Custom drill cycle...

[?Mark]

Hi everyone.

I've been using carbide drills with din holes for a few years now(high pressure coolant),but would like a drill to slow down when it goes into a part and after a certain distance to resume a normal feedrate.

How do you deal with this?

Custom drill cycle, long hand code...?

The reasoning behind this is, I'm trying to get a little better positioning accuracy since I can't use center or spot drill with this kind of drills.

Your help as always is greatly appreciated

It is for Mori SV50 with Fanuc 16 control (MSC 516)

Kind regards, Mark

[crazy^millman]

Do a search for deep hole drilling cycle Macro that James did not to long ago. I am thinking you could modify it to your needs.

[?Mark]

Thanks Ron, I couldn't find it on fist try, but since you say it's there I'll go look again

Kind regards, Mark

[crazy^millman]

All credit for this goes to James but here is what he had put up in a thread.

 

code:

---

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)

(#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

---

HTH

[Tim Johnson]

quote:

---

The reasoning behind this is, I'm trying to get a little better positioning accuracy since I can't use center or spot drill with this kind of drills.

---

Have you tried this technique and if you have how much more accurate is it? You can create a custom drilling cycle for this but I'm thinking for better accuracy you might be better off pilot drilling with a stub length thru coolant drill. The drill cycle Ron put up is a custom macro drilling cycle but not a custom drill cycle for the post.

[?Mark]

quote:

---

Have you tried this technique and if you have how much more accurate is it?

---

It does help a bit on up to 4xdia. I haven't had a chance to try it on deep holes yet but I believe there is a big advantage of doing it this way.

 

On a rigid setup: .250 drill, cat-50 holder, command xt precision collet chuck (the whole setup doesn't get much better ) I'm off by up to .0011" location wise in A2 steel (over the range of 200 holes). Using my way seems to get location down to about .0007" at the most.

There are some variables as how close the shank of the drill is to optimal holding range of a collet and so on, but general idea of slowing down on entrance especially on deep holes came to me from a local rep.

Any sugestions?

 

Thanks Ron, found this link but it's not exactly what I'm looking for (too complicated ).

 

 

That just about makes it my longest post

Kind regards, Mark

[Lars Christensen]

Millman,

You have a pretty good understanding how low my skill level is (thank you for all the help you have provided, owe you just about a house by now). Macro use is something that I in a long time have wanted to get into, and this Macro looks cool, is this Macro coming with a manual . I know my Haas has a Macro site, I am using it for a tool probe we have, but how do I input all the values in my program?

 

Thanks Lars

[Tim Johnson]

Mark,

 

I thought I'd have something for you now but it's been a busy day. I will get you a custom drill cycle as soon as I get time.

[?Mark]

quote:

---

I thought I'd have something for you now but it's been a busy day. I will get you a custom drill cycle as soon as I get time.

---

Thank you very much Tim

Where do I sign you up for a reward

Kind regards, Mark

[crazy^millman]

Well that is a very good Macro James had I was just lucky enough to be making a book from this place as I call it. I have at this point 100's of pages of stuff off of here. I think it is important I copy to word then print to keep in a notebook. I have all of the 5 axis power point printed, Vb stuff, and other things as well. There has been links to Macro sites where people have stuff to help you with it.

 

I think the biggest thing about Macros is knowing Algebra. Macros are just word equations so get an Algbera book to study up on word equations and that in my mind would help. The other thing is use examples liek this and othere people have put up to get ideas from. I have learned alot just by doing that very thing.

 

He who knows it all, knows nothing if he can not learn from others.

 

HTH

[jeff]

On a couple of our machines,we use this sub before EACH hole that has a tight tolerance of less than .001 :

 

G00G91X-1.Y1.

G01X1.Y-1.F50.

G90

M98

 

The only drawback is you would have to call the G83 before every hole location.

But maybe you could create a macro that would do this for you.

