# How to make my drill bits last longer



## StevenHansen849 (Jul 19, 2018)

So I'm not very knowledgeable when it comes to drilling into aluminum that is an 1.5 inches thick but I would think you would want to make a starter hole so your bits would last longer. Is this the case?

The whole story is, I work at a company that has a robot drilling a 16mm by 38mm thick. After about two week the bit starts to gum up and wonders. These holes can only about .5mm off the correct spot and when those drills wonder the holes end up being around 1-2mm off. I understand that the bits will lose there edge and because of the heat the aluminum shavings will "weld" to the hardened steel, but if you guys know a way to make the bits last even a couple days more that would be wonderful.

Thank you and I look forward to your replies.


----------



## shooter123456 (Jul 19, 2018)

Are you using any kind of lubrication for the drill? 

Does the machine start with a smaller drill and work up?

Do you sharpen the drills?

What kind of speeds and feeds is the robot using?

Also, what kind of aluminum?

Is it peck drilling or just going straight down?

Answers to these questions will help us give you a better answer.


----------



## cvairwerks (Jul 19, 2018)

Steven: Make sure you are using quality bits, correct speeds and feeds with coolant. You may need to do some pecking too.


----------



## benmychree (Jul 19, 2018)

Is a cutting fluid being used?  Is the drill being regularly sharpened?  Is a spotting drill used before the twist drill?


----------



## JimDawson (Jul 19, 2018)

Normally I would use peck drilling with a full retract, flood coolant.  Through-tool coolant would be better if available.  135° split point, cobalt, stub drill would be my first choice, or maybe a 3 or 4 flute solid carbide bit if the machine spindle speed will support that.


----------



## P. Waller (Jul 19, 2018)

We just ran 5000 aluminum parts with five 1/2" holes in each part in a Haas TM1, flood coolant, 4000 Rpms, .100" peck.

It took 1 OSG carbide SM drill which would probably drill another 25000 holes, use uncoated carbide.


----------



## RJSakowski (Jul 19, 2018)

An anodized surface will quickly dull a HHS drill.  Even carbide is softer than anodizing.  The aluminum oxide that makes up the coating is second only to diamond in hardness.


----------



## shooter123456 (Jul 19, 2018)

RJSakowski said:


> An anodized surface will quickly dull a HHS drill.  Even carbide is softer than anodizing.  The aluminum oxide that makes up the coating is second only to diamond in hardness.



Is the coating thick enough to make a difference when drilling?


----------



## StevenHansen849 (Jul 19, 2018)

shooter123456 said:


> Are you using any kind of lubrication for the drill?
> 
> Does the machine start with a smaller drill and work up?
> 
> ...


----------



## markba633csi (Jul 19, 2018)

Lubrication or cutting fluid?  Coated drills?


----------



## StevenHansen849 (Jul 19, 2018)

benmychree said:


> Is a cutting fluid being used?  Is the drill being regularly sharpened?  Is a spotting drill used before the twist drill?




So are using cutting fluid but the robot makes it a mist so we have a lot of extra fluid being used. We have only been sharpening them once they start to wonder. And there is no starting hole, step bits, or spotting drilling going on the robot just grabs the 16mm bit, turns on the lube mist, and drills (which makes a "lovely" squealing sound on the metal).


----------



## RJSakowski (Jul 19, 2018)

shooter123456 said:


> Is the coating thick enough to make a difference when drilling?


IMO, any thickness will cause wear.  Hard coated anodizing is much worse but even decorative anodizing is abrasive.  
I usually make it a practice to strip anodizing from a surface before machining.   When I do machine an anodized surface, I try to work it so the tool makes contact on exit.  Anodizing is brittle and will shatter.
The oxide coating on HR steel os also hard on tooling.  I will band saw out of necessity but before subjecting an expensive milling cutter to it, I will remove the oxide coating.


----------



## GoceKU (Jul 19, 2018)

Try using a Guhring HSCO drill bit they are carbide drill and last for ever also they are sharpen by laser, i've had great success with them.


----------



## shooter123456 (Jul 19, 2018)

What kind of robot is doing this drilling?  You mentioned the bits only work for about 2 weeks, how many holes are drilled in 2 weeks?  Roughly how long does the robot take to drill each hole?

Unfortunately, if you are plunging and using mist, the coolant is never going to get to the cutting face where it is needed.  It will just be spraying onto the chips that are already in the drills flutes.  To get the lubricant where it is needed, it needs to either retract or you need through spindle coolant.

When you sharpen them, how is that being done?  If they are just sharpened by hand and aren't done well, that will contribute to the drill walking while it cuts.  

