Cost effective Drilling ??? Most bang for the buck.

A short history of our shop we have been in business for over 40 years we have tested and used multiple different drills and or drill bodies and tips. Everything from solid carbide to allied spade drills and iscars sumocham drills. After reviewing our budget for the last year we have discovered that we spend a Semi truck load of money on drills and drill tips/bodies. Does anyone have any pointers on what the best drills or drill bodies to use? Long story short we wanna drill the most holes we can, for the least amount of money. Any suggestions would be greatly appreciated.

Bring the vendors in and let them compete. They'll happily supply some drills trying to prove theirs is best and you get the data to find out actually who is best.

What I've found so far, 1 look really hard(pun I know) at the material,
As above speed, feed, coolant , going through lots of tooling on anything tells you somthing is wrong, we used loads of tips on face mills, sandvick, we got Walter in to look at it (sandvick were quite happy as we spent loads on tips), first thing Walter said was the feed and speed were a fraction of what was needed, they were correct.
Tip usage drastically reduced using real heavy feed and increased speed.
Someone then got the job of optimising cutting on each process, really looking at each process, cu feet removed, time, temperature, coolant,
We got a more expensive coolant, saved money, counter intuitive I suppose.
Changed the material on a few jobs, we used excessively hard, tough, more than needed really but costly.
Couple of parts actually got heat treated before some machining and hard machined to save, how mad is that.
Mark

How important - what do you value time as. Purely on consumable costs alone its hard to beat Hss cobalt drill bits used correctly and reground as needed they will drill thousands of feet of hole before getting too worn - too short. Time wise its slowest though and that then has its own costs.

A lot of the tips can be reground in things like spade drills and re-coated, may not be viable on smaller sizes but can be on larger ones, but you have to stop before they have major edge fail for this to pay off. Depending on machine some of this can be programmed into tool life controls so the cnc monitors it its self.

Equally if your going through a lot of bodies, your probably not changing the inserts soon enough or are off on feeds and speeds. The big killer of inserted drill bodies is poor insert life management. You need to dial things in well enough to change them before they fail catastrophically. Getting another couple of cents of hole drilled out of a insert life does not save bugger all when it costs you a $100 body!

If you're going thru a ton of drills or drilling inserts (I assume this is on a cnc mill). The very first thing I'd look at is the runout. Do you have good holders? Good collets? Good coolant thru pressure?
Then I'd look to see if you're running at the correct speeds and feeds for the material you're cutting, provided you are using the correct drill for the job.
If all of the above is on par, the drill will last a long, long time.

Mtndew said:

If you're going thru a ton of drills or drilling inserts (I assume this is on a cnc mill). The very first thing I'd look at is the runout. Do you have good holders? Good collets? Good coolant thru pressure?
Then I'd look to see if you're running at the correct speeds and feeds for the material you're cutting, provided you are using the correct drill for the job.
If all of the above is on par, the drill will last a long, long time.

Click to expand...

We use 1000 psi through spindle coolant on all of our machines. They are all CNC mills. I could be wrong on what we are spending for the amount of work we have done it just seems like a whole lot of money was used on drilling. With all this being said we mainly use Iscar sumocham bodies which run at a ridiculously fast speed and feed. Most steels start in the 250-400 sfm range and chip loads vary buy size but usually are between .005 - .014 ipr mind you at 350sfm .007 ipr is darn near punching the hole in the metal. I believe I'm gonna have to do some more in depth research. To see if the problem is over spending in drilling or if we actually drilled that many holes. Thanks for the input fellas.

At thoes speeds - feeds, worn tip to no tip happens fast, hence better tool life management may end up saving you some tool body costs.

heavenlykid said:

We use 1000 psi through spindle coolant on all of our machines. They are all CNC mills. I could be wrong on what we are spending for the amount of work we have done it just seems like a whole lot of money was used on drilling. With all this being said we mainly use Iscar sumocham bodies which run at a ridiculously fast speed and feed. Most steels start in the 250-400 sfm range and chip loads vary buy size but usually are between .005 - .014 ipr mind you at 350sfm .007 ipr is darn near punching the hole in the metal. I believe I'm gonna have to do some more in depth research. To see if the problem is over spending in drilling or if we actually drilled that many holes. Thanks for the input fellas.

Click to expand...

