View Full Version : Large Dia Cast Iron Drilling

12-07-2010, 12:45 PM
I have some parts to drill out and finish bore to 2.625 inches inside diameter by 5 inches deep (clean through the part) . The material is Cast Iron. Are there any good tips on doing this effectively with a lower horspower home shop Lathe? I have a 2 horspower motor on my Engine Lathe? Any tips are appreciated Thankyou Mike

12-07-2010, 01:15 PM
I have some parts to drill out and finish bore to 2.625 inches inside diameter by 5 inches deep (clean through the part) . The material is Cast Iron. Are there any good tips on doing this effectively with a lower horspower home shop Lathe? I have a 2 horspower motor on my Engine Lathe? Any tips are appreciated Thankyou Mike
Hi Mike,
I would chain drill around the outside and knock out most of the centre material. The hole could then be cleaned up a bit with a bimetal holesaw (with an extension perhaps) followed by boring to size. It is going to take a long time whichever way you approach this.

12-07-2010, 01:28 PM
Sounds pretty horrid. The large hole removal process works nice but this is a casting looks like a large wheel bearing flange. I had some dumb ideas like a homemade boring bar that had a bunch of different hdss cutters in it that would each remove like .070 thou or so as i rammed it through the Bore??? What you think of that ? Would it work??? Then I could finish with a large Reamer?

12-07-2010, 01:40 PM
Rotobroach is a good cutter for large hole drilling with low power requirements. The 5" depth might be problematical though. Cost is not low for a onesy twosy job, but if quantity warrants he price, they are a good choice.


12-07-2010, 01:48 PM
holesaw from both sides. Then extend the hole saw . cut the top off the hole saw and weld in sheet metal to grow the depth of cut to over 2.5"

12-07-2010, 01:50 PM
I'd just drill it until i ran out drills and then bore it. If you had many Jim's idea of the rotobroach is good - always efficient when you can remove material such that you get one humongous chip....what happened to your big lathe?

12-07-2010, 01:54 PM
Big Lathe? You mean the Gargoyle 30 inch hydraulic MONSTER?? Or the one in my home shop the Cincinatti Tray top? The cinci only has a 2 horsepower motor, Yet it has Gnawed out all sorts of material for many many years. Old but Pretty Decent. Its the one Im going to be using on this Job Mike. take care mike

12-07-2010, 01:57 PM
That sounds pretty good. I have a really good low rpm on my lathe. I will try to find dealer in my area. Perhaps i could drill till its plugged (so to speak ) clear out and reinsert and complete drilling operation? Thanx all for the great Ideas. Merry xmas?? mike

12-07-2010, 02:18 PM
I would look for a big spade drill on ebay. Spade drills don't take a lot of HP and they cut good. It would be easy to find one to go 5" deep. Then finish to size with a boring bar.

12-07-2010, 02:34 PM
The Annular Cutter Idea sounded great but after I called a engineer at a annular cutter factory I was told in Cast Iron iw was NOT Feasable at all. The material is far too aberasive he told me. I was thinking this annular cutter would of been the cats ass so to speak. BUT now perhaps the spade drill may get the Job/ I wonder if a 2 horsepower lathe would drive it?? AND these castings already have a small hole cast through them? I wonder if a sppade drill will start in a previously cast bore hole/? Or will it require a flat starting surface? Thanx

12-07-2010, 02:45 PM
The spade drill will be fine in an existing or cast hole if it is concentric. If the hole is not concentric, get an endmill a little larger than the hole and bore an inch or so to give the drill a good starting place. Ease into the part until the cutting edge has made a seat and is cutting good, then you can apply more pressure as appropriate.

12-07-2010, 02:46 PM
I don't know where you're at with the time vs. cost on this job. That said, I have done quite a few larger holes like this with only a 1.5HP machine:
*Start with a 1/2 twist drill. Drill all the way through.
*Switch to 3/4" twist drill (I used a reduced shank silver+demming type). Drill all the way through.
*Switch to 1" twist drill (once again, reduced shank is what I used here). Drill all the way through.
*Insert a straight shank extension arbor with 3/4"-1" socket.
*Keep drilling through with end mills by 1/4" or 1/8" sequence as necessary. They don't need to be "good" end mills, obviously. A really cheap import set works great for this kind of duty.
*Get as close as you can and then finish with a boring head to final diameter.

