Deep hole drilling cycle

[Bob W.]

I am trying to add a deep hole drilling cycle to my post that will work as follows:

 

1. Feed drill into starter hole at 100 rpm

2. Increase rpm to drilling speed (3500 rpm)

3. Turn on TSC (per drill tool settings)

4. drill hole

5. With drill still in hole, reduce spindle speed back to 100 rpm

6. Turn off TSC

7. Retract drill from hole

 

I am setting this up under custom drilling cycles (cycle 19) and I need a little help. When the tool is first loaded the posted code spins the tool up to 3500 rpm right away. I was able to override this with a probing cycle (if t$ = 60, *speed, *spindle) but I am not sure how to handle multiple contingencies to handle deep hole drilling as well.

 

Here is what I have so far

 

Post logic:

 

pdrlcommonb										 ####### DEEP HOLE DRILL 9/3/2013 RWW
if drillcyc$ = 19,
[
z_feedplane = drl_prm1$
dhpeck = drl_prm2$
probe_clr1 = initht$
"(DEEP HOLE DRILL)", e$
pbld, n$, "S100 M3", e$
pbld, n$, "Z", *z_feedplane, *feed, e$ #WDS
pbld, n$, *speed, e$
pbld, n$, "G90 G81", *pfzout, *pcout, "R", *z_feedplane, *dhpeck, *feed, strcantext, e$
pbld, n$, "S100", e$
pbld, n$, *prdrlout, *feed, e$
pcom_movea
]

 

Posted code:

 

N417 G0 G17 G40 G49 G80 G90 G53 Z0.0
T417 M6 (12MM COOLANT THRU DRILL)
(OPERATION 1: )
#551=.4724 (TOOL DIAMETER VALUE)
/8 M98 P8100 (TOOL SETTING)
M557 (TOOL OFFSET CHECK)
G54 G90 G0 X0. Y0. S3500 M3
G43 H1 Z.25 M26
(DEEP HOLE DRILL)
S100 M3
Z-.3 F35.
S3500
G90 G81 Z-5. R-.3 Q2. F35.
S100
R0. F35.
G80
M9
/9 M98 P8101 (TOOL BREAK DETECT)

 

I'm sure there are a number of things I could be doing better. Any help or advice would be appreciated.

[Brando]

heres how my post outputs , if you want ill send you the post, macro, and control def it could be refined im sure but we dont do too much deep hole drilling

 

i know it says jobber drill i couldnt think of a file i have with a deep hole drill off the top of my head,

but i put the tsc commands in the macro for "g72",

the "S" is for the proper rpm, and the D is used to feed in from the r plane at 1.5 or 2.0 x the d value, then it kicks up the rpm to the S value and turns on tsc, feeds to z depth at F, then it backs off incremental .015, coolant off and spindle 150 rpm ,then feed out at 3 or 4x the F to the r plane

 

N10

(TAP DRILL 8-32)

(MC TOOLPATH# 8 )

T27 M06 (NO. 25 JOBBER DRILL)

M61

(UNLOCK TABLE)

G00 G17 G90 G54.1 P5 B86. X0. Y0. S100 M03

M10 (LOCK TABLE)

G43 H27 Z2.

G94

G72 X0. Y0. Z-.4649 R.04 S6387. D.1495 M03 F21.

G80

G91 G30 Z0. M05

G49 G90

M01

[Bob W.]

So G72 is a macro that resides on the machine? I hadn't really thought of doing it that way. I'd love to see the files.

[Brando]

yea the g72 working like a g65 simple call

it is assigned (if my memory serves me) somewhere between parameters 9010 and 9020 on a 16 or 18 series im not sure about the 30 series so that it calls up a macro program 9010 or 9011 9012 etc...

you could also do a g66 pxxxx that would work like a canned cycle where it stays in the mode and just change the x, y and repeats the cycle, i dont have the post for that type but it is another possibility

ill collect the necessary files at work tomorrow and put em on the ftp when I have a chance

[Guest MTB Technical Services]

Bob,

 

What you're really looking to would more commonly be called a gun-drilling cycle.

On oil-field parts like blow-out preventers, it's quite common to gun-drill 36" deep or greater.

For larger diameter drills with extended length, going to full cutting RPM immediately is just too dangerous.

The tool will whip without the support of the starter hole as a guide bushing.

 

Also, if you are doing this on a HMC, you'll REALLY want to consider entering your starter hole with the opposite rotation.

The added issue of droop from horizontal mounting will make this a necessity.

That's they way I do it and it WILL save you tooling.

I've watched people try it without opposite rotation and have the drill edge bite and then it's busted tool that went into launch mode at terminal velocity.

[Guest]

I did a gun drill cycle some time back, maybe the skeleton of it might be helpful

 

http://www.emastercam.com/board/index.php?showtopic=24080&hl=drill

[Guess_who]

Here is a very simple subprogram macro that we use here.