HTH

[Tim Johnson]

Mark,

 

Do you want to use G81 or G01 calls? My thoughts would be use G01 to get to your entrance point and then G81 for the rest of the hole. My reasoning behind this is if you ever need to change to a pecking, chip break or c-bore cycle it would be easy to copy this cycle to the next one and make the changes. The more efficient way is G01 though. Also do you change speeds on your entrance?

quote:

---

Where do I sign you up for a reward

---

Just keeping my name off the dart board is enough for me.

[?Mark]

I'm not sure Tim. Was thinking more along the lines of G81 but there has got to be G1 line in there anyway, so G1 alone would be great also.

Surprised that no one tried it before, seems to be pretty handy to go slower on entance.

No need to adjust rpm.

 

Appreciate your help

 

Kind regards, Mark

[Tim Johnson]

Here it is;

 

Edit this in the .txt file;

code:

---

[drill cycle 10]

1. "Reduced entry feed drill"

2. "Feed rate"

3. ""

4. "Clearance..."

5. "Retract..."

6. "Depth..."

7. ""

8. ""

9. ""

10. "Entrance feed rate"

11. "Entrance Depth [abs]"

---

In the fmt section;

code:

---

fmt  Q  2   peck1       #First peck increment (positive)

fmt 2 peck2 #Second or last peck (positive)

fmt 2 peckclr #Safety distance

fmt 2 retr #Retract height

fmt Q 2 shftdrl #Fine bore tool shift

fmt Z 2 entryz #Entry Z for custom drill <<<<<<<<<<<<<<<<<<<<<<< add this line

---

In the pdrlcst segment

code:

---

pdrlcst         #Custom drill cycles 8 - 19 (user option)

#Use this postblock to customize drilling cycles 8 - 19

pdrlcommonb

#if drillcyc = 8, pcan1, pbld, n, *sgdrlref, *sgdrill, pdrlxy, pfzout, pcout,

# prdrlout, dwell, *feed, strcantext, e

if drillcyc = 8, # Subprogram Call cycle

[

sub_prg_call = peck1

pcan1, pbld, n, *sg00, *sgabsinc, pfxout, pfyout, strcantext, e

pbld, n, "M98", *sub_prg_call, e

]

if drillcyc = 9, # Reduced entry feed cycle <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<, add from here

[

savdrl_gcode = gcode

entryz = shftdrl

pdrlcommonb

pbld, n, pdrlxy, e

pbld, n, *sg01, *entryz, "F", no_spc, *retr, e

pbld, n, *depth, *feed, e

pbld, n, *sg00, *refht, e

drillcyc = 12

pcom_movea

] # <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< to here

#else, "CUSTOMIZABLE DRILL CYCLE ", pfxout, pfyout, pfzout, pfcout, e

#pcom_movea

 

pdrlcst_2 #Custom drill cycles 8 - 19, additional points (user option)

#Use this postblock to customize drilling cycles 8 - 19

pdrlcommonb

#if drillcyc = 8, pcan1, pbld, n, pdrlxy, pzout, pcout, prdrlout, dwell,

# feed, strcantext, e

if drillcyc = 8, # Subprogram Call cycle

[

sub_prg_call = peck1

pcan1, pbld, n, *sg00, *sgabsinc, pfxout, pfyout, strcantext, e

pbld, n, "M98", *sub_prg_call, e

]

if drillcyc = 9, # Reduced entry feed cycle <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< add from here

[

savdrl_gcode = gcode

entryz = shftdrl

pdrlcommonb

pbld, n, pdrlxy, e

pbld, n, *sg01, *entryz, "F", no_spc, *retr, e

pbld, n, *depth, *feed, e

pbld, n, *sg00, *refht, e

drillcyc = 12

pcom_movea

] # <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< to here

#else, "CUSTOMIZABLE DRILL CYCLE", pfxout, pfyout, pfzout, pfcout, e

#pcom_movea

---

That should do ya. I set this for custom drill 10. If you want a different number the .txt file will have the new custom number and the drill cycle numbers will be the new number-1. E-mail me if you have any problems and we'll work them out.

Note: This is from the MPmaster post

[?Mark]

Looks great Tim. Hope I can get it to work with my mpfan post

Kind regards, Mark