Carbide drill "custom drill cycle"

[Gramby]

 We been having trouble with tool life on our solid carbide drills “corners chipping”. Currently we turn spindle thru coolant on and push the drill thru with no pecking. The tool salesmen wants us to change our procedure. To something similar to this.

 

1. Drill depth 1 ½ to 2X dia of drill with no spindle thru coolant but flood only and speed to be slower and feed to be slower.
2. Once we reach the 1 ½ to 2X depth we want the spindle thru coolant on and speed and feed increase to normal.

 

We believe the spindle thru coolant causes vibration at the drill point when starting a hole. Also wanting to start the drill at the material face less aggressively with less speed and feed.

 

Is this possible to do? Is there a drill cycle that does something like this? What type of procedures are others using?

 

We are drilling on a Johnford vertical machining center Fanuc control.

 

Mild steel die sets often 3 inches thick. Also commonly 4140 and Tool steels anywhere from 1.250 to 3 inches.

 

Yes we do spot drill first with a 140 deg carbide spotting drill. This 140 deg angle is larger then the drill point so the drill tip makes contact with the matl surface and not the drill edges.

 

Appreciate any input.

Thanks

 

[htm01]

we stopped spotting and have better life, over an 1" deep we use a short drill to pilot and then use a longer one

[MIL-TFP-41]

you can do what your looking for with a point(s) toolpaths.

A custom cycle would also work, tho it does mean some post modifications.

In to post section of this forum, search for gundrill. it will get you very close if you are looking to do the custom cycle route. The point toolpath route is effective, but time consuming if you got a whole bunch of holes to do.

[Gramby]

Mil -tfp-41  you have my curiosity with the points tool path. Never heard of this. Are you drawing points at different depths at a hole location or something?  Unfortunately yes we are doing many holes, sometimes a die set may have qty 400  3/8-16 tapped holes for example.

 

  We are not apposed to having our post altered if what we want is possible.

 

I am familiar with using a I,J,K in a G83 cycle to achieve a variable peck amount. But in addition to that we are wanting speed, feed and coolant type "spindle thru" to change in the middle of the drill cycle.

[bd41612]

Just to give you an idea:

drl_prm1$  = RPM for non cutting feed

drl_prm2$ = Pre-feed depth into pilot

drl_prm3$ = Dwell for speed change

drl_prm4$ = Retract rate or rapid, 0 is rapid

drl_prm5$ = Pilot infeed rate, 0 uses active feed rate

 

Postblock:

 

pdrlcst14   #Custom Drill cycle 14 - piloted deep hole
      if usecustpar = 0, result = mprint(scustperror)
      pdrlcommonb
      drl_prm1 = drl_prm1$
      drl_prm2 = drl_prm2$
      drl_prm3 = drl_prm3$
      drl_prm4 = drl_prm4$
      drl_prm5 = drl_prm5$
      if drl_prm3 = 0, drl_prm3 = 0.1
      drl_prm1, spindle, e$
      retraz = refht$
      if initht$ <> retraz, retraz, e$
      pilotz = (drl_sel_tos$ - drl_prm2$)
      if drl_prm5 = 0, drl_prm5 = feed
      "G1", *pilotz, *drl_prm5, e$
      *speed, *spindle, e$
      "G4" *drl_prm3, e$
      zdpth = z$
      "G1", *zdpth, *feed, e$
      drlz2 = zdpth + .03
      if (abs((drl_sel_tos$ - zdpth)*.05)) < .03,
       [
        drlz2 = zdpth + (abs((drl_sel_tos$ - zdpth)*.05))
       ]
      *drlz2, e$
      *drl_prm1, *spindle, e$
      "G4" *drl_prm3, e$
      if initht$ <> refht$, retraz = initht$
      if drl_prm4$ = 0, "G0", *retraz, e$
      if drl_prm4$ > 0, "G1", *retraz, *drl_prm4, e$
      if drl_prm4$ > 0, "G0"
      pcom_movea

[jlw™]

we stopped spotting and have better life, over an 1" deep we use a short drill to pilot and then use a longer one

I don't know what brand of drill your using but this will have an immediate impact. I run a lot of Guhring drills and never spot anything. I will however run a starter drill for deep hole drilling. If you haven't tried Guhring I highly recommend them. For those materials look at the drill guide:

 

https://www.google.com/url?sa=t&source=web&rct=j&url=http://www.guhring.com/documents/catalog/toolfinder/toolfinder.pdf&ved=0CDgQFjADahUKEwjU0YLkzInJAhXBVz4KHVNCDuY&usg=AFQjCNG438MmTwGf7m0pll5fQZTwRsjQlw

 

I have never had any issues with Guhring. You can program straight middle of the recommended f/s on the chart and expect your programs to run. If you have a production job you can tweak and push and get more out of them.

