[matridium]

I have a question about drilling.

I want to create a drilling cycle that will allow me to peck drill and dwell at the same time..
The process I want is to move the bit to the x, y location, drill the material for a depth of 0.005”, dwell for 2 seconds, retract from the hole, dwell for 2 seconds, drop back in to the hole and drill for another 0.005” then dwell for 2 seconds and so on and so on until the hole is done and than the bit is moved to the ne location. I know how to do peck drilling (g83) but how do you dwell during a g83? I am drilling with a #75 drill bit, into lexan .250” deep, through hole. Any help would be great

Regards
Mike

[jsantos]

Pxxx where xxx is in milliseconds.

[matridium]

so would this work?

G81 X0.3870 Y0.0250 Z-0.005 R0.0500 F0.10 P2000
G81 X0.3870 Y0.0250 Z-0.010 R0.0500 F0.10 P2000
G81 X0.3870 Y0.0250 Z-0.015 R0.0500 F0.10 P2000

[jsantos]

so would this work?

G81 X0.3870 Y0.0250 Z-0.005 R0.0500 F0.10 P2000
G81 X0.3870 Y0.0250 Z-0.010 R0.0500 F0.10 P2000
G81 X0.3870 Y0.0250 Z-0.015 R0.0500 F0.10 P2000

Just looked up the fixed cycles. G81 does not have a P. G82, however, does. You'll also need a G99.

Here's the G82 description;
1. Rapid motion to XY position.
2. Rapid motion to R-level
3. Feedrate motion to Z-depth
4. Dwell at the depth - in milliseconds (P)
5. Rapid retract to R-level (with G99) or rapid retract to initial level (with G98).

[DareBee]

You wont get a dwell at the retract plane. I don't know of any canned cycle that will. You could use G82 and 25% rapid overide to give it more out-of-material time.

How about making a really repetitive sub-program

[guru]

I agreed with DareBee, regular drill cycle won't give you a dwell at retract plane, but if you mast have it just write a Drilling macro

[matridium]

exactly waht is a sub program? and how do you write one?

What about this...

G82 X0.3870 Y0.0250 Z-0.005 R0.0500 F0.10 P2000
G99 X0.3870 Y0.0250 R0.0500
G04 P2000
G82 X0.3870 Y0.0250 Z-0.010 R0.0500 F0.10 P2000
G99 X0.3870 Y0.0250 R0.0500
G04 P2000
G82 X0.3870 Y0.0250 Z-0.015 R0.0500 F0.10 P2000
G99 X0.3870 Y0.0250 R0.0500
G04 P2000
G00 X0.9090 Y0.0250 Z0.0500

I can't see this not working? but what do you guys think?

Regards
Mike

[DareBee]

Close but not quite.
Your code would be for drill only (no X/Y) because you want to use it for every hole.

I would do a subroutine like this
Note - the control sees the M17 and won't start running the code until the first M30 thereafter.

%
L200 (subroutine)
G90
G82 G98 Z-0.005 R0.0500 F0.10 P2000
G04 P2000
G82 G98 Z-0.010 R0.0500 F0.10 P2000
G04 P2000
G82 G98 Z-0.015 R0.0500 F0.10 P2000
G04 P2000
etc.etc.etc.
G00 Z0.0500
M17
M30
G00 G40 G49 G80 G90 G17 G70 (MAIN PROGRAM)
T12 M6 (Center Drill)
G58 S2200. M3 M8
X0.3870 Y0.0250
L201 (run sub 200 - 1 time)
X?? Y?? (next hole)
L201
X?? Y?? (last hole)
G80
M05 M09
G91 G28 Z0.0
G00 G90 E0 X5.0 Y9.5 A0.0
M19
M30
%