Sort of like this, but in a round boring bar:
I've been lurking on this forum and other machining forums for almost a year now, and I clearly remember seeing a thread about a lathe boring bar that uses a triangular insert and lets you cut with 3 different sides of the tool. You could bore, face, then OD turn all in the same pass. But now for the life of me I can't find it anywhere! It might not have been on this forum, possibly on PM, I really can't remember. But I've just spent the past several hours searching everywhere for it, nothing.
I remember one guy in the thread saying that he bought one but never used it yet. There was also a link to the company's website who made them, and they seemed relatively affordable (sub $100 for sure). It's driving me bonkers that I can't find it! I also can't really find them for sale at any of the big tool suppliers, enco, msc, shars, etc. I see one in the KBC catalog which looks great for $42 bucks, but I'd still love to hear more info if anyone has actually tried them. Here's a pic, its on page 293 of their catalog.
Any thoughts on how well this sort of tool would work? I've got a cnc converted grizzly 10x22 which I'm absolutely in love with. The part I'm making starts out as a solid 3" bar, gets drilled and bored to 2" dia ID, then the end gets faced and the OD gets turned to 2.96 (to scrape the ugly off). And instead of having to do a tool change in here to go from boring bar to turning tool, I thought this would be easier. Or not, I don't really know, it's just driving me nuts that I can't find it. I wonder how well it would do at boring. Right now I've got a 1/2" boring bar with a CCMT insert that seems to do well.
Thanks guys, hopefully someone remembers the stuff I'm rambling about.
Sort of like this, but in a round boring bar:
On second thought, the one I'm thinking of might have even used a square insert, making it better for facing. I remember the marketing info on the company's website going into detail on how it's great for turning/facing/boring.
I think you'd be better-off with the triangular insert. A square would rub on the sides, and have to be mounted perfectly square to avoid tapered diameters for the length of the insert's cutting edge.
That said, it's definitely a compromise tool. You always get better quality cuts out of I.D. and O.D.-specific tooling.
The boring bar in the pic is Iscar or Carmax both have boring bars like what you are showing
Your CCMT insert/toolholder should work great with the right insert I use them all the time
Pixman, by square I really meant diamond, but that wouldn't work so well for boring because you'd have a 45° angle at the bottom of the bore.
Mactec, I was just on Iscar and Carmex's website and I couldn't find a boring bar like that on either one (though I didn't look thaaaat hard).
Quick sub-question. What's the fastest/easiest way to remove lots of metal when boring on the lathe? On this part I've gotta make a 2" hole in 3" AL bar, 1.15" deep. What I've found to work well on my prototype is to drill a 1/4" hole, then use a 1" endmill REALLY slow to almost the full depth, then bore the last inch using my CCMT boring bar. Works well, but it's pretty slow going. My spindle motor is only 1hp so I can either do a high feed rate with a weak depth of cut, or high DOC and painfully slow feed. And it's 3 different tools. Time to build a pneumatic tool post turret methinks.
Is there a better way? I've considered one of those indexible insert drills, 1.5" would be a good all around size for me. I've gotta make 3 of these holes per unit, and I'd like to get to the point of being able to produce 50 units a month from my little home based shop. With that sort of volume, eventually spending $250 on a tool that does the job quickly and efficiently would be worth it for sure.
This is going to be simple: Valenite CenterDex! Those things have been around since dirt was invented, and are still one of their best-selling tools. It's a center-cutting milling cutter, but often used on lathes as a one-shot holemaker/boring bar for shorter holes.
Tell me what diameter shank is the biggest you can hold onto in your lathe and I'll tell you just which one to get. It's meant for low HP applications, but can take quite a bit if you have it. No starter hole required. Push it in on-center, then bore to finish size with one of the 2 inserts.
On a milling machine, it works the same way. Plunge in on-center, then circle mill your finish size.
Simple, and cheap. A cutter body with inserts should be under $150, and will do so much work it's indispensable. Honestly, no shop should be without at least one for quickly blanking out short, flat-bottom bores.