I have found cast aluminum to be particularly gummy and prone to packing into the drill when I am drilling.  With something like extruded 6061, I can usually get to 2 or 3x diameter with the drill before the chips stop escaping before it retracts.  With cast, it tends to get stuck almost immediately and gets knocked loose from the drill bit once it goes back in after the retract. 

There are some things you could try which might help.  I am not sure how practical they will be for your application, but nonetheless:
1. Try to peck drill instead of through drilling.  This will let it clear the chips and get some lubricant to the cutting surface.
2. If the robot can do it, try using an end mill to interpolate the circle instead of drill.
3. You could drill a little bit under the diameter needed then switch to a boring head and bore it.  It will be straighter, rounder, and you won't need to worry about the drill walking.
4. Make sure you are using the right drill bits.  This sounds like an industrial application, so weigh the cost of better gear against the time it takes to drill the holes, sharpen, change out the bits, replace them, etc.  
5. Make sure you are using a proper lubricant for the drill.  When I drill cast, WD40 does a much better job than any of the oils I have tried. Something specifically for aluminum might make sense for your application.
6. Make sure feeds and speeds are on.  If it is squeeling and the hole is all chattery, the drill bit is going to wear out faster.  Ideally there should be no squeeling.  If your RPMs are too high and feed to slow, the bit will wear out faster.

It is hard to give really good specific answers without knowing a lot more details, but just using torque to force a drill bit through is really the worst case scenario.


----------



## Smithdoor (Jul 19, 2018)

I have had 9/16" last over years on very day use. We sharpen drill bit down to 1/8" and 9/16" we would down 1/2" of flute
Dave


----------



## dbq49 (Jul 19, 2018)

Who does laser sharpening??


----------



## StevenHansen849 (Jul 19, 2018)

shooter123456 said:


> What kind of robot is doing this drilling?  You mentioned the bits only work for about 2 weeks, how many holes are drilled in 2 weeks?  Roughly how long does the robot take to drill each hole?
> 
> Unfortunately, if you are plunging and using mist, the coolant is never going to get to the cutting face where it is needed.  It will just be spraying onto the chips that are already in the drills flutes.  To get the lubricant where it is needed, it needs to either retract or you need through spindle coolant.
> 
> ...




We are using a Fanuc M10iA robot that has a drill mount. I'm not to sure how they sharpen them but I think we send it back to our drill supplier and they sharpen them for us. And it takes roughly 4-5 min to get each hole done.
I'll see if I can change the code a bit so the robot sprays some lubricant, then start drill for 30 seconds, stop drill, spray lubricant, then repeat until the hole is done and see that makes a difference. And I'll have to ask about the boring bit, we might be able to switch the bit to a 15.75mm or a 15.5mm then bore the rest of the diameter. 

Thank you for the tips, I'll keep you posted on what works and doesn't. If any of you have any other suggestions that would be great.

Steven Hansen


----------



## P. Waller (Jul 19, 2018)

That is a big hole to drill with such a small arm. Fanuc literature lists it as a 12 Kg (27 Lb) payload machine, I am unsurprised that you are having problems.

http://www.flexibleautomationsupply...MIuevxk5us3AIVmISzCh36jQ_MEAAYASAAEgIVUfD_BwE


----------



## markba633csi (Jul 19, 2018)

"I'll see if I can change the code a bit so the robot sprays some lubricant, then start drill for 30 seconds, stop drill, spray lubricant, then repeat until the hole is done and see that makes a difference. And I'll have to ask about the boring bit, we might be able to switch the bit to a 15.75mm or a 15.5mm then bore the rest of the diameter."
I think that will make a big improvement- the squealing is telling you something is not quite right- pay attention to that
Mark


----------



## Smithdoor (Jul 19, 2018)

I use a 6" bench grinder 

Dave 





dbq49 said:


> Who does laser sharpening??



Sent from my SAMSUNG-SM-J320A using Tapatalk


----------



## brino (Jul 19, 2018)

@StevenHansen849 

Looks like you have plenty of great feedback above.
I just stopped by to say two things.....

1) Welcome to the Hobby-Machinist!

2) Please do update us with what works and does not work in your situation.

-brino


----------



## P. Waller (Jul 19, 2018)

Smithdoor said:


> I use a 6" bench grinder
> 
> Dave


Elegant solution.