 

My local Guhring guy is Charles Simpson. He does a good and gave me one of my favorite sayings when he was referring to one of his drills:

 

"You gotta let that dog eat!"

[Guest]

IF I spot it is solely to just nick the surface. like .1mm-.2mm deep. I do not spot until after the hole is there then it for edge break to spec.

[Newbeeee™]

^^^this.

Straight in and spot to chamfer/deburr the hole after it's been drilled

[jlw™]

^^^^that right there^^^^^

Yep, me too but that's not a spot silly goose! You can also use any drill provided your guys touch off on tip and you know the angle. I also do it with some 45deg chamfer mills.

 

You can do it if they comp to full diameter but you'll get burned sooner or later.

[jeff]

 We been having trouble with tool life on our solid carbide drills “corners chipping”. Currently we turn spindle thru coolant on and push the drill thru with no pecking. The tool salesmen wants us to change our procedure. To something similar to this.

 

1. Drill depth 1 ½ to 2X dia of drill with no spindle thru coolant but flood only and speed to be slower and feed to be slower.
2. Once we reach the 1 ½ to 2X depth we want the spindle thru coolant on and speed and feed increase to normal.

 

We believe the spindle thru coolant causes vibration at the drill point when starting a hole. Also wanting to start the drill at the material face less aggressively with less speed and feed.

 

Is this possible to do? Is there a drill cycle that does something like this? What type of procedures are others using?

 

We are drilling on a Johnford vertical machining center Fanuc control.

 

Mild steel die sets often 3 inches thick. Also commonly 4140 and Tool steels anywhere from 1.250 to 3 inches.

 

Yes we do spot drill first with a 140 deg carbide spotting drill. This 140 deg angle is larger then the drill point so the drill tip makes contact with the matl surface and not the drill edges.

 

Appreciate any input.

Thanks

What brand of drills are you using?

As said above try Guhring. I've found they are the best. http://www.guhring.com/ProductsServices/Tools/?Type=1

Also, what is your runout? Speeds and feeds?

http://www.guhring.com/Documents/tech/speedfeed/5511.pdf

I spot with a 5/16 dia spot drill 142 degree .045 deep,  ONLY so my operators can check location of the hole pattern before drilling the holes,in case I programmed them wrong.

I don't need to spot,but that's just how I've always done it. 

[Gramby]

Thanks guys we do use Guhring drills. We only spot drill -.050 140 deg first to keep the drill centered well on position. We are Not spotting deep enough to chamfer the hole. We are using longer Guhring drills in order to get thru 3 inch die sets. Common carbide drill sizes we use are 13/64 , 17/64, 21/64, 23/64, 7/16, 31/64 and 17/32. We really can't sacrifice our 60 tool pod holder with duplicate drills. That being a short carbide drill for starting a hole and another tool pod holding a long carbide drill to get 3 inches plus deep.

My goal is to continue using our longer drills from start to finish. But take it easy with the drill for the first 1 1/2 times dia depth that being no spindle thru coolant and slower speed and feed. Then accelerate thru once at 1 1/2 times deep, dwell for a brief moment to turn spindle thru coolant on, and increase speed and feed to normal.

Perhaps what I am hoping for may not be possible. So I am certainly interested in hearing how others are drilling with carbide.

 

Thanks again,

Keep the comments coming.

 

PS I should add our max spindle speed is 4000 rpm. So some of those smaller drills we cant drill per recommedations. But we are maintaining the chip load.

[MIL-TFP-41]

Usually on holes that are more than 10X dia I will go in with a 3X dia drill first, drill in 2X dia deep, then load the long drill, enter the hole slow, ramp up rpm & go to town.

 

Like I said before, point toolpaths is an option, but cumbersome. A custom cycle is soooooo much easier, and reliable.

 

 

Point.zip

[djstedman]

Creating a hole that's that is 1 to 1.5 x diameter for depth prior to drilling with your long drill is going to give you the best hole..

 

You said you can't afford to have shorter drills in your magazine, but do you have an end mill available? If so you could just use a helical ramp and create your pilot holes that way.. just a thought. .

 

I can see the reasoning behind going slower and not using through coolant when starting the hole, but on some of those smaller drill sizes your up at 14x diameter, regardless what you change your cycle to, your still trying to pilot a hole with an extremely long drill that's not made to make a pilot hole.