Woah that's exactly what I need! Thanks buddy, I hadn't seen that before. At the moment I've only made a holder for a 1/2" boring bar, but I could certainly make a bigger one if I needed to. I'll make sure to pick one up within the next month or two, I can definitely see how useful they would be! What inserts do they use? Something common I hope. And are they square 4 sided inserts? Cause that would be sweet, 4 new cutting edges.
Uh...it's Valenite, not valentine.
For your 2" diameter hole and needing a smallish holder size, I'll suggest one with a 3/4" shank. That'll allow you to also use it in a Bridgeport mill if you have one. The bigest-cutting one with a 3/4" shank is an effective cutting diameter of 1.125", and it'll go 1.25" deep. (You can also do a little hard turning to relieve the shank back a bit further and go deeper if need be. The part number:
S VMSP 112R 90CCC Use inserts: SD322P, grade VP5020 (the most versatile one)
The inserts will have a .031" radius on the corners, but you do indeed get 4 edges to work with per insert. If you're working at slower speeds and need a tougher, though less wear-resistant insert, ask for grade VP5045 (or if they have it now, the upcoming grade VP5050.) If all you need to do with it for now is aluminum, brass and maybe cast iron, there's a choice of 3 uncoated grades, UK20, UP30, and US10. For strictly aluminum, I'd go with the UP30, it's polished.
Overall, those tools are the most widely-used and cost-effective insert type drill-bore-mill tool ever made. Probably why they've been in their catalog since the 1960's!
Wow I fail at reading comprehension, thanks for the clear up. I've got a Grizzly mini-mill (Sieg X2) and I don't plan on getting anything bigger, but for now I'm only thinking about using this tool on my lathe. That one you suggested with 1.125" cutting diameter and 3/4" shank sounds perfect!
So is uncoated really better for aluminum than TIN or other coatings? I've heard that a little bit, but wasn't sure. And polished is even better, good to know! I've only tried coated inserts so far, they seem to work alright for aluminum with coolant, but I'm not digging in there very fast or very hard.
I just finished my coolant shield for the lathe, so now I can really turn on the fire hose without making an absolute mess!
I called Valenite's tech support to learn more about their uncoated grades and found out they're not polished as I had thought. Sorry about that! Their nomenclature is as follows:
US10 grade means "S" material class (high temp alloys, iron base alloys, titanium alloys), the "10" means harder , more wear-resistant carbide, low cobalt content.
UK20 grade means "K" material class (cast irons), the "20" means a little more cobalt content for added toughness.
UP30 grade means "P" material class (steels), the "30" means highest cobalt content for most impact resistance.
CVD coatings, especially straight TiN, is a high temperature process that can erode the sharp edge as it coats. Also, those high temp process coatings are typically porous surfaces that with aluminum can cause problems with a "built-up edge" condition (material sticking to the topside of the cutting edge.) PVD coatings are thinner and lower temp, so they usually can preserve the sharp ground edges. There are now a lot of MTCVD (medium temperature chemical vapor deposition) multi-layer coatings that out-perform simple one-layer PVD (physical vapor deposition) and CVD coatings. If your aluminum is a high-silicon alloy, use the "10" grade MTCVD coatings. For 6061, uncoated 10 grade is best.
Hope this helps.
Pretty much everything I do is 6061, for the aluminums anyways. Then probably equal amounts of stainless and mild steel. Very little if any cast iron. When doing aluminum I've definitely had the built-up edge condition, I've gotta go in there and knock the chunk off with a little screwdriver. I don't think it actually affects the cut, but I'm not sure. Certainly doesn't help chip evacuation. Looks like I can pick up some polished CCGT and TCGT inserts from my local KBC, which are the tools I use most often, so next time I'm driving by I'll be sure to do that.
I just machined a 2" dia hole 0.7" deep in some 6061 with my boring bar using facing cuts, with a few fancy dimensions and fillets inside, and the program took 9 minutes! Once I get to the point of making a LOT of these parts, that Centre-Dex will save me a whole ton of time.
Ohh and the coolant shield... WOW! Why didn't I do this sooner!