keep me outta trouble

[mike thomas]

All, I am going to start the DeHaas Vault Lock 2 this weekend. The first step is to make the falling block hole. It is round, and of 1 inch diameter. The material is 4140 with a RC of 30. The hole is to be at an angle of 3-4* rearward. Using the Bridgeport, I plan to drill to 7/8, take out another .115 with the boring bar, and finish ream. The boring bar is carbide insert, the reamer is HSS. I was thinking of 220RPM for the bar, and 80RPM for the reamer with lots of cutting oil.
Where am I going to get into trouble? Do I need to mill a flat before starting a hole at this shallow angle? Thanks, Mike

[msrm]

How are holding the material? In a vise etc?
You need to have very very sturdy setup to
begin with. To ream a hole up to 1/2" drill
the hole 1/64 undersize. To ream a hole 1/2"
and larger drill the hole 1/32 undersize.
I'm not sure how you are going setup your
operation, but I really wouldn't use a boring
bar and boring head(?) at an angle. This
could get ugly quickly. I would set up your
material, mill a small flat for a center drill. Use a small (1/4") center cutting
endmill to start a hole. An endmill starts a
hole perpindicular to your horizontal plane
where a drill bit may walk. Mill down about
an inch switch to a VERY SHARP 1/4" drill bit(this creates a pilot hole for the larger
bits to follow)Do not use dull or semi sharp
cutting tools on 4140 it work hardens very quickly. The RPM is always touchy,when I
drill big holes in wierd directions I back
off if I feel any vibration. You might want
drill and ream another piece of 4140 to see
how it acts and to adjust your RPM. Also,
4140 is unforgiving if you go to slow.If you
have to bore the hole bore it about .969,
1.00-.031=.969 Be careful and good luck I
hope I've helped and not hindered

[mike thomas]

I was planning to clamp the work in a vise, and tilt the head on the mill 3*. I forgot to mention that I have to go down 2.5", and come out the bottom. Thanks for the tips, I will procrastinate for a bit and see what else is recommended, as I was already nervous about the bar and boring head. I was smart enough to get a practice block of the same material. Mike

[JCHannum]

Personally, I try to avoid ever moving the head of my mill once it has beem trammed in to the table. I would set the block at the 3-4* angle using an angle plate or shim. See the post about sine bar.

Keep in mind that de Haas built these actions with a 9 or 10" Atlas and drill press. Nothing exotic, just careful workmanship.

Also, check that angle, I believe it is toward the barrel. The dotted line on page 34 is perpendicular to the base of the breechblock.

[mike thomas]

De Haas had one big advantage over me. He knew what he was doing. I'm counting on you guys. I have only had the mill a couple of months, and have a darn sight to learn yet. Probably a good idea not to move the head.
I wanted to bore, as I will have to invest in new bits to drill this. I keep lots of new jobber lengths 1/2 and below around, but not the larger ones.
JC, is my terminology wrong? I know that the hole leans toward the barrel, but is there a standard way to refer to the direction of an angled hole. I'm not getting smart, this will bug me until I know if we are referencing from different directions, or whether I am missing something.
So, if I shim the one end, can I get by boring? Or do I get frisky and buy bits? Mike

[JCHannum]

Mike,
I don't know if there is standard terminology or not, I would refer to it the other way.
I just thought I'd mention it, as I usually do the first thing on a project like this bass-ackwards myself.
There is nothing wrong with boring, but, I would finish ream. The tricky part about boring is the interrupted cut at top & bottom. Use a stiff boring bar, and go easy until you are making a full cut & it should be ok. If it is not going to work, you will know pretty quick, and then you can buy a couple larger bits.

[Martin]

I don't know if this will help or hinder, but
instead of boring, why not just use a jig reamer ? A jig reamer will cut a straight hole even if the drilled hole is a little out.
Martin

[halfnut]

Hope you haven't got in trouble yet.

Rule of thumbs, drilled holes aren't round, straight, nor to size. Sometimes they are close, but don't depend on them.

To get a nice straight reamed hole, run a boring bar through drilled hole first. You've got the right idea.

