Deep hole drilling

Good afternoon,

I am doing deep hole drilling in 4140 material to about 18" deep with a 7/16 hss drill. Is there a drill cycle or code to put in my G83 that would allow me to start at my R.1, have the first peck go 10" down, then continue to 18" with a peck of .15?

You're assuming too much.
Like we all know what machine and control you're doing this on for starters.

You could have wrote it by hand by now and had it to exactly what you wanted.

Haas has some extra variables on drill cycles but like Mtn said, what machine?

Hi Schotz11:
Is there a typo in your first post?
It reads to me like you want your first peck to be 10" deep?
Should it be 1" deep instead?
The rules I learned way back when were: first peck was to be maximum 3X drill diameter to avoid flute packing.

Moving on; have you considered and rejected gun drilling them?
Even if you don't want to farm it out to a gundrilling company, there are setups available for bog standard CNC machines and even manual machines.
You have to prep the bar end rather than running the drill through a removable bushing but they apparently work very well, although I've never run one.
There are no pecks necessary when gundrilling and you get better holes faster too.

Moving on to your question directly; I've always programmed oddball drilling cycles by hand to get what I want, however so far as I know the G83 variable peck cycle increments the pecks smaller by a peck reduction increment you specify for each successive peck after the first one until it gets to the minimum you also specify and then it goes the rest of the way at that increment.
So a standard Fanuc variable peck cycle will get you almost what you requested. (assuming your control will support it)

Here's a link to a blurb about it:
G73 and G83 Peck Drilling Cycles

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

Yes, you use I,J,and K, (Iirc), First peck depth(I), then how much less each subsequent peck(J) till you get to the minimum peck(K).

implmex said:

Hi Schotz11:
Moving on to your question directly; I've always programmed oddball drilling cycles by hand to get what I want, however so far as I know the G83 variable peck cycle increments the pecks smaller by a peck reduction increment you specify for each successive peck after the first one until it gets to the minimum you also specify and then it goes the rest of the way at that increment.
So a standard Fanuc variable peck cycle will get you almost what you requested. (assuming your control will support it)

Here's a link to a blurb about it:
G73 and G83 Peck Drilling Cycles

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

Click to expand...

Hello Marcus,
Variable Peck amount during one G83 Cycle is not possible with a Fanuc Control. Haas Yes, Fanuc No.

It would help a lot if the OP were to declare the make and model of the control being used.

Regards,

Bill

Hi Bill:
Thanks for chiming in; I always learn something new when you contribute, and i appreciate it.
I was unaware of that particular nugget; I've never used that variant of G83 so I was going only by what I'd heard, not by anything I've actually tried.
I don't really run production anyway, so that sort of cycle optimization is almost meaningless for what I do.
I just assumed that any reasonable sophisticated Fanuc control would be able to run variable peck G83.

Cheers

Marcus

G81 G99 Z-10. R.1 F_
G83 G99 Z-18. R-9.9 Q.15 F_ (Or G73 if you don't want your pecks to come all the way back to the R-plane)
G80



Probably not the wisest strategy, but there you go...

some use G98 and not G99 that is you can have drill go or retract to initial Z up out of the hole at every hole if you want and have R down in the hole
.
thus you can use one G83 to drill 6" deep and another G83 with a longer drill rapid down into hole say 5.8" deep and start drilling at feed again. you can have 10 each G83 on same hole position and each have different peck and feed rate and different R and different Z if thats what you want.
.
or use many G73 or short peck on same hole position. so drill pulls all the way out say every 3" on a 12" deep hole. thus you get the long peck all the way out of hole AND a short peck combination if thats what you want. often used when coolant not reaching drill tip and a over 9" deep horizontally drilled hole with only external coolant
.
many variations are possible. often just using multiple G83 on same hole location is easiest

The obvious problem with having a retract plane that is 10" deep, is chip control. What they need is a G-code that makes chips disappear, into thin air. (Not heavy air).

R

actual a big problem with deep holes if on full retract out of hole if any chips still in the hole and you rapid peck back in hole the chips get pushed to bottom of hole and when compressed at high rapids its like hitting a solid wall
.
usually a parameter can adjust how far from last peck rapids stop like 0.1" or 0.15" in case operator leaves it at 100% rapids. many a B axis on a horz cnc will get pushed out of B position cause big spade drill going back in hole at high rapid and chips still in the hole
.
also if down in hole chip or burr sticking up it helps drill tip if rapids stop some distance away from last peck. different material might need more distance. many many people have pecking trouble cause they dont appreciate this often critical distance and peck rapid speeds and slamming into compressed chips at hole bottom

implmex said:

Hi Bill:
Thanks for chiming in; I always learn something new when you contribute, and i appreciate it.
I was unaware of that particular nugget; I've never used that variant of G83 so I was going only by what I'd heard, not by anything I've actually tried.
I don't really run production anyway, so that sort of cycle optimization is almost meaningless for what I do.
I just assumed that any reasonable sophisticated Fanuc control would be able to run variable peck G83.

