Best Al cutting solution..

I have a new Tormach CNC mill I'm using for some hobby stuff. A lot of what I'm doing is making parts of Aluminum billet.
What is the best cutter solution for removing lots of aluminum.
My Max RPM is 4500, the tooling is R-8 The spindle is 1.5Hp.
So I'm looking for suggestions as to the best bit for roughing out aluminum.
I'd also like feed and speed reccomendations to go with it .
Thanks in advance
Paul.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Why,
I'm sure we're all *very happy* for you....

No such thing exists what is properly called an 'aluminum billet'.

Not gonna remove any material at much of a competitive rate what with having only 1-1/2 hp. available...

Suggest cut dry, and with a 'roughing endmill' whenever possible....usually will be 3 fl and med helix in Al....look for nice deep gullets, highly pronounced rake generally speaking, of course.

Cut at a removal rate just slightly below where the spindle would otherwise stall.
--
SVL




Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

having
possible....usually
otherwise
Oh, I almost forgot.
Also, suggest learn how to quickly DUCK.
--
SVL






Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Proper term would be barstock...
alas if you google billet parts you will find that it's the popular term for parts machined from a signle peice of barstock. See: http://www.billetandacrylic.com / (Not really to my taste but they clearly have a differnt view of the term billet thn you do.
;-)
See my follow up post at the end of the thread for other comments wrt this post.
Paul
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Paul, You could try one of these. http://www1.mscdirect.com/CGI/NNPDFF?PMPAGE82&PMCTLG I've used the 3/4 dia. at about 3000 rpm x 1/4 to 3/8 deep @ 20 ipm. and had good luck on a machine with similar hp and rpms (bridgeport) as yours. I used microdrop mist coolant. There's a speed and feed chart on the page but you don't have enough power to push it that hard so you'll have to experiment. I could remove more at 3000 rpm then wide open I think because of the torque. I used the cheap one on the top of the page but the cobalt isn't much more. Steve
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Steve, thanks for a response to the origional question.
For the other posters... If you ask an electronics question I'll make sure to ridcule you first and then not answer your question. (Electronics is my profession)
I realize that the machine is not a 50 hp CAT50 VMC, but that would be a bit of overkill for my Garage ;-)
I've had the Tormach for about 3 weeks and I'm quite happy with it. For $6800 it comes ready to use.
Most of the stuff I build is small
http://www.rasdoc.com/paul/rockets/ballvalve.html and http://www.rasdoc.com/paul/rockets/airlander.html
and Parts
http://www.rasdoc.com/splinter/BilletFrame.jpg
for http://www.rasdoc.com/splinter/solar2004.htm
I had been using a Taig and the tormach is a nice upgrade for me. Heres a simple tutorial I did for some other rc modelers... http://www.rasdoc.com/splinter/RibsCut.htm
Paul
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
snipped-for-privacy@Rasdoc.com wrote:

Paul:          Some people in here just like to play to the role of the crusty curmudgeon, I wouldn't take it personal.
    Two flute end mills are good for removing a lot of material in aluminum. Four flute end mills don't have as much gullet clearance. I wouldn't cut alum. dry since it's a gummy material and often likes to adhere to the end mill (with sometimes disastrous results). A spray mister, of even a hand squirt bottle of mixed coolant can work wonders.    
    Nice work on the plane.
    Is that servo operated ball valve your invention? If so (and it has zero leakage under 3,000 psi), you might try to sell it to an automotive performance oriented supply house as a Nitrous Bottle remote operated valve.
--
BottleBob
http://home.earthlink.net/~bottlbob
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

I've been posting on newsgroups for a long time. I know not to take it personal, alas its sometimes nice to poke fun at the curmudgeons....
If your fairly new to a group you can pose as the innocent newbe and mabe make the curmudgeons feel bad for a few uSeconds. Its all part of the sport.
As for the Ball valves they are probably a lot bigger than they need to be for nitrous. The key component is the very high torque servo.
I'm using the ball valves for my air rocket and also for a biprop rocket similar to
http://www-rohan.sdsu.edu/~sharring/sdsurocket.html
Paul
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
snipped-for-privacy@Rasdoc.com wrote in
Paul, If you want really nice finishes, PCD or diamond coated tooling is the answer in aluminum. Not cheap, but they will last forever.
--
Anthony

