Boring Advice

[rcazwillis]

I need to bore a 3/4" hole 5/8" deep in 1018 1" round bar X 7/8". The bottom of the hole needs to be flat. I need to make 18 or so of these. I have a 7" lathe, large drill press, and a cnc mill. What is the most efficient method to cut this hole? I look at counterbores, but not sure what will work. I cut the first 12 using drills and the lathe. Then squared up the bottom. This took awhile and I would like a quicker method. Purchasing additional tooling is OK. Suggestions?

[miljnor]

I have lots of stuff I could bore you to death with!

but you said CNC mill and not on anything else so my vote is a cnc mill with an standard bottom cutting end mill. and hold the piece in a three jaw. If you have a toolchanger then drill it first otherwise circular interpolate and finish at depth! walla! flat bottom hole with automation.

of course lathes were made for these roundish kinda parts. But you said CNC and I am naturally lazy so the mill wins.

[Ken_Shea]

rcazwillis,
There is not much of a better way of removing material then drilling. What you are describing can be done entirely on the lathe with out using the drill press. Once the hole is drilled as large as possible and to depth, then I would get a boring bar and finish the remainder. Boring bars will square off the bottom. A CNC mill might be quicker, but for 18 it is doubtful considering the programming and some form of fixture would need to be made first so as to not require the indicating of each piece. For 18 it would likely be quicker just to do them manually. If a precise hole is required then boring is really the only sure way, checking the dimensions as you go, although it is possible to come very close using most CNC mills.
Ken

[dertsap]

cnc mill , chuck it , depending on the tolerance i would relieve the flutes on a 3/4" 4 flt carb em , until you have .25 cutting surface ( as not to taper the hole at the top from constand rubbing ), if you dial it in dead nuts shouldn t be a problem ,carbides are normally .0002 undersize predrill to what you would for a reamer and plung the em ,
1018 isn t exactly the nicest material for a perfect finish ,but this meathod will probably get you the best finish

[Ken_Shea]

Hey Dertsap,
Is that your personal 3/4" 4fl carbide EM that you paid for and then grind or the company you work for

[HuFlungDung]

It is a lot of bother to make a truly flat bottom hole in the lathe. I would prefer the mill as well. If nothing else, the finish will be excellent with the endmill, whereas it can be difficult to not damage the end of a lathe tool when facing exactly to center. The rough depth tolerance is practically nil if you don't want to destroy the lathe facing bar.

So, in the cnc mill:
- open the hole with a drill.
- circular interpolation with helical advance to rough out the rest of the material in the bottom of the hole. Maybe use a 3/8" endmill for this in this size of hole. Air blast would be good to get those chips out of there.
- circular interpolation of hole diameter to size (if your mill is accurate enough).
- final pass, again, circular interpolation with helical ramp in at full depth, maybe taking out .005 to finish to depth.
- if necessary, bore the hole ID to finish with a boring tool.

[Ken_Shea]

Hu, what do you know? I agree with Ken_Shea

[widgitmaster]

If the hole thing has fractional tollerances, just drill them all in the lathe, then grind a flat on the bottom of the drill and redrill them to depth!

Are these 1018 steel parts for welding later?

easier is better!
Eric

[HuFlungDung]

Hu, what do you know? I agree with Ken_Shea

Insulting you was a risk I had to take, Ken

Everybody has a different approach, maybe depending on what may have happened to them just recently. I was just doing some precision work of this sort lately, and I got fed up with the lack of control over the details of the depth and flat bottom in the lathe. I'll grant you that the lathe is great for holding the size on the final bore diameter

[Ken_Shea]

Insulting you was a risk I had to take, Ken


Well if the tables had been reversed I would have enjoyed every moment of it

[rcazwillis]

Are these 1018 steel parts for welding later?
Eric

Yes, I will be welding on them.

Thanks to everyone for the suggestions.

Based on the suggestions, here is what I am thinking. My skills for setting up center on the mill are weak. I think I will drill a 3/8" hole in each piece on the lathe. This is needed in the final part. Then use a 3/8" end mill to make the depth cut. Hitting center will be easy and I can use offsets to recenter each time to use the same code repeated. That should be efficient and produce good results, right?

[widgitmaster]

Another point that hasen't been mentioned is the ability to bore the predrilled hole diameter and flat bottom with a simple endmill of the right diameter, just resharpen the end to be flat instead of hollow. Just use a 1/64 smaller drill a few thousandths shy of final depth! (using a milling machine)

Your choice of methods depends on the tollerances required, as each method will produce a flat bottom hole. The repeatability of your machine is the only factor in controlling the depth.

Eric
Eric