[Matthew Hajicek - Singularity]

I spot face (flat) any non-flat surface before putting a carb drill into it.  If you do spot drill, you need to make sure the tip angles between the tools are compatible.

[crazy^millman]

Thanks guys we do use Guhring drills. We only spot drill -.050 140 deg first to keep the drill centered well on position. We are Not spotting deep enough to chamfer the hole. We are using longer Guhring drills in order to get thru 3 inch die sets. Common carbide drill sizes we use are 13/64 , 17/64, 21/64, 23/64, 7/16, 31/64 and 17/32. We really can't sacrifice our 60 tool pod holder with duplicate drills. That being a short carbide drill for starting a hole and another tool pod holding a long carbide drill to get 3 inches plus deep.

My goal is to continue using our longer drills from start to finish. But take it easy with the drill for the first 1 1/2 times dia depth that being no spindle thru coolant and slower speed and feed. Then accelerate thru once at 1 1/2 times deep, dwell for a brief moment to turn spindle thru coolant on, and increase speed and feed to normal.

Perhaps what I am hoping for may not be possible. So I am certainly interested in hearing how others are drilling with carbide.

 

Thanks again,

Keep the comments coming.

 

PS I should add our max spindle speed is 4000 rpm. So some of those smaller drills we cant drill per recommedations. But we are maintaining the chip load.

 

 I think is part of your problem is do want to spot. Your spot should be as big if not bigger than the drill. at .05 deep you are not creating enough area. Increase the area it come into contact with and see if it helps if you are dead set on spotting the holes 1st.

[cncchipmaker]

Thanks guys we do use Guhring drills. We only spot drill -.050 140 deg first to keep the drill centered well on position. We are Not spotting deep enough to chamfer the hole. We are using longer Guhring drills in order to get thru 3 inch die sets. Common carbide drill sizes we use are 13/64 , 17/64, 21/64, 23/64, 7/16, 31/64 and 17/32. We really can't sacrifice our 60 tool pod holder with duplicate drills. That being a short carbide drill for starting a hole and another tool pod holding a long carbide drill to get 3 inches plus deep.

My goal is to continue using our longer drills from start to finish. But take it easy with the drill for the first 1 1/2 times dia depth that being no spindle thru coolant and slower speed and feed. Then accelerate thru once at 1 1/2 times deep, dwell for a brief moment to turn spindle thru coolant on, and increase speed and feed to normal.

Perhaps what I am hoping for may not be possible. So I am certainly interested in hearing how others are drilling with carbide.

 

Thanks again,

Keep the comments coming.

 

PS I should add our max spindle speed is 4000 rpm. So some of those smaller drills we cant drill per recommedations. But we are maintaining the chip load.

If your machine has custom macro B I can write a macro for you that will incorporate everything you would like to try. If you are not sure if it has it just type in MDI #100=1. If you do not get an alarm your machine has macro B.

[Mike@Lustre]

I have always been told not to spot or center drill a hole to be drilled with a carbide drill , reason being all the initial cutting pressure is on the outside edge of the drill rather then being distributed across the cutting edge from the center out .

 

we run Sandvik and Iscar solid carbide drills with thru coolant we drill 303 ss or 6061-t6 all day and have drills that regularly get into the thousands for parts counts before being rotated out

[cncchipmaker]

Hopefully this will give you an idea of what you can do if you have macro B.

 

O5001(CARBIDE DRILL MACRO)
(ABSOLUTE MACRO)
(UNPROVEN)
 
(FORMAT G65/G66 DASFEZWR)
(D = #7    - DRILL DIAMETER)
(A = #1    - INITIAL RPM)
(S = #19  - SECOND RPM)
(F = #9    - INITIAL FEEDRATE)
(E = #8    - SECOND FEEDRATE)
(Z = #26  - Z START)
(W = #23 - Z END)
(R = #18  - R PLANE)
(*********************************)

