How long to drill / bore these holes ???

I have 4 hot roll plates 1 1/2" thick x 6" wide x 24" long. I had to drill and bore a 2 1/8" hole centered and held 21" from one end.

I used a Bridgeport mill, center drilled the hole, drilled a 1/2" pilot through to relieve the center and then followed with a 2" drill. I then finished each hole with 2 passes using a boring head to get me out to 2 1/8".

Altogether, it took me 3 1/2 hours to load, drill, bore and deburr, and I was hustling. Does that sound right ???




Frank



www.randolphmach.com

Time for an operation will vary dependng on the materials, tooling available, and machine - and the tolerance you were holding - and the phone calls and other interruptions.

A Bridgeport is not a stock remover. An 11 ft arm Carlton radial arm drill would drill that hole from the solid in a couple of minutes about 5 minutes floor to floor in simple work like that allowing time to deburr the hole.

I'm the world's worst estmator but I'd say once you get rollng you could drill and bore each hole on a BP in less than an hour. Much less if you used an annular cutter.

http://cgi.ebay.com/Champion-RotoBr...emQQptZLH_DefaultDomain_0?hash=item20ae9e2ea9

With the equipment you have it sounds good to me Frank.

I'm in a simiar position machine wise and would have quoted an hour each.

Did a quick calc, there's 21cu in + of steel to come out of the 4 holes.

I just wanted to get a general idea if I was in the ballpark, as this is a time and material job and I want to be fair to the customer. To be honest, when I first looked at the job, I didn't think it would take that long ....... but I didn't realize the time drilling would take.

Yes, a radial drill press would be great to have, but I really don't punch too many large holes this size enough to justify the cost or floorspace.




Frank


www.randolphmach.com

Just took a minute or 2 to program that up, how I would run it. Running at a decent, but conservative clip with a 1/2" endmill. 1 minute 23 seconds each. Add another minute or two if it needs to be cleaned up with a boring head.

Just looked to make sure I'm not crazy, we do a part quite often, 1.875" hole, through 1.5" A36, 1min 21 seconds.

This is not a high end machine.

OK Bob, and I'm not picking a fight here ;- what would your total time be for the 4 parts, right from moving the parts, programme & set up through to out the door & clean up?

Sure, but like Forrest said, it matters greatly what machinery you have. Any 7.5 HP CNC can blow this hole out in no time flat, as could a big radial. OP has neither of these, just what seems to be a manual BP. How was it moving that 2" drill? I'm a bit surprised you got away with that.

What was the spec on hole location, size, and finish? Within a 1/16", or within .002"? If it's a tight spec, and constrained to manual machinery, I'd quote 50-60 minutes. If it's loose, 20 minutes. That's per hole.

Regards.

Finegrain

Limy Sami said:

OK Bob, and I'm not picking a fight here ;- what would your total time be for the 4 parts, right from moving the parts, programme & set up through to out the door & clean up?

Click to expand...

Yeah that is just the run time.

So lets say they have the material delivered, that means I have to open the gate, pray to something the forklift will start, or unload it by hand, snip off the bands, get it near the machines, thats worth 20 minutes right there.

Now, I need to figure out how to hold it, odds are I have a machine that is set with a series of vises that will hold that easily, so figure 15 minutes there.

Program time, already done, figure 5 minutes since I have to check my e-mail and have a smoke.

Setting the tool(s) and the zero's, another 10 minutes. Up to almost an hour now.

Run time, figure 20 minutes with load and unload, deburr and inspect.

If I have to deliver it or pack it to ship it, add another 1/2 hour.

If I actually have to do paperwork, formal PO, Certificate of Conformance, invoice, inspection log, add in another 20 minutes.

So, 2 hours for about 6 minutes of actual spindle up time, add in another hour if its a tight tolerance hole that I actually have to use a boring head and give some care to measuring it, actually at that point, I'm pricing in replacement cost of a piece of material.

Add in the fact that your customer can't do it themselves, and I'm sure they called you on the phone more than once, and nobody seems to pay me for quoting, even though that takes time.

3+ hours of billable time is not unreasonable.

Thanks Bob, IMO it's always the unproductive time that's a killer,...... but seems we're not that far apart.

Finegrain said:

How was it moving that 2" drill? I'm a bit surprised you got away with that.

Click to expand...

Actually, I have a 2" screw machine length drill that I use regularly on my turret lathe, which has a 1 1/2" shank .......... so I turned up an adapter with a 3/4" shank and held that in a collet. I used 1/2-13 set screws in the adapter and made small delrin pads for the screws to bind on, so if it slipped inside the adapter it would minimize damage to both the drill and adapter.

I did have the drill slip once or twice because I was pushing the drill too hard, but it slipped in the adapter as I had hoped and there was no damage. It worked very well, actually.



Frank


www.randolphmach.com

rockfish said:

Actually, I have a 2" screw machine length drill that I use regularly on my turret lathe, which has a 1 1/2" shank .......... so I turned up an adapter with a 3/4" shank and held that in a collet.

Click to expand...

Haha. We have something similar, just made in a little more git-r-done style. We came upon a big ~2" 45 degree chamfer end mill with 1 1/2" shank that we could never use in any of our machines. We also happened to have a bunch of extra 1 1/4" drills with MT taper built-in the shank. So cut the drill off at the end of the shank, lined the shank up with the shank of the end mill using the lathe and dead center, and brought the TIG torch over. It's proved to be an amazing metal removal tool when large diameter holes are needed for things like bearing bores. Removing all that material with a boring bar would take forever, now the initial chunk goes much quicker.

Those who have had a big radial around know this is a fast money job.


Locate 2 1/8" #4 MT taper drill in shop 0.5hrs. Mount vise on table 0.2hrs. Holes are almost exactly 1.19 min ea at 90rpm and .014/rev feed, which is babying the machine. Could probably push them to 140rpm and .020/rev, if in a hurry and have the holes done in 30 seconds apiece, but you'll have to use a little Tapmagic (add .001hrs for material). That's with our little 5ft arm 9"column 5hp G&L radial, a toy compared to Forrest's 11ft Carton with probably 40hp on tap.

Yeah, I'd charge them an hour a pop for the annoyance, but look what we have in the machine... no overhead.

I had a friend with a job of drilling 2-3/8" diameter holes through A-6 tool steel plates, 3.18" thick. He had been doing much the same as the OP with a HSS drill then multiple passes with a boring head on his Milltronics CNC mill. It tool him just about 37 minutes per hole to complete, over 9 minutes just for the drill.

I gave him my Valenite 1.5" cutting diameter (1-1/4" striaght shank) 3-insert V556 high feed mill. His machine maxed out @ 200 ipm feedrate, though the cutter was capable of 275ipm in that application. Using a helical toolpath with a .035" depth per pass, the hole was done in just over 1.5 minutes. No pilot drill needed either.

If you had a CNC mill capable of helical milling and able to take that 1-1/2" plate, I imagine the "hole job" could've been done PDQ!