The angle might throw reamer off, best if it was starting with flat surface. I'd bore to .005-.010 under reamer, measure well, reset boring head to finish size and bore just a bit until reamer has a nice spot to start.

If you have to drop table to run reamer, reindicate the hole in again to spindle.

Run reamer in low hole, lots of oil.

1/32 is a bit much to ream, I have reamed this much in big lathe, big chuck, big part set up nice and sturdy. Less to remove on finish ream is better.

[mike thomas]

No, I have not got into trouble yet. Probably only because while I was trying to mill this stuff square, I dulled my larger end mills. Gotta get more and better ones. I am seriously wondering how I am going to cut threads into this stuff. It is tough. I am doing three blocks, if I am lucky I will have more than one survivor.
I think that I have enough material in depth that I could set the blocks at an angle, mill a flat area for starting. Then, after finishing the holes, I could set the blocks level and mill square. I'll check on this while waiting for the end mills to arrive. Thanks guys, Mike

[msrm]

I said in the beginning of my reply that you will need "very very sturdy setup" to machine
at an angle. Good luck

[mike thomas]

msrm, You sure were right about the 4140 work hardening. When my hss end mill started to dull, that was it. The other hss mills would hardly scratch it, after it work hardened. I had a small carbide, and that worked. I ordered some carbide, perhaps that is overkill,and about 4 replacement bits for my S&D set. Plus one bit 31/32. Good thing money is no object. I can see that a good drill sharpener is going to be on this summers list of ebay purchases. Clamped down solid is a relative term. I do not have enough experience with the mill to know if I am solid enough, and would not know until something went south. Most recommended a Kurt vise, but when I came across a 6 inch Bridgeport vise in good shape, I bought it for $90. I figured it was better than import, but I really don't know. I would be so much more confortable doing this on the lathe and drill press, but this is a learning experience. Mike

[C. Tate]

If you don't want to bore the hole take a 1.0 emill have it sharpened so that it is a few thou under and plunge the .875 drilled hole. This will give a clean round hole ready for the ream. I would not turn the head of your mill if the angle is critical, the markings on the side of the Bridgeport are good for reference only not holding 1 deg. The angle blocks or a sine plate would be a much better solution.

[snorman]

4140 is terribly bad about hardening when you shoot a little oil on it and then try to drill etc. Best to just machine it dry imo. Usually no problems that way.

[msrm]

I always try to give myself just enough
clearance in the vise so my cutting tool doesn't cut into the vise or mill table.
If you feel uncomfortable about the whole
operation setup like normal, instead of using
the 4140 try nylon, derin, aluminum or some
thing a little more forgiving instead of
steel, so you can get the feel for the
operation and to get comfortable with the
large tooling. Good buy on the vise. I have
had good luck with my ENCO (Kurt Copy). The
second ENCO I bought wasn't as good but I was
able to grind the bed on the vise. I really
would like a Kurt especially the one with
work stop that comes with it. I use the
Kurts at work and their is a difference, but
I can't let a 400.00 vise just sit around in my own shop. The carbide should do well. I take shallow cuts and run coolant basically to save the cutting edges and to keep from snapping them off when cutting. Good Luck

[mike thomas]

The tools arrived from MSC today. Soon as I feel unstressed out from working, being a parent, etc. I will try it. I have spent the last couple of evenings reading Machinery's Handbook 25. I should have done this first. Interesting stuff this 4140. The book says to lube with sulfur oil when drilling, and reaming, but when milling or turning to use water soluable oil. I thought that I was getting smart when I reduced the amount of cut I was taking, but the book said that one must take a cut sufficient to keep the tool from burnishing the material, and thereby work hardening it. So the smarter I was getting, the more difficult I was making this.
I was standing by the lathe, thinking, huh, 4-jaw, 3/16 drill rod shim. But, I will master the mill. I am going to drill to 31/32, bore a few thou, and finish ream. There is not enough material excess on the blocks to mill a flat to bore and ream, but I feel much better about this now that I have a hint what I am doing. I will do the lubing and cooling as the book said. I might have to drink the water soluable, wait a couple of hours, and then stand on a milk box, as I don't have a pump. I pressurize a tank of water souluable to ream barrels, but this could get messy. Mike