Sign in to follow this  
ton

Drill + Peck cycle combo?

Recommended Posts

Hello everyone,

I run an older Fanuc15m.

We have a spade drill bits that does not like to drill deeper then its shoulder depth without burning out the sides of the inserts.

We currently are pecking with G73 Q_ R.3 Z_ F_ which is very time consuming.

Is there a specific cycle that allows for a drilling cycle to dill to any specified shoulder depth and then start the pecking to the desired depth cut?

For example:

G_ _ D-.48 (drill value for shoulder Z-depth) Q.05(peck value for the remaining Z-depth) R.1 Z-1.2 F5.

 

 

Thanks for your time and input!

Share this post


Link to post
Share on other sites

Thankyou!

 

I was looking for more of a custom drill cycle?. Where I can input any desired shoulder depth and have a custom cycle figure it out the remaining z depth to peck.

Share this post


Link to post
Share on other sites
3 hours ago, ton said:

Thankyou!

 

I was looking for more of a custom drill cycle?. Where I can input any desired shoulder depth and have a custom cycle figure it out the remaining z depth to peck.

You would have to have the custom cycle implemented on your machine somehow. What G-Code are you going to run?

This may be possible by using a Subroutine with two Drill Cycles in a row.

%

O5001

G00 Z0.1

G99 G81 Z-0.64 R.1 F20.

G99 G83 Z-1.1 R-0.6 Q.1

G80

M99

%

 

Otherwise, you'll need to use something like Advanced Drill. 

Share this post


Link to post
Share on other sites

That may just work! Thankyou I'll try it out...

Thanks a bunch!!!

Share this post


Link to post
Share on other sites
3 hours ago, ton said:

That may just work! Thankyou I'll try it out...

Thanks a bunch!!!

*Be careful about using G98 versus G99. If you use G99, it *should* return to the Initial Point, after finishing the G83 Peck Drill.

G81, with those parameters, starts at Z0.1, then drills to Z-.64, then returns to Z.1

G83 starts at the Initial Point (Z.1), should rapid to the R Plane (Z-.6), then peck from there. (Note: It won't rapid out of the hole, due to the R plane, so it is kind of more like a chip-break cycle. When the cycle finishes, the G99 tells it to return to the Initial Point. It wouldn't hurt to make this little modification:

%

O5001

G00 Z0.1

G99 G81 Z-0.64 R.1 F20.

G99 G83 Z-1.1 R-0.6 Q.1

Z0.1 G80

M99

%

Share this post


Link to post
Share on other sites

Yes thanks I'm aware of G98(clearence) and G99(R plane). I was busy at work and haven't yet had a chance to perform the subroutine.

I do not want the cycle to rapid back up to R.1 I would like G83 to continue where G81 ended off at Z-0.64 can I throw in a incremental and then a G98 in the end?

 

%

O5001

G00 Z0.1

G99 G81 Z-0.64 R.1 F20.

G91 G83 Z-1.1 R-0.6 Q.1

G90

G98

Z0.1 G80

M99 

%

Share this post


Link to post
Share on other sites

G81 cycle will always go back to R or Z plane then G83 will always start from here. This is part of the cycle process and there is nothing you can do about this. Or use 'advanced drill' command for a fully customized cycle.

  • Like 1

Share this post


Link to post
Share on other sites

Here's a Reducing peck cycle...

Designed for a 16 control. So with some mods, you could adapt it for a 15. In the last 15 years I've only put my hands on a 15 Control 1x.... so it's been a while.