.
.
1) what is part cost ? if expensive parts where a damaged or broken drill causes 10 hours or more of rework i would factor that in. i have spent over 10 hours using a edm tap burner to get a drill broke off 6" deep into a part before. saving 30 seconds drilling and then spending 10 hours getting drill out was not worth saving the 30 seconds
.
2) short and long length drills i run at different feeds and speeds. long length drills break 10x more if pushed like short drills. many a long drill you can often see it bending from high feed then bend starts rotating and it breaks in seconds
.
3) how are drills failing ? normal wear or sudden tool failures. obviously what you drill has a effect. metal with hard spots or slag in it can easily use 10x more tooling cause you are drilling harder and or more abrasive material.
.
4) speeds and feeds going faster til sudden tool failure occur is common then backing off a bit. of course sometimes you do 10 parts ok then get bad metal with hard spots and the next 10 parts have multiple tool failures.
.
5) i have had long length drill break multiple times cause pilot drill 4" deep was .001" smaller in dia. some drill bits make bad reamers
.
6) i have seen spade drills where tip insert screws were falling out and or just breaking. when i reduced feed it stopped happening.
.
7) drills breaking through other side is hard on drill bits especially at high feed. just saying when manually drilling most reduce feed when they are close to breaking through other side.

heavenlykid said:

Most steels start in the 250-400 sfm range and chip loads vary buy size but usually are between .005 - .014 ipr

Click to expand...

That sounds about right. We run a lot of 4150pht and similar steels and I program my solid carbide drills usually within those parameters.

Just to be sure... you're NOT pecking,right? That will wreck a carbide drill fast.

Mtndew said:

That sounds about right. We run a lot of 4150pht and similar steels and I program my solid carbide drills usually within those parameters.

Just to be sure... you're NOT pecking,right? That will wreck a carbide drill fast.

Click to expand...

.
important factors
.
1) length of drill. carbide doesnt like to bend
.
2) dia of drill. bigger drills can take more ipt or ipr feed
.
3) shallow hole or drilling through part
.
4) depth of hole and problems with chips and coolant cause of depth
.
5) material drilled. if it good steel or full of hard spots or slag. that alone can make drilling 10x more difficult and make feeds and speeds that worked before start having massive problems
.
6) cost of drill. for some places they still use hss twist drills cause they can be resharpened many times. some bosses would be upset using a $20. drill tip insert thats only good for 60 minutes. sure some can be resharpened but usually not by hand. some places still resharpen by hand

Forget the drills and drilling techniques for now!

Turn the problem round and look at cycle time / throughput / tool life / tool costs for the best matches of Return on Investment and Number of Jobs Out of the Door. Should give you some ideas about where you can make serious improvements and where its worth spending money. All these things go in plateaus where there is a fairly wide range of performance for a particular technology with little change in cost. Generally you want to be operating close to the bottom of the next step up.

Focusing on technique and technology alone its easy to end up spending out to get to the top of the next step and perhaps a bit along the plateau but not be able to get right along to the bottom of the next step without spending shedloads of money on other upgrades.

May well do much better by stepping back a bit from the bleeding edge with drilling but putting equivalent effort into other aspects of the business. Need to keep the business balanced by knowing how much of a change is required to feed useful though to the bottom line.

Clive

adama said:

At those speeds - feeds, worn tip to no tip happens fast, hence better tool life management may end up saving you some tool body costs.

Click to expand...

Really? Those are not high Drill sfp numbers for steel in my shop and I am not running TSC.

nothing worse than somebody bragging about saving 30 seconds a hole drilling and by end of year they spends a extra $2000. in drills and spent 20 hours ($2000) reworking or remaking parts
.
so at end of year drilling at max sfpm and feeds saves 4 hours or $400. but costing $4000 in extra tooling and rework costs (20 hours extra).
.
just saying if you record in a work log extra time to finish jobs including rework and sudden tool failure costs you might find it faster and cheaper to go slower
.
carbide drills are expensive. you can easily break $2000 in carbide drills in one day if not careful

To the OP.

Most answers were right .. but imho as a business-oriented guy, not comprehensive.
Anyone drilling with TSC and thus presumably modern, +/-, machine tools should get at least decent tool life.

What size holes, what material, how many/minute, how many/deep/fast, what machine, what are you aiming for ?
What is the desired accuracy ?
TIR, size, cylindricity, etc.

350 sfm with an indexable drill is not really high-performance. I was quoting some Walter indexable drills for a customer, and we're planning on running over 400sfm in 47hrc material...

Low carbon steels, you should be near 700sfm, and up to 38hrc or so, you should be able to achieve 500-550sfm. I know that Seco's Perfomax drill will do it. I would also consider the Sandvik 800 or Walter indexable drill as well. But a few years ago at the last shop I worked in, the Seco Perfomax was the one left standing after a 10-way shootout or so...

In a job shop, you may not notice the performance between brand X and brand Y drills. In a production shop, it's easier to see.


In our case (past shop) a 2" Seco drill at 500sfm in a 38hrc material, we could drill (80) holes 3" deep, per edge of the insert. That's 240 inches, or 20 feet deep, on one edge. X 4 edges, so 80-feet deep on a single insert. The inner inserts would last about 2:1 compared to the outer. You're going to be hard pressed to find a lower cost-per-hole than that.

-----------

Edit: - I juse realized that you mentioned you were using Allied & Iscar replaceable tip drills. Those are good options for replaceable tip drills. If you're after lowest cost-per-hole though, you need to look into indexables. There is simply no comparison on a cost-per-hole basis.