the courseworks we have to write comments explaining G-code given to us.
Ive downloaded CNCSimulator and entered the code to understand more of whats going on still a bit unclear about a few things.

The first two parts of the program used canned cycles, which have some parameters i cant find information about.

N90 G81 G99 X10 Y10 Z-3.5 R2 F100
N100 G99 X10 Y70
N110 G99 X70
N120 G99 Y10
N130 G98 X40 Y40
N140 G40 G80
N150 G91 G28 X0 Y0 Z0
N160 M01
N170 T02 M06

my comments were that the drilling boring canned cycle was selected and the first hole drilled at X10 Y10 at a depth of Z-3.5 and with a feed rate of 100 mm/minute (as there are earlier G21 and G94 commands).

I dont undestand the point of the G99 command and dont know what the R2 command does. Can someone please explain.

Also I believe that three other holes are drilled with this canned cycle at X10 Y70 and X70 Y70 and X70 Y10, is this correct?
In CNC simulator it drills the initial hole at X10 Y10 but not at the three other positions.

[HuFlungDung]

Study the Haas Mill workbook, available in pdf format on their website. A lot of the information presented is generic sort of programming information.
http://www.haascnc.com/custserv_training.asp#mill

In general terms, the R2 is the Return plane, and represents the height where the tool makes a rapid move to before it begins the feedrate drilling motion. If this is a metric file, then R2 represents 2 mm of clearance of the tool tip above the surface.

Now prior to calling the G81 cycle, the tool is typically positioned much higher above the part, for safety reasons. Your sample program does not show us this value, but typically, it might be at Z25 mm.

G98 will cause the tool to retract to the Z start position when the cycle was called. So the tool will go safely up to Z25 between each hole. The tool might then safely clear any clamp or bolt that is less than 25mm high on this operation.

G99 will cause the tool to retract only to the R plane, which would be only 2mm clearance between positioning moves. This is fine for drilling many holes in a large flat area with no concern for the tool running into obstructions.

And finally, yes the program would drill a total of 5 holes before the cycle is cancelled with the G80.

[demonwolf]

Five holes are drilled?
Then that means that another hole is drilled at X40 Y40? but after that hole is drilled it (or before?) the tool retracts back to the specified R value in this case 2mm above the surface.

Thanks for the help and the link to the workbook, im going through it and the examples and comments are invaluable.

[HuFlungDung]

Sorry, I did a typo up there with G99 and G98 backwards. It is fixed now.

Yes, the intermediate holes get drilled with G98 (minimum R plane return height), and the last one turns on return to the initial plane at whatever height the tool began at when drilling is completed