Cheers

Marcus

Click to expand...

Hello Marcus,
Following is a Deep Hole Peck Drilling Macro I wrote on request of a Forum member a few years ago, where the Peck, Feed and Spindle Speed can be varied. I'm not sure if this is the final version, but without examining it in detail, my comments at the end still apply.

Regards,

Bill
%
O0001
N1 G00 G17 G21 G40 G80 G94
G91 G28 Z0.0
G28 Y0.0
T01 M06
S2000 M03
G90 G54
G00 X10.0 Y50.0
G43 Z10.0 H01 M08
G183 Z-50.0 R-20.0 Q5.0 K0.50 E0.250 F100
G91 G28 Z0.0 M09
G28 Y0.0
M01

The above will call Macro Program O9010 if 183 is registered in parameter 6050

If its to be called to repeat at a number of X,Y coordinates, the Macro can be called using the Modal Call G Code G66 as shown in the following example:

%
O0001
N1 G00 G17 G21 G40 G80 G94
G91 G28 Z0.0
G28 Y0.0
T01 M06
S2000 M03
G90 G54
G00 X10.0 Y50.0
G43 Z10.0 H01 M08
G66 P9010 Z-50.0 R-20.0 Q5.0 K0.50 E0.250 F100
G00 X40.0 Y80.0
X60.0 Y90.0
X80.0 Y100.0
X100.0 Y110.0
G67
G91 G28 Z0.0 M09
G28 Y0.0
M01

Where:
Z = #26 - Final Z
R = #18 - R Plane
Q = #17 - Peck value
K = #6 - Clearance on return
E = #8 - Dwell when retracted from hole
F = #9 - Feed Rate
S = #19 - Feed Change Z Level
W = #23 - Reduced feed
D = #7 - Speed Change Z Level
V = #22 - Initial Spindle Speed
B = #2 - Spindle Speed
H = #11 - Percentage of Spindle Speed
J = #5 - Peck reduction factor
C = #3 - Min Peck amount

The above is a Modal Call of the Macro Program, and repeat at the X,Y coordinates following the call block and before the Modal Cancel G code, G67.

In both the above methods of calling the Macro Program, the K and E arguments can be omitted and default values will be applied in the Macro program.

O9010
IF[[#9 EQ #0]OR[#17 EQ #0]OR[#18 EQ #0]OR[#26 EQ #0]]GOTO100 (ERROR TRAP FOR MISSING REQUIRED ARGUMENTS)
IF[#6 EQ #0]TH #6=0.25 (DEFAULT RETRACT OFFSET)
IF[#8 EQ #0]TH #8=0.0 (DEFAULT DWELL) (THIS BLOCK IS NOT REALLY NECESSARY - ITS JUST CLEANER PROGRAMMING)
#17=ABS[#17] (ENSURE VARIABLE IS ABSOLUTE VALUE)
#6=ABS[#6] (ENSURE VARIALBLE IS ABSOLUTE VALUE)

#27=#4003 (STORE THE GROUP 3 G CODE - G90/G91)
#28=#5043 (STORE THE INITIAL Z COORDINATE)

#1=#18 (INITIALLY SET #1 TO THE R PLANE)
#4=#18 (USE A COPY OF #18 TO MODIFY IN THE MACRO)
N10
#1=#1-#17 (Q PECK AMOUNT) (CUT IN Z COORDINATE)
IF[#1 LT #26]TH #1=#26 (ENSURES NO OVER CUTTING IN Z)
#17=#17 * #5 (CALCULATE NEW PECK VALUE)
IF[#17 LT #3]TH #17=#3 (ENSURES PECK IS NO LESS THAN SET MINIMUM)
IF[#1 LE #19]TH #9=#23 (FEED CHANGE TEST)
IF[#1 LE #7]TH #2=#22 * [[100 - #11] / 100] (SPEED CHANGE TEST)
G90 G00 Z#4
G01 Z#1 F#9
#4=#1+#6 (K - RETURN OFFSET)
G00 Z#28 (INITIAL LEVEL)
G04 X#8 (E DWELL - IF REQUIRED, SO COOLANT OR AIR BLAST CAN ENTER THE HOLE)
IF[#1 GT #26]GOTO10
GOTO200
N100
#3006=1(MISSING DATA IN CALL BLOCK)
N200
G#27 (RESTORE GROUP 3 G CODE)
M99
%

I've not tested the program on a machine. Accordingly, proceed with caution if you use it. However, I can't see any blaring mistakes.

