[cnczoner]

Hi all,

I am experimenting with turning alum tube, but getting a really odd finish. The photo below will explain the problem, but some important data -- this is 2.25" OD, 6061-T6 round tube. I'm spinning at 1500 rpm, so sfm works out to 883 sfm. That sounds high from numbers I've seen elsewhere, but I'm using cheapo C2 carbide tool bits (the 1/4" shaft one of these... http://shars.com/product_categories/...09/E_Threading) and don't have any data on what is the correct speed is for this.

I've tried cutting .005" and .010" DOC at feeds of 0.5 ipm, 1 ipm, 2 ipm and 3 ipm, and the best seems to be .005" at 1 ipm. And I've tried both dry and spritzes of ATF, but the finish is still dull, even in the rate cases that I manage not to get this odd bumpy effect. Any thoughts on if this is related to my SFM speed, cutting bit, DOC, feed, or something else?

Thanks,
-Neil





.

[mrcodewiz]

I always spin the aluminum fast and use finishing hss tool with a large radius and copius amounts of wd-40. Comes out like a mirror.

I just looked at those bits - they are threading tools. The radius is waaay too small.

[The Blight]

Looks like a dull cutting edge. You might want to use a cutter with a sharper edge (angle actually) and a small radius at the tip. Also check if your tool is in center.

Edit: Took a look at the tools you are using (just read mrcodewiz's post), and you should definitely use a tool with a radius at the tip. If you can grind HSS tools yourself, you should grind a tool with a sharp cutting edge and a radius at the tip with a chipbreaker.

[ronfournier]

I turn ala. on a regular basis you need to get your surface footage up to 1200 and you shoould be using a high shearing insert and feeding at .0035 per rev.

[Eurisko]

Make sure that the tool is cutting on center. Also make sure that the spindle is running in the proper direction don't laugh, I've done it myself.

It sounds like the tool is rubbing, not cutting.

[cnczoner]

Thanks for the replies.
My max rpm is 1500, which is the 883 sfm. How should I adjust feed and doc for this? I did verify direction, but I'll check to verify that the tool is centered properly. I also have one of these tool bits in a flycutter currently (which gives me a beautiful finish!), so perhaps I should try that bit instead. It's C2 also. I intend to pick up indexable tooling later, but I wanted to experiment with el-cheapos first.

I'm avoiding grinding my own bits for now since that introduces another (major) variable, and other for other "logistics" reasons.

So what is a "high shearing" insert? As I continue to build up info on the type of inserts I'll need for indexible tools, I have figured out that I'll need a positive rake or a sharp chipbreaker (so it essentially forms a positive rake). Is that related to "high shearing"?

BTW, any recommendations on tool bits (not indexable) that work well on aluminum, and that I can pick up from Enco, McMaster, etc?

Cheers,
-Neil.

[cnczoner]

.

[mc-motorsports]

Carbide inserts for aluminum are great for production work where you want to keep the machine running and not worry about tool wear changing your finish too much or changing your tolerance, reduces down time by not having to change tools out or compensate for wear to stay in tolerance. HSS is a better tool for nice finishes on aluminum, especially if your using a conventional lathe.

[skmetal7]

1500 rpm seems a bit fast, especially for how slow the tool is moving, try running round 650-1000 rpm and 5ipm and yeah you should use a larger radius tool.

[mrcodewiz]

I hand grind them but mine look very similar to the following. If you make your own, Just round the nose and stone it up real nice - You will get a great finish. Otherwise just get an HSS bit like this. Of course you will rough it with a normal LH or RH tool.

http://littlemachineshop.com/product...967&category=8

-CW

[cnczoner]

I don't know if indexable HSS inserts exist. This will be low-volume production (~50-100 pcs per batch), and definitely CNC'ed. The way I'm looking at it is that if production shops can get a great finish with indexable tooling, then I can too -- once I figure out what I need (tooling and machine). For now though, I'm experimenting with a chuck mounted in my mill, which makes it a vertical CNC lathe.

[cnczoner]

So I did some tests and had major successes. I'll tell you now that the tool bit was the issue.

First, I dug up this toolbit from a box of parts for my 7x10 lathe. IIRC this came from LMS some years ago, but I can't remember if it was for turning steel or alum. Either way, the finish was MUCH better...




