[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.

[kong]

Hu the man, that's the type I was considering, so I will go ahead and get myslef one. As mentioned earlier, roughing on the mill (or in my case, the router) is out, due to time considerations, so I will rough with a SCLCR bar I have, then attempt the fine facing cuts with the new bar.
Mrainey, I will need to cut bith sides of the part, so there will be blend mark. Like you said, this is not a critical application, so I can get away with it. The hub is facing the inside of the RC car anyway, so will not be seen.

If the worst comes to the worst, I can re-work the model to remove some of the profile on the hub-side of the wheel, but I need to prove to myself I can do it, even if it is with the aid of you guys

[Cold Fusion]

Nice looking rims! I've got another design like that except the spokes are twisted. It should fit the nitro rustler since I built it for the electric one. Would you like me to email it to you?

[kong]

One step at a time eh?! Since I can't even machine these ones yet, I would rather not get involved in twisted spokes, thanks anyways BTW, these are for schumacher XTR3e, hence the hub in the centre.

[mrainey]

Here's another bar I used years back. It's not strong and won't handle more than light cuts and feedrates, but as you can see, has a lot of reach. Uses a standard vnmg332 35 degree diamond.

http://216.239.39.104/search?q=cache...p+boring&hl=en

[kong]

Quick update and question -
I am awaiting a couple of catalogues to come through the post - you don't know how difficult it is to find a supplier of these tools that don't want to know the ins and outs of a cats ****!
However, jusytbrowsing ebay today, and found the perfect tool. Kennemetal A08-SVMB - 35 degree diamond insert, with 50 degrees clearance between the flank and part face, similar to your link mrainey.
So onto the question. It has a bore for through coolant, and the drawing quotes "1/16 - 27 NPT" so I take it this is the thread, and I need to provide a suitable hose adaptor to screw straight in? It may sound daft, but I have never used through-coolant before! Thanks guys.

[HuFlungDung]

Kong,

1/16" NPT is the smallest National Pipe Thread form (in the Inch thread system). It has 27 threads per inch, and most likely is a tapered thread (3/4inch per foot taper).

A lot of small lathes will not have the gearing to cut 27 tpi, if you want to try to make one, but cnc allows you to cut any pitch you want, of course.

It might actually be tough to find a fitting for that, but you could likely tap the thread out to something else that would be handier for you. You might have to anneal the end of the bar to do this.

[metlmunchr]

Cardinal rule of productive machining: NEVER try to use a mill to do lathe work. That being said, what you need is a bar to use high positive rake aluminum-specific turning inserts. Typical insert designations are CCGT, TCGT, VCGT, and DCGT. Bars to use these inserts are typically available down to at least as small as 3/8". From most every source, these are expensive inserts, but Travers http://www.travers.com has them in a Korloy brand at extremely good prices. I've used quite a lot of them and they work great and hold up well. If the pic I attempted to attach shows up, this is an example of what I use these inserts for. The wheel goes straight from turning center to buffer with no intermediate prep. For the RC wheel, I would first use a 2 flute ball nose endmill in the lathe to plunge and remove a good amount of the stock. Using the ballnose allows you to leave the minimum stock at X0, where turning is inefficient. Then, with these inserts, you'll have no problem in cutting to X0. Hope this helps.........Cliff

[kong]

Now that is a thing of beauty!
I have looked into the aluminium cutting inserts, and you are right, they are not cheap. but if I can achieve that kind of finnish then they will be a huge time saver. The only thing that worries me is the toolholder I have bought has either a neutral or negative slant on the tip (I can't recall offhand). Being a boring bar, I guess I can rotate it (or modify slightly since it is an ebay special) to give the positive cutting angle, then use the vcgt tips.
I have noticed that the other sclcr boring bars I own all have a negative slant to the tip, whereas my regular tools are neutral. Is there something different in the design on the bars for this to be the "norm"?

edit - of course, I don't understabd why the tip is angled downwards, but I do understand the tips of the inserts need to be positive. Hoep this makes sense!