Breaking Drills - Haas VF2 - .076 diameter

[Colin Gilchrist]

Ok, so admittedly it has been a little while since I've run a machine, but I've drilled thousands of holes in my life. I recently took on some R&D work for a company in Connecticut, and I'm running their VF2.

 

I'm thinking I either have a problem with run out, or I'm taking too deep a peck and packing the flutes with chips. So here are the specs:

 

.076 diameter drill (#48), .750 flute length, 1.25 Out of Holder

 

8000 RPM (I could go up to 10K, but I'm holding this drill in an Albright Drill Chuck. It is better than the worn out ER20 collets they have!)

 

Feed = 1.8 IPM, Peck Depth = .152 (2X Dia)

 

I'm drilling 22 holes, at .920 total depth per hole.

 

The only #48 drills in the shop that I could find were already used, but the cutting edges still looked OK, and I'm cutting 6061 AL. I figured for two parts, I'd just baby the drill through them and be done. The first drill only made it through 5 holes before I heard the crunch. (And to top it off, I was running at only 70% feed, 1.26 IPM.) The stock is 2" thick, and the flange finishes at .800 thick, hence me thinking I could just flip it over without interference.)

 

This part looks like a cone with a flange, so rather than spending time trying to extract the broken drill, I just deburred and flipped the block over. (The roughing on OP2 will take care of this, and I have some extra carbide endmills, so I'm not too worried about chipping a tooth on the leftover bit.)

 

So I'm on the 2nd attempt. I put in the only other #48 drill they had, and ran at 50% feed. This time I made it to hole 14 out of 22 before it broke. I thought that maybe I had not tightened the drill enough the first time around, so I put a spanner wrench on the chuck and added a couple foot pounds. I'm pretty careful about not over tightening threads. In fact, when I checked the broken drill the 2nd time, I was sure it had not pulled out.

 

The first drill had a TIR of .0004, and the 2nd drill had a TIR of .0003. I considered that better than the .0012 I was getting with their only 1-2 mm collet.

 

I thought that excessive runout was causing the breakage, but the more I think about it, the more I think that it could have been too deep a peck value, and I'm packing the flutes with chips.

 

So what do you guys think: Crappy drills? Too much run out? Too deep a peck?

 

I'm stopping by a tool supply company tomorrow morning to grab a pack of drills on my way into the shop. I'm going to try the same RPM, with a feed of 1.2 IPM, and a peck depth of .075. If I feel like getting fancy, I will probably also use the Peck Reduction cycle, and start with a peck of .15, and then have it reduce from there. (I still want to make the best cycle time I can. I don't want to be there all day just to drill 44 small diameter holes.)

 

Thanks for your advice and insight.

 

Best regards,

 

Colin

[JMahon]

I'd go with a smaller peck and higher feed

[Eric@HorsepowerInc.]

Colin couple things come to mind, used drill bits, but you got that covered in the a.m. The webs could have been off, those few tenths wouldn't be doing that, are the holes your doing straight and round? What are you spotting with? make sure the spot point is smaller than the drill web, in your case almost a point. Also, don't use a 90deg spot, go with a 140+ for the straightest holes, you want the point of the drill to touch first. If all else fails, I would blame it on the HAAS, we just dumped $6k i ours this week, junk I tell you, our Doosan's run circles round these. Ok, I'm done ranting, let us know how you make out.

[The Cathedral]

I'd go with a smaller peck, but the first thing I'd look at is coolant. That's a tiny-a$$ drill and it has nowhere to dissipate heat so once it gets warm, that aluminum starts galling, and snap! Are you deep-hole pecking (staying in the hole) or are you pulling all the way out on your peck?

[THEE THAINZ™]

At 1.26 IPM you'd have less than .0003" CPR. if your drill point was a little dull and your coolant was less than 6% you probably had a galling issue. If it was me I would go with a peck of .100 for depth and start at 3.8 IPM if the coolant mix looks good.

[Guest MTB Technical Services]

Peck is too deep and you're likely galling at the bottom of each peck.

 

Rule of thumb is 1/3 of diameter as a starting point.

 

Without a coolant thru holder, avoid G73 chipbreak cycles.

You don't get enough swarf clearance and the lack of coolant will causing galling.

Make sure you're using a G83 deep hole cycle.

 

Have you set the programmable coolant nozzle position in the offset table?

[MIL-TFP-41]

Peck is too deep and you're likely galling at the bottom of each peck.

 

Rule of thumb is 1/3 of diameter as a starting point.

 

Without a coolant thru holder, avoid G73 chipbreak cycles.

You don't get enough swarf clearance and the lack of coolant will causing galling.

Make sure you're using a G83 deep hole cycle.