After some experimentation, I figured out that too fast (1500 rpm at 10ipm feed) caused problems, as did too slow.




I later tried the C2 carbide bit from my fly-cutter and that produced some excellent results. I first got the best finish at 850 rpm (~500 sfm), but later discovered that I can go up to 1500 rpm if I increase the feed, but too much doc (over .010") was a problem. Ignore the lowest section in the photo below, as I was experimenting with brushing with scotchbrite pad to smooth out the surface and eliminate burrs.




That said, I've just ordered some C2 tool bits from Enco, so I can run more experiments, but it'll be indexable after that.

Thanks,
-Neil.

[BobWarfield]

You can grind an HSS tool to do what you want. If you prefer indexable tooling, you want to track down some of the aluminum finishing inserts that look like this:



or this:



As you can see, these are polished inserts with super high positive rake. They look a lot different from normal CCMT inserts.

These are almost always sold as CCGT, though they'll fit CCMT tooling. You can get the latter from Glanze or Micro100. Grizzly sells the Glanze tooling, and I think I got my Micro100 1/2" shank tools from Wholesale Tool.

For more information on this kind of tooling, you can check my website:

http://www.cnccookbook.com/index.htm

Search for the word "positive" and there are several posts.

Also note you can get very high positive rake mill tooling. For example, I have a Lovejoy face mill and an Iscar Helimill 5/8" indexable end mill. Both are great for a small mill in aluminum.

Cheers,

BW

[thebodger@roger]

A fine mist of water based coolant from a old carpet spray pump bottle, will help a lot when doing any aluminium cutting. The problem with aluminium, is that it starts to "stick" or build up on the cutting tool edge, as things get hot from the cutting action. The trick is a little cooling of the material and tool to prevent this build up. And of course your tool must have the proper angles, so it's actually cutting not rubbing.

[cnczoner]

Funny you mention that. I've been looking at Grizzly's boring bar H8282 and DCGT32.51-AK inserts similar to those CCGT's you mention (http://grizzly.com/products/Carbide-...Aluminum/H8339)

I was hoping to find something similar using a V- insert (35-deg included angle) as that would allow me to machine the outside and inside of the part with a single tool. I'm not sure if a V- insert will have any finish issues, although I can't see why it would if it has the same radius.

Cheers,
-Neil.

[cnczoner]

Bodger, I did try my usual coolant (spray bottle with ATF) but that made no noticeable difference. Perhaps because I was cutting so slow and with so much delay between passes (typing individual lines of g-code into mach 3 while machining) that there was minimal heat. And I did touch the cutting tip between passes once and it was barely even warm.

Cheers,
-Neil.

[BobWarfield]

Funny you mention that. I've been looking at Grizzly's boring bar H8282 and DCGT32.51-AK inserts similar to those CCGT's you mention (http://grizzly.com/products/Carbide-...Aluminum/H8339)

I was hoping to find something similar using a V- insert (35-deg included angle) as that would allow me to machine the outside and inside of the part with a single tool. I'm not sure if a V- insert will have any finish issues, although I can't see why it would if it has the same radius.

Cheers,
-Neil.

Here is another thread discussion the CCGT inserts and boring:

http://www.practicalmachinist.com/vb...d.php?t=153611

Check in with exkenna. He mentions a special he's about to run that sounds like a good price to me.

Even if you don't wind up with a single tool, just being able to use the same insert simplifies life.

Cheers,

BW

[Verfur]

look at a CCGX insert design and you will see what it takes for relive angles.

also tubing can be tricky (lack of regidity) so very small radi (430-431) and low IPR of around .003 DOC will depend on regidity so ovious to go heaviest first pass (even higher IPR) and progressivly lighter passes (DOC and IPR).

Carbide inserts for alum would easly run you into the 1000+ SFM

add lots of coolant

[cnczoner]

I've been in touch with exkenna and think I'm going with 2 tools both using the DCGT inserts, and I'll make a gang-tool adapter for them. My previous thought of using a single tool to machine both the inside and outside of the tube would've required changing the spindle direction, but I've worked out that I mount one tool at an angle to get the cuts I need. I'll post some results.

Cheers,
-Neil.