----------



## StevenHansen849 (Jul 20, 2018)

P. Waller said:


> That is a big hole to drill with such a small arm. Fanuc literature lists it as a 12 Kg (27 Lb) payload machine, I am unsurprised that you are having problems.
> 
> http://www.flexibleautomationsupply...MIuevxk5us3AIVmISzCh36jQ_MEAAYASAAEgIVUfD_BwE



Okay so I got some better information because I checked it myself instead of hear from someone else. The robot we are using is a Fanuc R-2000iA/165F with a Hiteco QD-1F 4/12 63F NC CB Electrospindle Powertech 200 series 4 kw. We are drilling through 3/8" extruded aluminum (I am not a materials guy so I don't know if that's a thing, but I was told it was like casted). The 16mm bit is a Fullerton's solid carbide 1565 series AlumaDrill and we are spinning it at 3500 RPMs. We have tried going slower but from what I'm told the bit didn't have enough torque to go through the aluminum. The guy who coded the robot has tried peck drilling before and it didn't work (I'll have to get back to you on the detail on why it didn't work because that guy is on vacation till Monday). 

The major issue is when the bit tarts to drill it cause the whole part to vibrate, we hooked up four hydraulic clamps to robots so when he process starts the clamps engage and stop the frame from moving vertically and horizontally but the part still shacks and squeels (worst than when you try to ride a pig lol). We have thought about putting more clamps but the issue with that is we ran out inputs on the bot so the clamps would have to manual. If any of you got something for to try that would be wonderful.


----------



## JimDawson (Jul 20, 2018)

Wow!  I didn't even know that was possible to drill with a robot, the fact that it works at all is impressive.  The only thing I can suggest is to try reducing the feed rate along with reducing the RPM.  There is normally a sweet spot that works.

For those who don't know what a Fanuc R-2000iA/165F is ( I had to do a Google search   ):


----------



## rowbare (Jul 20, 2018)

StevenHansen849 said:


> And it takes roughly 4-5 min to get each hole done.



Sounds to me like you are trying to rub a hole through the part. I put the initial hole diameter 19mm into a  feed and speed calculator (https://fswizard.com/) and got  50 ipm @ 2300 rpm, that means your 38 mm hole should be drilled in about 2 or 3 seconds.

Now with the information from your latest post, 16mm, carbide bit the calculator comes up with 132 ipm 6200 rpm. Drilling 3/8 deep, that should take less than a second per hole.

WIth a 4KW spindle you certainly aren't low on power even if it's running well below its rated speed. Based on your description, your problem isn't with the spinney bits, it is a work holding issue. You can't drill a hole if you can't resist the cutting force.

You need to work on how your material is fixtured. If you can post a few pictures, I am sure someone will be able to suggest some improvements.

bob


----------



## P. Waller (Jul 20, 2018)

One of the best uses of an arm that I have ever seen, making something new look old, brilliant.


----------



## StevenHansen849 (Jul 23, 2018)

So this our set up, the first and third images are the drill bit we are using and the last to images are what we are drilling. the bit is sticking out 100.5 mm and its 150 mm long. The guy who programmed the robot told me that he was going to try using a end mill to drill through 3/8 aluminum or we can try drilling a 9.5 mm hole then stepping up to a 16 mm hole. What do you guys think? Would that work?


----------



## JimDawson (Jul 23, 2018)

Normally trying to drill with an endmill ends badly if the setup is not absolutely rigid.  The endmill puts a lot of asymmetrical radial load on the system as it plunges in.  Hanging on the end of a robot arm would be just about the worst case setup.  If you can create a helix tool path then it may work OK.  If you can create a helix plunge tool path, then use a 5/16 endmill, and interpolate the holes to size.

Given the application, I guess I might spot the holes with a spotting drill in the robot arm, then just hand drill the holes to finished size.  As an alternative to hand drilling, a drill press would be a good option.

The other option would be to pre-drill the holes in the brackets, then fixture them properly to do the weldments.  I really think you need to look at the overall process.  Drilling the holes on a drill press or small milling machine should take less than a minute.


----------



## StevenHansen849 (Jul 23, 2018)

JimDawson said:


> Normally trying to drill with an endmill ends badly if the setup is not absolutely rigid.  The endmill puts a lot of asymmetrical radial load on the system as it plunges in.  Hanging on the end of a robot arm would be just about the worst case setup.  If you can create a helix tool path then it may work OK.  If you can create a helix plunge tool path, then use a 5/16 endmill, and interpolate the holes to size.
> 
> Given the application, I guess I might spot the holes with a spotting drill in the robot arm, then just hand drill the holes to finished size.  As an alternative to hand drilling, a drill press would be a good option.
> 
> The other option would be to pre-drill the holes in the brackets, then fixture them properly to do the weldments.  I really think you need to look at the overall process.  Drilling the holes on a drill press or small milling machine should take less than a minute.



