Drilling advice

[Columbo™]

Material 15-5 heat treated to H1025 (Rc34-42)

 

I need to come out to the .550/.552 diameter bore during peck drilling the .187 and .156 holes to clear chips, then rapid back in. Is there a way for Mastercam to do this?? I do NOT want to start pecking at the start of the .550/.552 hole as it would cut air. {see attached file}

 

Custom drill cycle maybe....never used them....How is it done???

[DODGERFAN]

the peck will start from the defined material. If you wanted to start from the .400 depth use that as the top of stock in the linking perameters. Hope this helps

[K2csq7]

Assuming Datum "D" is your Z zero, set your top of stock to -.400 and your retract to .1 incremental or -.3 absolute

[DODGERFAN]

Assuming Datum "D" is your Z zero, set your top of stock to -.400 and your retract to .1 incremental or -.3 absolute

+1000 Keith

[Columbo™]

I need to start the .156 drill in the .188 hole, peck .05 retract out to the .550 bore, rapid to .05 from last peck drill another .05 retract out to the .550, rapid back in etc.

 

NOT starting the .156 peck in the .550 bore.

[DODGERFAN]

if datum "D" is z origin the your top of stock value will be -1.230.

[Joe788]

Columbo, this will need a custom drill cycle.....or a Haas machine. I'm pretty sure Haas is the only major builder with a standard canned cycle to do what you want.

[Dave.L]

Henry, FWIW If you get the right tooling (and it should not be an issue), you can do the Cbore then the .156 without an issue. I assume your plan of attack (based on your question) is to do process large to small but I don't see the need to do this if you have the right tools.

[Columbo™]

Dave,

 

Yes that is the plan of attack.

 

That is standard here for small deep holes. In another area of this part I am working on the holes are deeper than 3.5". We have had issues here where the drill hit chips during the peck and broke.

 

There is a sub program in some of our machines that need three points to drill this way. (BUT needs to be entered MANUALLY into the program) 1st is the retract, 2nd is the clearance above the hole to be drilled and 3rd is the final drill depth. Also need a peck, feedrate and return clearance

 

This is what we use now on an OSP control. (have to add to program manually)

 

 

N1090 T18M06 (LONG .157 TWISTDRILL)

N1100M00(MAKE SURE DRILL IS NOT BOUNCING )

N1110 G15H05G90G00X-3.2Y4.05S1500M03B90.T43

N1120 G56Z8.H18M08 (.180 DIA. SPOT FOR DRILL)

N1130 Z2.43

N1140VC40=-1.895 (FINISH Z)

N1150VC41=2.43 (CLEARANCE PLANE/OUTSIDE THE PART)

N1160VC42=.05 (PECK/Q/POSITIVE VALUE)

N1170VC43=1.68 (START POINT/R)

N1180VC44=.025 (PECK RETURN CLEARANCE/POSITIVE VALUE)

N1190VC45=3.6 (FEED)

N1200CALL O0831

N1210 G00Z8.M09

N1220 M05

N1230 G30P1

N1240 M00

 

O0831

N10 (1ST PASS)

G00G90Z=VC41 (Z RAPID TO OUTSIDE R)

G01Z=VC43 F30.(FAST FEED TO INSIDE R)

VC46=VC43-VC42 (R-Q/CALCULATE 1ST DEPTH)

G01Z=VC46 F=VC45 (DRILL 1ST PECK)

G00Z=VC41 (Z RAPID TO OUTSIDE R)

N20 (OTHER THAN 1ST PASS)

VC43=VC46+VC44 (LAST DEPTH + CLEAR./NEW INSIDE R)

VC46=VC46-VC42 (NEW Z)

IF[VC46 LE VC40]N30 (NEW CAL. Z LESS THAN FIN Z, GO TO LAST PASS)

G00Z=VC43 (Z RAPID TO NEW INSIDE R)

G01Z=VC46 F=VC45 ( DRILL)

G00Z=VC41 (Z RAPID TO OUTSIDE R)

GOTO N20

N30 (FINAL PASS)

G00Z=VC43 (Z RAPID TO NEW INSIDE R)

G01Z=VC40 F=VC45 (FINAL Z DEPTH)

G00Z=VC41 (Z RAPID TO OUTSIDE R)

RTS

 

 

we also have something similar for fanuc controls.

 

AGAIN......has to be typed into the program manually......can something like this be posted???

[CJep]

Columbo,

 

The Haas uses something similar in a canned drill cycle, but get Mcam to output in the format you're looking for would require a custom drill cycle post block.

 

G83 DEEP HOLE PECK DRILL CANNED CYCLE

X* Rapid X-axis location

Y* Rapid Y-axis location

Z Z-depth (feed to Z-depth starting from R plane)

Q* Pecking equal incremental depth amount (if I, J and K are not used)

I* Size of first peck depth (if Q is not used)

J* Amount reducing each peck after first peck depth (if Q is not used)

K* Minimum peck depth (if Q is not used)

P Dwell time at Z-depth

R R-plane (rapid point to start feeding)

F Feed rate in inches (mm) per minute

[Leigh @ Kodiak]

....can something like this be posted???

 

As far as I know, the only way to accomplish this is with a custom drill cycle. You could use a point to point path, but if you do this sort of thing with any regularity, the custom drill cycle is the only way to go.

[John @ High Tech Machine]

If you have the custom cycle already written for the machine(what control?) as a subprogram, couldn't you modify it to have the values as variables and have it called as a macro (if you have the capability in the control)? Then modify your post to include that macro as a custom drill cycle with your required variables as data filled in like with any other drill cycle type.

[MIL-TFP-41]

This can be easily done with a standard peck cycle.....you just have to turn off "used canned cycles" in your control definition. The output is longhand...something like this...

 

G0 G17 G90 G54 X0. Y0. S2515 M03
G43 H1 Z.1 M8
Z-.35
G1 Z-.75 F4.
G0 Z-.35
Z-.74
G1 Z-.8
G0 Z-.35
Z-.79
G1 Z-.85
G0 Z-.35
Z-.84
G1 Z-.9
G0 Z-.35
Z-.89
G1 Z-.95
G0 Z-.35
ect

[darko herak]

Material 15-5 heat treated to H1025 (Rc34-42)

 

I need to come out to the .550/.552 diameter bore during peck drilling the .187 and .156 holes to clear chips, then rapid back in. Is there a way for Mastercam to do this?? I do NOT want to start pecking at the start of the .550/.552 hole as it would cut air. {see attached file}

 

Custom drill cycle maybe....never used them....How is it done???

 

you should use some of comon drill cycles, but adjust clerance to eg. .3, and retract to eg. .-0.3 , top of stock is probably 0, and depht is what is on you blueprint, should be careful, the tab clerance must be active and z+, in case of multiple holes