 

O9981( DRILLED HOLE SPECIAL )
( E = #8 ENTER/EXIT FEEDRATE )
( F = #9 - CUT FEEDRATE )
( I = #4 ENTER CUT FEED OR .6 OF CUT )
( R = #18 - START DRILL R-PLANE )
( S = #19 - FULL DIA -Z- FOR INIT FEED )
( T = #20 - RAPID PLANE )
( W = #23 - START BREAK-THRU -Z- )
( Z = #26 - FINAL -Z- DEPTH )
#100=#5003
IF[#19EQ#0]THEN#19=#18
IF[#20EQ#0]THEN#20=#18
IF[#4EQ#0]THEN#4=[#9*.6]
IF[#23EQ#0]THEN#23=#26
IF[#8EQ#0]THEN#8=[#9*5.]
G0G90Z#20
G1Z#18F#8
Z#19F#4
G1Z#23F#9
Z#26F[#9/2]
Z#18F[#8*2]
G0G90Z#100
M99

 

Then we have our post setup to spit out just a G65 or G66 P9981

 

If you want to see the post code used, let me know.

 

Just an idea.

[Brando]

Bob,

 

Also, if you are doing this on a HMC, you'll REALLY want to consider entering your starter hole with the opposite rotation.

The added issue of droop from horizontal mounting will make this a necessity.

That's they way I do it and it WILL save you tooling.

I've watched people try it without opposite rotation and have the drill edge bite and then it's busted tool that went into launch mode at terminal velocity.

 

ive never considered that factor, but i did just change all my macros to reverse the spindle on the entry, thanks for the tip

 

another tip for anyone is to slow the tool changer speed down, most machines have a mcode for slow tc cycle, in addition i slowed the slow tc cycle for our doosan hmc even slower in the machines parameters for smoother operation i had a few that broke off during a tc

[Bob W.]

Thanks for the replys. It has been a pretty busy day with training so I haven't had a chance to digest it all yet. Weekend project

[Bob W.]

Thank you all for the help. I have the structure of the post working well and there are two distinct directions I can take on this. I can have the program call the drill cycle with a G66 macro call and the actual cycle will be stored in the macro on the machines (strategy 1), or I can have the program post the entire routine for every hole location (strategy 2). Any thoughts on advantages/ disadvantages of each strategy?

 

Strategy 1:

 

G66 P9001 Z, S, D

X..., Y...

X..., Y...

X..., Y...

G67

 

 

Strategy 2:

 

X..., Y...
S100 M3
Z-.3 F35.
S3500
G90 G81 Z-5. R-.3 Q2. F35.
S100
R0. F35.
X..., Y...
S100 M3
Z-.3 F35.
S3500
G90 G81 Z-5. R-.3 Q2. F35.
S100
R0. F35.
X..., Y...
S100 M3
Z-.3 F35.
S3500
G90 G81 Z-5. R-.3 Q2. F35.
S100
R0. F35.

[Guest MTB Technical Services]

Bob,

 

Save your macro on the machine and create a custom G-Code for it.

It will simplify the post and reduce the required code output as well make it easier for the operator reading the data.

 

Be careful using 9001 or 9010 as your macro program number.

Those 2 numbers are the most commonly used for custom M06 Tool Change macros.

Parameters #6050 through #6059 hold the actual G-Code integer you wish to use.

9001 can't be assigned through these parameters as the referenced program IDs start at 9010.

However, it can be used for custom M-Codes so be careful.

 

With custom G & M codes it is important to keep in mind that you should use custom G-Codes only if you are actually parsing macro data through the use of variables.

If there isn't any Macro calculation actually being done, create a custom M-code that references a sub-program instead of a macro as trying to execute it as a custom M-code Macro will cause an alarm.

I use custom M-codes for aliasing M-codes for things like air through the tool where this isn't standard on all Fanuc based machines.

You can standardize your output this way across multiple machines with Fanuc controls from different builders.

[Bob W.]

Thanks Tim. The 9001 macro was just the first 9000 series number that came to mind. When I do assign a number to it there will be some thought involved to make sure it will work on both Fanuc based machines. One thing I like about the G66 call is I can do multiple holes in one operation. I will be passing along a lot of information to the macro in the G66 or assigned G code command including peck depth, coolant type, hole depth, spindle speed, etc... Is it possible to do multiple holes in one operation with a standard G code call? If I were to assign G72 (wild guess) to the macro I could post something like this:

 

G72 X1, Y1, Z-3., S2500, M26, D2.0 (peck depth)

G72 X2, Y2, Z-3., S2500, M26, D2.0 (peck depth)

...

 

Would all of that information be passed to the macro the same as a G65 or G66 command?

[Guest MTB Technical Services]

Bob,

 

Yes. you can make your custom G-code arguments modal or non-modal.

All the arguments would be read the same way.

 

Let's say you decide on G181 as your custom G-code and your Macro Program number is 9011.

If you set the integer in parameter #6051 to a negative value (-181) it will treat all the arguments as modal.

This means you can treat it just like a regular drill cycle as the call itself (G181) and all the arguments are still modal.

 

Now keep in mind that a modal macro requires explicit cancellation whether or not it is used for a custom G-Code.

 

You can handle this by using the G67 directly or creating a custom G80 subprogram uses the standard G80 but also would include the G67.

You could also create a completely separate code like G180 that uses the standard G80 but also would include the G67

[Zbuilder]

On ‎9‎/‎6‎/‎2013 at 10:25 AM, Brando said:

another tip for anyone is to slow the tool changer speed down, most machines have a mcode for slow tc cycle, in addition i slowed the slow tc cycle for our doosan hmc even slower in the machines parameters for smoother operation i had a few that broke off during a tc

Hey Brando, we would like to slow our Doosan TC also but can't find the param or Keep relay for it. Can you tell my which one and I'll see if ours is compatible. Thanks