(IF DATA LACKING GOTO N1000)
IF[[#7*#1*#19*#9*#8]EQ0]GOTO1000
(STORE ABS POS OF X)
#100=#5001
(STORE ABS POS OF Y)
#101=#5002
(CALCULATE Z POINT FOR)
(RPM AND FEEDRATE CHANGE)
(BASED ON 1.5 TIMES DIA. OF DRILL)
#102=#7*1.5
(INIITIAL RPM)
M03S#1
(TURN ON FLOOD COOLANT)
M08
(GOTO HOLE)
G0G90X#100Y#101
(RAPID TO .1 ABOVE Z START)
Z[#26+.1]
(FEED TO Z START W/ INITIAL FEED)
G1Z#26F#9
(STORE ABS POS OF Z)
#103=#5003
(GOTO RPM AND FEEDRATE CHANGE Z)
Z[#103-#102]
(TURN ON THRU COOLANT)
M26
(DWELL FOR 5 SECONDS)
(TO ALLOW THRU COOLANT)
(TO BE TURNED ON ALL THE WAY)
G4X5.
(SECOND RPM)
M03S#19
(FEED TO Z END W/ SECOND FEED)
G1Z#23F#8
(RAPID TO R PLANE)
G0Z#18
(TURN OFF COOLANT)
M09
(GOTO HOLE)
X#100Y#101
(RETURN TO MAIN PGM)
M99
N1000
#3000=1(DATA LACKING!)

[Gramby]

In regards to Spot drilling. This is really necessary for us. Because we are using long drills from start to finish. Unable to sacrifice another tool pod for pilot. Spot drill is keeping our position. Keep in mind our spot drill is 140 deg. Which is a greater angle then our Guhing drills. Thus when the drill makes contact with the material it is only cutting on the center and not the outer edges.

CNCchipmaker I am really liking your macro suggestion. Although in my 25 years of machining I have never used or seen a macro in use. Kind of over my head how to test and implement this. Does this macro sample you wrote above get implemented into the post or is this Macro stored in the CNC control panel? Also would using something like this drastically increase the program size? Would for example drilling qty 400 21/64 holes be much more then just moving to X , Y position in a drill can cycle? We will try your Macro

B test at the control soon. MDI #100=1

 

Thank You much

[djstedman]

Gramby,

 

Macro's are stored in the control as a separate program, then depending how you set them up, and how they are written, they can be called a number of ways..

 

A macro with no options to be set could be called with a regular M98 (though to be honest I don't know why you would do this)

 

A macro can also be used using a G65 call which lets you pass in values like you would in a canned cycle in order to modify the behavior of the program

for example.. you could pass in a D1.25Z-1.0  to control the diameter and depth of a hole (assuming you had a macro written to handle those values)

 

The last method you can use is a G66 Macro call which is a modal call and will work like a canned drill cycle where it will repeat the macro at each new position until it is cancelled.

 

On some controls it is also possible to 'link' a macro program to a G code so you can simply call a custom G code and it will call the macro..  this is particularly handy IMO when you create a modal macro that is made to utilize a G66 call ..

 

 

As for file size.. since the macro is a separate program and you can call it like you would another canned cycle.. it can be used without influencing file size if done correctly.

[cncchipmaker]

In regards to Spot drilling. This is really necessary for us. Because we are using long drills from start to finish. Unable to sacrifice another tool pod for pilot. Spot drill is keeping our position. Keep in mind our spot drill is 140 deg. Which is a greater angle then our Guhing drills. Thus when the drill makes contact with the material it is only cutting on the center and not the outer edges.

CNCchipmaker I am really liking your macro suggestion. Although in my 25 years of machining I have never used or seen a macro in use. Kind of over my head how to test and implement this. Does this macro sample you wrote above get implemented into the post or is this Macro stored in the CNC control panel? Also would using something like this drastically increase the program size? Would for example drilling qty 400 21/64 holes be much more then just moving to X , Y position in a drill can cycle? We will try your Macro

B test at the control soon. MDI #100=1

 

Thank You much

 

The macro is stored in the control and acts like a sub program and only uses the space of the sub so the program is much shorter. So basically what happens is that in your main program the sub is called using a G66(multiple positions) macro call  just before all of your hole locations and cancelled with a G67 after you are done with all of the holes. It is key that you do this. So for example the code in your main program would look like this:

 

G0G40G49G80G20G90G54

T1M06

G0G90G54X0Y0

G43Z5.H1

G66P5001D1.A2000.S3000.F10.E20.Z0W-2.R.1

(START HOLE POSITIONS)

X0Y0

X2.Y2.

X-2.

Y-2.

X2.

G67

G0G80Z5.

M05

G91G28Z0

M30

 

NOTE: If you are doing a single position you only have to use a G65 instead of a G66 with no G67 cancel and basically you are creating your own canned cycle by doing this.

[TerryT]

I'm no expert, but couldn't you just program G81 to whatever your 11/2 depth would be , then call your coolant on M28, then command your M3 to the new speed, then G81 to final depth with your new F rate.

[djstedman]

You could, but most likely that would be a hand edit and he mentioned earlier in the thread something about 400 holes. That just doesn't sound like fun to me.