Boring Deep Holes

[Bob_W]

Ok, Probably going to wear out my welcome here as I try out this new site format. But now a real question:

I am just beginning to build a 1/2 scale Olds hit and miss engine. The crankcase is cast iron and I will begin the first major operation of boring the main bearing journals and the cylinder bore soon. The journals will be 13/16" diameter with a bore depth of 4.5" if I go through both sides with one setup. The crankcase is too large to set up on my lathe for line boring (?). After the journals are complete I will bore the cylinder at 1.875 for a depth of 5". I only have a 2.5" boring head for the milling machine for this operation. I have made a boring bar that will reach the 5" depth from .75 dia 4130 steel rod and am just starting making practice cuts with it in some CRS in the lathe. Not sure it will work well in the mill. I expect that I will have to stop several thousandths short and finish by honing and lapping. If I can't do it on my equipment I do at least have a friend that does, but that just isn't the same [img]/ubb/images/graemlins/frown.gif"%20alt="[/img]

Any suggestions on getting the main bearing journal and cylinder bored accurately would be appreciated.

Thanks
Bob

[JimGlass]

Hi Bob;

If I understand correctly, your boring a 13/16 dia hole 4.5" deep. Your depth/diameter ratio is not in your favor becuase the diameter will limit the size and rigidity of the boring bar. However, I think you can do it in a mill. Not sure why you are making your own boring bars?

I'll bet your boring head accepts 1/2 shank bars. That will be a problem. Kinda like a log chain with 3/8 links accept for one 1/4" link. The whole chain may as well have 1/4 links.
Jim

[Harold_V]

Bob,

There's one thing you can do to help you through this, but it won't be cheap. A solid carbide boring bar will do the trick, but they're not cheap. They are hell for stout and don't chatter nearly as much as steel bars. You can hang them out quite far with great success. If your pockets are deep enough, get one. It is VERY important that the shank be solid carbide, otherwise you gain nothing. I'd suggest one as large as possible in diameter, naturally.

I understand all too well your desire to do the job yourself. I feel the same way about the things I do, too.

Good luck,

Harold

[Bob_W]

Jim (and others):

Seems you understand the problem. The bore depth is not continuous due to the portion reserved for the crankshaft. I did not have a boring bar long enough to handle the job, but did have a piece of 4130 laying around to make one. I also thought that by using the 3/4" diameter rod I would gain a little stiffness even though I had to turn down the end to 1/2" to fit the boring head. A carbide shank bar would probably be better if I had to buy one.

Since the journals will be lined with 5/8 ID bronze bearings, would I be better off by using a 13/16 reamer to try to get the finished bore in one setup? I can make the bearings to fit. I had done this before on a previous engine and it worked OK, but this one is larger. On the previous one, I spotted and drilled the first side to a diameter that matched the spot drill. Then spotted the other side by passing the long spot drill through the first side using it as a 'drill bushing' to help prevent the drill from wandering. Then drilled and reamed both sides to final size. Will this work on the larger engine or will I have the holes wandering off too much? I can tolerate a small deviation since the cylinder will be aligned and bored to the crankshaft.

Bob W

[Harold_V]

Bob,
I'm not sure I'd ream it, but that could work. If you did choose that route, you'd be very well served to line bore first, picking up the second bore to guarantee concentricity, then allow the reamer to take the hole to depth. That way you could use a shorter bar and limit chatter. Personally, I wouldn't trust the reamer to locate concentric with the first bore without this operation. Problem with a reamer is unless it's still in the first side, when it enters the second hole there's little guarantee that it will come out concentric. Even then it can wander a thou or two. Crankshafts should not run in that condition. The only way you can get them to run without binding is to have excessive clearance, and that's no way to do the job. The other problem is if the crank runs mis-aligned , the throw of the crank will not be square with the bore, so the rod will bind. Of course, I did read that you'd align the bore with the crank, so you might get away with it in this case. Good luck, regardless of the direction you choose. Fun stuff, figuring out the best way to go with what tools are at hand, eh? [img]/ubb/images/graemlins/smile.gif"%20alt="[/img]

Harold

[Hanz]

If you don't midn investing a little time, what about making a jig, out of a weldment, that would be similar to a full size engine align bore machine.

First rough your hole in however, and leave say .060 or so.

The jig I picture is basicly a steel box, with the engine bolted or clamped in place securely. There is a .750 alignment hole on each end, bushed if you want to be fancy, or for one time use not neccesary.

