Which boring bar?

[kong]

Which boring bar is best suited to internal profiling, and removing a fair bit of metal with it? I have seen somewith round tips which look good for profiling, but when it comes to removing material, the depth of cut on my little machine will be small. I have also seen bars which use a D style insert, but how well will these profile? Since I don't a lot of spare cash, trying to earn some money from this hobby, I can't afford a range of tools, so trying to buy one or two that will do the job. I am trying to make alloy wheels for RC-cars, the models I am working on at the moment are 2.5" diameter, and around 2" wide. Any comments on the necessary tooling for cutting the insides would be great, since there are some complex cuts around the back which give me problems! It is difficult to see, but the spokes are curved.

[DAB_Design]

Why not just use an endmill and 'pocket' them? I'm sure the tolerance isn't too great on RC parts, but holding it to within +/-.002 shouldn't be a problem (unless the machine itself is of concern).

[kong]

I don't have a mill (well, not cnc, and not one which runs), so I will use the cnc router to cut the spokes. but for pocketing a 1" deep profile, with a curved bottom would take too long, then it would have to be put on the lathe for a clean-up anyhow. Good idea, but I just don't have the equipment for it

Hmmm, hang on a minute, are you on about putting the end mill in the lathe?

[DAB_Design]

Actually I was thinking in a mill. But since that won't work........

You can't use end mills in your CNC router? Sorry, just don't know. Not enough Z travel?

[kong]

Oh yeah, I use end mills all the time, I just don't like the thought of cutting a 1" deep pocket with a curved bottom, the surface finnish would be rubbish, and it would take forever! My router does tend to vibrate a bit when the going gets too tough!

[DAB_Design]

Forgive my ignorance, I have NO experience with routers. CNC though I can do.

But, if you were to use say a 1/2" tool just to rough it, in small steps, .125 or .250, then use a 1/2" ballnose tool to finish the convex/concave surface, with a small enough step over, you should be able to accomplish a fast enough feedrate and the finish wouldn't be all that bad. For example, using a 1/2" ballnose with a .020 stepover on a FLAT surface, the scallop height is only .0002" of course it would increase bit on an angle.

Maybe I'm not understanding exactly what you are wanting to do.

[balsaman]

Kong,

What about this style. If you rounded the nose a little it should make a reasonable finish. Not that I know beans about boring bars but I have found going in, then setting the cutting depth on the inside (bottom of the hole), then cutting out away from the chuck works not too bad with this style boring bar. Results may vary.

Eric

[kong]

Dab, I can take a maximum 2mm depth per pass before things turn ugly, but you are right about the ballnose bit. It's just a time thing, and the noise of operating the router for prolonged periods. Don't forget, this is not a one off piece, so the need to get it right now is important if I am to sell them.
Balsaman, here is a better look at the problem. The standard boring bar makes it tricky to get a good radius cut on the back side of the wheel. I figure a D style insert will have enough of a point to plunge into that un-machined space safely. Of course, I do not know for sure though!

[mrainey]

I used to machine a lot of aerospace parts that had a shape similar to your part - just a lot bigger.

I used a boring bar similar to the one pictured to get out everything I could, then followed with what we called a trepanning tool with full nose radius insert (essentially a tool for deep face grooving), with a blade under the insert for support. The blade has a radius to clear the bore of the part.

Don't even know if they're made that small.

Here's a picture:

http://manchestertools.com/products/...d_sdfg_rst.asp

[kong]

I am awaiting delivery of a cataologue from www.thinbit.com that specialise in these small tools, they may have something that will do it. They do sell small trepanning tools, the only problem is the waiting time for spares since they are in the US and I am in the UK!

[HuFlungDung]

Hi Kong,

Plunging and machining a blind recess in the lathe is challenging, especially the roughing. I would attempt to do the basic roughing in the mill and then take a light cut in the lathe with a profiling tool. You can buy boring bars that are made for profiling. I would check out Kennametal (as an example) for ideas: Top Notch Profiling Boring bar A08-NKQCR05 This is a 1/2" shank bar which will bore in a hole as small as .67". But, if properly set on center, I would expect that you could face right to X0 with it, at about .005" depth of cut. This bar has 17 degrees of clearance between the flank of the insert and the part face.

[mrainey]

If you're doing the left side of your illustration, one bar should work. If you're doing the side pictured with a bar (my assumption when I mentioned trepanning), one bar can't do it all. You have a straight bore and a straight hub diameter on the same part. You might get away with a r.h. and a l.h. bar, but will have to contend with an almost-inevitable blend mark. Blend marks weren't allowed in aerospace, small ones are probably ok for your job.