 

Have you set the programmable coolant nozzle position in the offset table?

 

^^^^^

Agreed. 1/3 of your drill dia for a peck is a safe starting point.

Your feed is very light. Try 6 IPM @ 8000 RPM

[?Mark]

".076 diameter drill (#48), .750 flute length, 1.25 Out of Holder

 

I'm drilling 22 holes, at .920 total depth per hole."

 

 

 

 

 

Colin, isn't flute length too short?

 

Here are the numbers for this tool: S12822 F15.0 33% peck (scale speed and feed accordingly to your machine capability)

[Mic6]

For me, when drills get under Ø.09, I peck the diameter of the drill.  No issues, but it may take a few seconds longer.

[Machineguy]

ITs not the machine. I run one every day.

[Colin Gilchrist]

Hi Guys,

 

It was the peck depth. I used the Haas peck reduction cycle, and it worked great. 5 IPM, 8000 RPM. Starting peck was .075, and I set a peck reduction to .01 per peck, and a minimum peck value of .025. It is cutting right now and sounds sweet.

 

Plus, now I'm using a carbide drill. I found a tool supplier called All Start Tool Inc., that is right down the street from us. I would have been happy with HSS, but they only had carbide in stock. For $10 bucks, I'm not complaining. Especially since I could walk in and grab the tool off the shelf, and have it running in the machine 20 minutes later.

 

Thanks everyone for the advice. When I first started on this forum over 10 years ago, all I did was ask questions. Eventually that turned into me answering the questions, and I'm grateful that this place still exists when I get stuck.

[Colin Gilchrist]

".076 diameter drill (#48), .750 flute length, 1.25 Out of Holder

 

I'm drilling 22 holes, at .920 total depth per hole."

 

 

 

 

 

Colin, isn't flute length too short?

 

Here are the numbers for this tool: S12822 F15.0 33% peck (scale speed and feed accordingly to your machine capability)

 

Hi Mark,

 

Yes, the flute length is shorter than the hole I'm drilling. That is what the pecking is for, to make small chips and lift them out of the hole. Someone else asked if I was just doing a chip break cycle, but I'm doing a full retract, G83.

 

Unfortunately this place is on a tight budget. So for a lot of stuff, it is "use what we have got" and "make it work". It is frustrating at times, but such is the nature of R&D work.

 

If anyone is interested, our company is working on a new type of rotary engine technology.

 

www.liquidpiston.com

 

Cheers,

 

Colin

[matt m]

Do any of you program some dwell in your cycles..... I did this with X2 or something and it worked very well since then I haven't done it.

[Colin Gilchrist]

I used dwell on my spotting cycle. Actually, I'm using a small carbide center drill (#1?), since they don't have any NC spotting drills. No need to use a dwell on the peck reduction cycle, it worked beautifully, and these are thru holes.

[Sticky]

Glad you got it figured out, the carbide drill is going to make a big difference if you don't have enough flute length, hss drills will wander a lot more and be more prone to binding when you bury the flutes. I'd relieve that shank if you want some added reliability.

 

Seems a couple years ago I saw a job ad for a machining position at Liquid piston. Did they not find what they were looking for? In a company like that a good machinist would be quite valuable. I'd really like to see their stuff get off the ground.

[jeff]

From Guhring's website:

 

"Note: Pilot holes (depth >1xD) are recommended when using RT100T drills. Use a series 5514 or similar drill to drill
a minimum of 1xD deep. Then enter the pilot hole with the RT100T drill at approx 300 rev/min and 500 mm/min speed,
start high coolant pressure and increase RPM. Drill to hole depth without pecking."

 

What type of material are you drilling?

 

http://www.guhring.com/Documents/tech/speedfeed/6512.pdf

[Colin Gilchrist]

Glad you got it figured out, the carbide drill is going to make a big difference if you don't have enough flute length, hss drills will wander a lot more and be more prone to binding when you bury the flutes. I'd relieve that shank if you want some added reliability.

 

Seems a couple years ago I saw a job ad for a machining position at Liquid piston. Did they not find what they were looking for? In a company like that a good machinist would be quite valuable. I'd really like to see their stuff get off the ground.

 

Hi Sticky,

 

Yes, they have gone through a couple different guys in the shop. Most of them had great machinist skills, but didn't have the advanced programming skills needed to do everything these guys need done. I think they finally found the right guy (me, lol), but we'll see how it goes. I'm hoping I can show enough return on their investment in me to start getting some of the equipment we desperately need. Simple things like having enough collets and holders to mount up more than 5 drills/taps at a time, and getting some endmill holders that aren't just cheap side locks. We still have a ton of our parts made outside, because we can't hold the tolerance, or just don't have capacity...