Your boring bar is now a long piece of .750 rod, with a small cutter protruding through a hole 90 degrees to the shaft. Set screw 90 degrees to the cutter, to lock it in place. Depth of cut is set and measured from the shaft, ie .050 out of the shaft would be a .850 bore (.425 radius)

This jig would sit vertically in the mill and the end of the shaft could be held in a collet to drive it and feed it. Can you picture it?

[Bob_W]

I agree with the concerns using reamers. The gap between sides in this engine is approx 2.125" so I would suspect on a 13/16th reamer the flutes would still be in the first section when they reach the second side. I was checking on the carbide boring bars and they may be priced a little high for the amount of use I would give them. Useually I don't have a problem buying special tools just for one job, since it gives me an excuse to buy more tools! I'll keep thinking about this and reading posts for a little while before I start. The casting had some work already started by the person I bought it from and now I first have to re-establish the alignment and dimensions to the tooling plate it is mounted to. The guy wasn't quite as accurate as I would have liked. Shouldn't be a problem once I get through the planning stage.

Thanks for the ideas.

Bob

[Jim_King]

Bob.If you want to make a boring bar,use the full 3/4" stock and put it in a collet or tool holder.You may turn a short length of taper at the tool end for chip clearance.I dont know if you ever bored with a fixed bar but you place an indicator against the back side of the tool and loosen the set screw and bump your tool out half of what you want to remove.It is a little tuff for a small bar because of the space limitations. You can finish the top bore first with a shorter bar and then change to the longer bar and touch off this finished bore to set your tool for the bottom bore.This would probley work out fine for you if you use the 3/4 in bar as I mentioned. Wish you success. Jim

[Al_Messer]

Bob, you say the workpiece is too big for your lathe. Do you mean it's too big to mount on the carriage, or on the faceplate? Years ago, I saw a construction article where a jig was made to fit the compound to which the workpiece was bolted before a boring operation was carried out. What size lathe are you using?

[Bob_W]

First item: I tried my boring bar in the mill with the boring head a couple hours ago. Had terrible chatter while cutting approx 1.25 dia in a test piece of CRS. The slowest speed on the mill of 270 RPM doesn't help. Expect more problems in the cast iron at 1.875" bore. Any feed and depth of cut chattered, but the little more aggressive cuts were better. That will be a problem as I aproach finish diameter. Don't care too much before that point. Any suggestions as to tool geometry that might reduce this chatter? Currently I have a sharp point on the tool and have tried different angles on the tool. It is a 1/4 round shank tool bit so I can rotate in the bar.

Second item: I had thought about fixturing the crankcase on the cross slide and then bore with a bar mounted between centers. This is a small lathe and the bore is way above center [img]/ubb/images/graemlins/frown.gif"%20alt="[/img]

Not going to give up easily but will be talking to some friends about boring this for me. If I can rough it out, it will at least save them some time. Also have to consider the working height of the mill as it will be close also.

With the new site, I can post pictures if that would be helpful. Although I think you guys don't have problems visualizing this one.

Thanks
Bob W

[Hanz]

Hey Bob-
Maybe fine tuning your setup will help. You made your boring bar- is it a VERY nice fit in the head? My new boring bars are such a perfect fit that when you insert them, you have to wait for the air to bleed by. Then you can let go of them and they won't fall out, because of vaccum.
Second- is the tool bit razor sharp?
Third- what feed rate?
I am asking theese questions because I just bored a 1.750 hole in CRS yesterday. Although my bar was .750, and I believe maybe 4" long, I pushed it good and had great results. My roughing speed was about 180, with a .040 cut, at .006/rev. My CRS was 2" thick, I used the long bar just to clear my clamps. For finishing, I backed it down to about 120 rpm, took .010 and then .002, at .003/rev. Results were a very slick finish. I do believe with the right tweaking that you maybe could do this with your casting.

Keep the tool VERY sharp with plenty of relief, and small cuts (.010 or less), and what is your feed rate?

Let us know.

[jan3]

Hi Bob Don't know what kind of mill you have,but if you use R8 collets make a boring bar 1" on the small end and 1.750 the remaining length.Tool bit can be adjusted via a set screw and another set srew to hold in place.Use a carbide tool bit,set it to rough all bores ,then for finish cut .Leave .002-.003 for honing.For the crank journals use the mill also.Use a .750 diameter bar, drill a hole in back side about an inch deep say .437 in diameter and insert a piece of carbide rod,tap 1/2-13 and insert set screw this should help with the chatter problem.