HTH

%
O9004(REDUCING PECK MACRO)
(THIS PROGRAM IS DESIGNED TO RUN FROM A PRE-DRILLED HOLE)
(USED FOR A DEEP HOLE WHERE TWO DIFFERENT DRILL LENGTHS ARE NEEDED)
(USED WITH G184 CUSTOM MACRO CANNED CYCLE)
(EX. G184Z-9.65R.01F6.I.3J.5Q.1E-6.3)
(#18 "R" RAPID PLANE)
(#4 "I" 1ST PECK)
(#17 "Q" MINIMUM PECK)
(#26 "Z" FINAL DEPTH)
(#5 "J" REDUCTION MULTIPLIER)
(#9 "F" FEEDRATE)
(#3 "C" PECK RETRACT COUNT)
(#100 INITIAL PLANE STORAGE)
(#101 REMAINING DISTANCE CHECK)
(#102 "Z" TARGET VALUE)
(#103 "Z" FEED/RAPID VALUE)
(#8 "E" SUB RAPID PLANE)
#10=#4
(ERROR CHECKS)
IF[#3EQ#0]GOTO5
#3=FIX[#3]
GOTO6
N5#3=1
N6IF[#26EQ#0]GOTO50
IF[#18EQ#0]GOTO51
IF[#9EQ#0]GOTO52
IF[#4EQ#0]GOTO53
IF[#18LT#26]GOTO54
IF[#5NE#0]GOTO7
#5=1
N7IF[#5GT1]GOTO55
IF[#17GE.2]GOTO8
#17=.2
N8#100=#5003(STORE CURRENT Z POSITION)
G0Z#18(RAPID TO R PLANE)
#101=ABS[#5003-#26](CHECK FOR REMAINING DISTANCE #101=FINAL DEPTH)
#103=#18(SET 103 TO R PLANE, #103=NEW "R" IN PART)
WHILE[#101GT[#4+.02]]DO1(TEST 101 FOR FINAL DEPTH)
#149=0
WHILE[#3NE#149]DO2(CHECK FOR RETURN TO "R")
G0Z#103(RAPID INTO NEW "R" PLANE)
IF[#101LE[#4+.02]]GOTO2
#103=[#5003-#4](NEW DEPTH)
G1Z#103F#9(FEED TO "Z")
#101=ABS[#5003-#26](RECALIBRATE DISTANCE TO GO)
#103=#103+.1(RETURN PECK IN "R" PLANE)
G0Z#103(RAPID TO NEW "R")
#4=[#4*#5](RECALCULATE FEED DISTANCE)
#149=#149+1(INCREMENT COUNTER)
IF[#4GT#17]GOTO1(CHECK FOR MINIMUM PECK)
#4=#17(SET TO MINIMUM PECK)
N1END2
G0Z#18(RAPID TO ORIGIONAL "R" PLANE)
END1
G0Z#103(RAPID TO PECK RETURN PLANE)
N2G1Z#26(FEED TO FINAL Z)
GOZ#18
N3G0Z#100
#4=#10

GOTO4
(ERROR STATEMENTS)
N50#3000=1(NO VALUE IN Z)
N51#3000=2(NO VALUE IN R)
N52#3000=3(NO VALUE IN F)
N53#3000=4(NO VALUE IN I)
N54#3000=5(R IS DEEPER THAN Z)
N55#3000=6(J VALUE MUST BE LE 1.)
N4M99

%

  • Like 3

Share this post


Link to post
Share on other sites

Yes I think this is the custom cycle I've been looking for! To input any values as desired and allowing the cycle to figure the remaining depth.

I'll try to copy and paste to see if it works.  Because I'm not sure what kind of custom features differ from the two hopefully it will work. I'll run it in air before test cut...

Thanks a million!

Share this post


Link to post
Share on other sites

I was under the impression the G83 and subsequent peck would be used for that purpose. I find that it is not.

So what is the subsequent meant for?

My code using .250 initial peck and .100 subsequent :

G43 H43 Z.5
G94
G99 G83 Z-1. R.5 Q.25 F3.57
G80
G49
M05

 

I could have sworn years ago I used it and the first peck would typically cover my retract distance and subsequent would be what I used in material.

Share this post


Link to post
Share on other sites

Bill, the code you seek is in most of the newer Gen Haas posts...

Share this post


Link to post
Share on other sites

Thanks John.

I had to repost my program to run on a Doosan DVF8000.  Which resulted in a broken drill. R.250 Q.250 doh!  My bad. Just assumed it would post a peck reduction. Luckily it was just a fixture.

 

Share this post


Link to post
Share on other sites
On 3/2/2021 at 8:46 PM, Colin Gilchrist said:

*Be careful about using G98 versus G99. If you use G99, it *should* return to the Initial Point, after finishing the G83 Peck Drill.

G81, with those parameters, starts at Z0.1, then drills to Z-.64, then returns to Z.1

G83 starts at the Initial Point (Z.1), should rapid to the R Plane (Z-.6), then peck from there. (Note: It won't rapid out of the hole, due to the R plane, so it is kind of more like a chip-break cycle. When the cycle finishes, the G99 tells it to return to the Initial Point. It wouldn't hurt to make this little modification:

%

O5001

G00 Z0.1

G99 G81 Z-0.64 R.1 F20.

G99 G83 Z-1.1 R-0.6 Q.1

Z0.1 G80

M99

%

Everydays a schoolday!

I always thought end of cycle (before calling another cycle) needed a G80 so the G99 line would have needed the G80 between the following G99 line.

And then the G80 had to be on a separate line....like the below!

%

O5001

G00 Z0.1

G99 G81 Z-0.64 R.1 F20.

G80

G99 G83 Z-1.1 R-0.6 Q.1

Z0.1

G80

M99

%

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us