Takes a while. You might experiment with how much HP you have and the number of sequential steps are needed in enlarging your original drilled hole to speed it up. Works fine, though.

12-07-2010, 02:58 PM
Deleted double post.

12-07-2010, 03:02 PM
I would think that horsepower, or the lack therof, is not the limiting factor here. I think a lack of rigidity will be the biggest problem.

What is the largest boring bar that you can reasonably mount on your lathe?

What type of tolerances are you trying to hit?

If it is nice soft grey cast iron, this would be very doable with an 1-1/2 twist drill to start and lots of patience with an 1-1/4 boring bar. Sharp or very small radius on either hss bit or carbide, either brazed tool or insert. If you can step up to a larger bar as you bore, so much the better. Or start with a larger drill. A Cincinnati should be able to handle something like that.

Any kind of white or chilled cast iron, give up now. :D


12-07-2010, 03:02 PM
I sterted trying to find spade drill s locally. Travers i punched up spade drill and got some weird looking thing called a Multi Tool page 450 it was reasonably priced. Yet i always like to know someone who actually had bought one and it really worked. Ive bought things that i bnnever had any luck with at all. So im a bit gun shy so to speak about dropping lopts of cash (which i DO NOT Have) Visa takes another big Dump) Have to do some more research the spdae drill sounds interesting. i have never uded one. Thanx all Mike

bob ward
12-07-2010, 03:13 PM
With my 2HP lathe and standard tooling I would be doing a traditional method of drill 3/4" and bore it from there in 10 or 12 passes. All done from one side in one set up.

12-07-2010, 03:22 PM
It IS Grey Cast Iron. I will try out some basic drilling boring ops. Yet i wanted to be efficient in doing these nbores. The KBC p46 multi bore tool is cheap and looks like it might work> I have a few boring bars,. Some huge homemade ones that hold HSS blanks. I will try out a few things when the castings arive. They are on the way i been told. Thanx Guys for the varying insights to my post . I appreciated all the tips. Mike

12-07-2010, 03:39 PM
The Multi Tool is manufactured by APT, a good company. It would also be a good choice. It has the advantage of being piloted.

12-07-2010, 03:48 PM
While we're on it, has anyone actually used the specialty trepanning tools?---for example KBC p.52. Travers also sells them, p.77

12-07-2010, 04:06 PM
If you had started the job with a 3/4" -1" drill then set-up a boring bar when you first posted you would almost be done.

mike os
12-07-2010, 04:08 PM
I didnt want to say that:rolleyes:

12-07-2010, 05:22 PM
I'd vote for a spade drill followed by a boring bar, 1" min dia. Mount the spade drill on the toolpost and use feed. Peter

12-07-2010, 08:32 PM
Trepan tool pictured would have a limited DOC, perhaps 1" before
the fixing nut head hit the side of the hole. Ends of the tool
holder would rub first however. Used carefully it is not much
different from an adjustable boring head.

12-07-2010, 10:47 PM
Madman, The APT multi-tool is GREAT. It really works well in low HP situations, which is not an experience that I have had with spade drills. Spade drills have to go straight to full diameter and let me tell you turning a 2.6" (or so) spade with 2hp is NOT going to be fun, I'd consider 7.5hp a minimum for such a size.

Don't use coolant, cut dry and use low pressures air to push the dust (swarf?) out of the hole and a shop-vac or three to capture it before you coat your entire shop black.

12-08-2010, 09:28 AM
HA HA NO i would NOT of had them done. I am hoping to get these parts stready for a while. Not just 1 piece or 12 pieces more than that. When you eke out a humble existence in youre Garage Proper Planning on certain Jobs goes a long ways towards smooth sailing so to speak. Thanx all for the advice. Especially John i likesd youre idea. thanx again Mike

12-08-2010, 12:52 PM
If you are doing a lot of them, trepanning would give you some usable scrap and reduce the amount of metal you need to convert to shavings. Braze some carbide or HSS bits on the end of a piece of pipe.

Here is a pic of a very large (24-36") trepanning tool used to bore a hole 60 feet long, looks like it was made from pipe:
taken from this thread:

On a small machine, I would want a small number of teeth. 1-3. Helical groves would be preferred if you can, for better chip clearance. Bits should be a little wider than the pipe wall thickness to provide clearance on the ID and OD so the pipe doesn't rub. If you use more than one tooth, you can stagger them instead of each tooth cutting full width.