Regards,

Bill

implmex said:

.....I just assumed that any reasonable sophisticated Fanuc control would be able to run variable peck G83..

Click to expand...

Not specifically talking about deep hole variable pecking....

Years ago when discussing control features with some fairly high level Fanuc engineers, I asked why they did not try to "keep up" with other control builders as far as milling cycles were concerned. Their somewhat confused response was that they support any kind of cycle the customers wishes to implement. All a user has to do is determine what they want the cycle to do and create a macro to perform the task. They said they felt it was better to provide a tool for users to create their own cycles. They can be written to perform how they wanted them to perform rather than having to use a cycle that worked just one way which might not be how the user preferred.

I agree to some extent with that, but over the years have determined that few users want to invest the time into learning macro programming, let alone actually write them.

I'm guessing that he wants to change tools at the 10" line, so's not to put unneeded wear on the most expensive tool.

10/1 odds that this is going to be long coding.


Sure hope this is horizontal!
If not - I'd like to see the vert with that much daylight!



---------------

Think Snow Eh!
Ox

Over 40xD.....Yikes! Out of curiosity, what's your machine and tooling situation? I've done 20xD in brass with a long parabolic flute drill, but at 41xD and change and in 4140 I'd be looking at gundrilling that. Maybe I underestimate what can be done with good tools and TSC?

Has anyone here done this in 4140 and a HSS twist drill?
I think a HSS drill is of this L/D going to be lacking torsional stiffness.
So it will wind up like a spring in the cut and then relax with the peck pullout.
Then when reentering the cut it is gonna wind up again meaning no cut at first but a sort of chiseling the Z into the part.
Perhaps a very fancy macro where the intial entry is a lighter feed to allow for the wind up or just a super light feed per rev.
I wonder under normal feed rates what the windup would be in degrees.
It of course depends on drill core diameter but this is a very long drill. Lots of flute area wanted to transport the chips but that makes the tool weaker to rotation.
Bob

CarbideBob said:

I think a HSS drill is of this L/D going to be lacking torsional stiffness.
So it will wind up like a spring in the cut and then relax with the peck pullout.
....
I wonder under normal feed rates what the windup would be in degrees.
It of course depends on drill core diameter but this is a very long drill. Lots of flute area wanted to transport the chips but that makes the tool weaker to rotation.
Bob

Click to expand...

That's what I was thinking! Chip clearing aside, 4140 isn't particularly soft and will take a not insignificant cutting force.

CarbideBob said:

Has anyone here done this in 4140 and a HSS twist drill?
I think a HSS drill is of this L/D going to be lacking torsional stiffness.
So it will wind up like a spring in the cut and then relax with the peck pullout.
Then when reentering the cut it is gonna wind up again meaning no cut at first but a sort of chiseling the Z into the part.
Perhaps a very fancy macro where the intial entry is a lighter feed to allow for the wind up or just a super light feed per rev.
I wonder under normal feed rates what the windup would be in degrees.
It of course depends on drill core diameter but this is a very long drill. Lots of flute area wanted to transport the chips but that makes the tool weaker to rotation.
Bob

Click to expand...

I had that issue in a long drill in 310SS (posted about recently in other thread).
But it didn't behave like you say.
In my case it would wind up and release. Wind up and release.
Pop, pop, pop .....

Have you experienced a "wind and hold" application before, or are you just envisioning it?

I had to go to carbide to address that issue.
I was only 14D at that, but only at 7/32".
I'm not sure that the 7/16 drill would act the same at the same L/D?
I doubt that is a linear reaction?
I understand this is 40D - so may be same results? Drill mfgr should know what to expect.


----------------------

Think Snow Eh!
Ox

Ox said:

....

Have you experienced a "wind and hold" application before, or are you just envisioning it?
......

Think Snow Eh!
Ox

Click to expand...

Confused or maybe my wording not right.
They always wind up and then pop back to free state.
At this L/D I'd think enough to destroy a twist drill.
The reentry from a peck has to be brutal to both the tip and shank.
For that first little bit everything is going wrong during the rewind back.
Flank angle will not be high enough, chip will not form correctly, shear plane will be all wrong.
You are hammering into the part.

Or maybe you are talking "pop-pop-pop" while in the cut which is the equivalent of turning an od with a tool chattering. Never works well.
Bob

Joke about "twist" drills goes here?