I agree with the end mill, I 've used one to drill before and it always wonders. The problem with drilling the hole before we weld the part on the whole frame is we hand weld those pieces to the frame. If one of the holes are off we won't be able to put the box together. And when it comes to the whole hand drilling or using a drill press we are trying to get away from using people so we can produce 15 boxes a day instead of 7. 

Another thing we haven't tried is we could change the mist lube to flood coolant and make a big tray to catch the excess coolant, if you guy think it would be worth we could try it.


----------



## JimDawson (Jul 23, 2018)

I don't think flood coolant would be a big help here, but getting the coolant nozzle closer to the work area might be helpful.  I use kerosene in my mist coolant system for aluminum, applied at about 1/2 cup/hour.  There is some fire danger but it's minimal, may not be appropriate in your enviroment.  Peck drilling with a full retract would be helpful.

Does the robot have a tool changer on it?  How many holes need to be drilled per unit?


----------



## StevenHansen849 (Jul 23, 2018)

JimDawson said:


> Does the robot have a tool changer on it?  How many holes need to be drilled per unit?



Yes it has a rack 6 slots for drill bit chucks, slots 1-4 are filled but we are only using the one in slot 4 because we couldn't program the robot just right for the other 200 holes. And we are currently only drilling 8 holes per unit and that's all the 16mm bit will ever do.


----------



## JimDawson (Jul 23, 2018)

That being the case, I would add 2 more drills.  A spotting drill, and a pilot drill (maybe 6mm or so).  I would use a 17mm spotting drill with a 150° point.  That will also put a nice chamfer on the hole edge.  Even with the tool changes it should speed up the operation.


----------



## Downunder Bob (Jul 23, 2018)

The best way to make any cutting tool last longer is reduce the cutting speed FPM, 10 to 20% should be more than enough to considerably increase tool life. Also make sure you DOC and feed are appropriate, not too high, nor too low. Aim for the middle of the recommended range. Machine rigidity is also a consideration. And don't forget the correct cutting fluid for job, will always extend tool life.


----------



## StevenHansen849 (Jul 23, 2018)

JimDawson said:


> That being the case, I would add 2 more drills.  A spotting drill, and a pilot drill (maybe 6mm or so).  I would use a 17mm spotting drill with a 150° point.  That will also put a nice chamfer on the hole edge.  Even with the tool changes it should speed up the operation.



The largest diameter we can go is 16.025mm and the smallest is 15.88mm, so we can go that big but I can see if I can find a 16mm with a 150° point, and to @Downunder Bob point I'll be talking to Hiteco to see how they calculate the RPMs so we can get it just right.


----------



## JimDawson (Jul 23, 2018)

The tool holder appears to take a standard ER32 collet, available from 1 to 21 mm.  You should be able to use any drill bit in that range, you only need the correct collet.


----------



## StevenHansen849 (Jul 23, 2018)

No I mean the holes in the boxes can't be over 16.025mm and under 15.88mm, we can cut the hole anyway we like, but the customer wants the holes to be that size.


----------



## JimDawson (Jul 23, 2018)

StevenHansen849 said:


> No I mean the holes in the boxes can't be over 16.025mm and under 15.88mm, we can cut the hole anyway we like, but the customer wants the holes to be that size.


I wasn't suggesting that you drill the hole oversize, just hit it with a spotting drill to create an on-center starting point.  If you use a 17mm spotting drill, that would just debur the top of the hole with a narrow chamfer, 0.5mm max width, depending on how deep you go.  The other drill bit you might try would be a 16mm, 135° split point, cobalt,  stub drill.  I use those all the time in aluminum (and most other materials).  You might look at a CXDSS 1600AP drill bit from M.A. Ford also.


----------



## Silverbullet (Jul 24, 2018)

Would an annular type coring drill work , I think they come in carbide also ..   They sure cut good for me and some have a spring loaded plug pusher . It's like a hole saw on steroids .


----------



## BGHansen (Jul 27, 2018)

Looks like you're trying to drill a 16 mm hole through 3/8" thick aluminum on the TIG-welded on bracket.  That bracket is kind of hanging out there in space with no support on the bottom side.  I'm thinking you will need to support the tab from below if you are going to drill the 16 mm hole in one shot.  Or try a smaller pilot drill that goes through without flexing the welded on bracket, then go for the 16 mm drill.

Bruce


----------



## Winegrower (Jul 27, 2018)

There must be an experienced machinist left in Lansing...I would guess seeing your setup he/she could diagnose it fast, rather than deal with a bunch of our guesses.   Just saying.


----------