You can't 'idiot proof' anything....every time you try, they just make
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

Hey Anthony, along those lines, we have started using quite a bit of PCD tooling - largely from your recommendation. It has worked out very well for us, even though our particular application is not necessarily ideal for any cutting tool. We have a very high volume production part that is made out of 2024 AL, that needs a reflective surface on one of the faces.
Our speeds, feeds, and depth of cut is not really optimal cutting conditions, but it is what we found works. We run 8000 rpm on a face starting at .375" diameter and going to .650" diameter, feed .0005"/rev. with a .03125" nose radius, and take about a .002"-.003" depth of cut. This ends up with nice results for us, although with PCD inserts, after about 10,000 or 20,000 parts, we start to get poor results. So we tried a TFD insert (chemical vapor deposition sheet of some type) from SP3 Diamond Cutting Tools, and we have had much better edge life so far, as well as better surface finishes.
Thanks for steering us that way, we are now using both types for turning as well as boring applications, with outstanding results.
Another particular job that it has worked out well on has a bore that is finished after a 4-48 cross hole is roll tapped through the side, and standard carbide boring bars were leaving a burr in the threaded hole. PCD bars leave virtually zero noticeable burr of any kind. That's super nice.
--
Bryce

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Bryce, The grade of PCD will have an effect on the finish. For roughing or normal machining, a coarse grade is better, as the larger diamond particles last longer. But, with larger diamond particles, the binding agent breaks down at the cutting edge between the diamond crystals, leaving a rougher surface finish. A smaller (finer) crystal size will help this considerably. Check with GE and Debeers for a fine-crystal PCD blank. This may be the reason TFD is outperforming the PCD in this application. Edge prep on the diamond also makes a difference. Relief angle plays a major role also. That's an itsy-bitsy radius for trying to get a mirror finish. If you can get to the part with something along the lines of a 0.120" radius you could speed up your feeds considerably and maintain the finish. It will impart a bit more load into the cut as your surface contact area is larger.

Your welcome. I just try to help.

That is one NICE thing about diamond tooling, it cuts CLEAN - Meaning it actually cuts instead of just mashing it out of the way. I'll also bet you don't make many (if any) adjustments during a run either. Consistency is it's other enduring trait.
--
Anthony

You can't 'idiot proof' anything....every time you try, they just make
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

Unfortunately, our part geometry barely lends itself to 1/32" radius. These are screw machine parts, dontchaknow (.650" part OD). Our failure indication is actually a chatter problem, which even with a new insert, is evident at our current feedrates if we take a lighter or a heavier depth of cut. Just had to play around for awhile, but everything is working great now.

Only for temperature, which depends on which axes of our swiss machines we are using to position the tool (or part). The longer the axis travel, the more temperature changes become a factor. We're in a new building with a much bigger shop recently, and the ambient temperature doesn't change as much. :-)
--
Bryce

----== Posted via Newsfeeds.Com - Unlimited-Unrestricted-Secure Usenet News==----
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Bryce,
You might want to see if the insert can be prepped with a wiper. We did a turnkey a while back on an aluminum casting that had a taper that was a sealing surface.
It was a very high volume part so by having the insert prepped with a wiper we were able touble the feed rate. It was also a fairly light DOC and we were restricted to a small radius due to the part geometry.
I want to say it was Kennametal that provided the inserts but I don't remember for sure.
Note to Cliff: Yes a wiper will work on a tapered surface. It just needs to be lapped on the proper angle.
Not that the note will prevent a hundred posts, but one can dream, eh?
--

Dan

Scopulus est usquequaque nefas
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

I had been thinking about having a special insert made to do exactly that, but I just haven't had the time. One thing that I was not sure about is what normal wiper geometry was like - in other words is the whole wiper actually in contact with the feature you are cutting, or does it have some relief, just less than 5 that an 80 insert would normally have?
The feedrate of .0005"/rev. is the other thing that I was not sure of. Would a wiper still be able to aid in this situation? I suppose it depends on the geometry, which I was unsure about.
We spent about a year of messing around trying to get all the other problems worked out of that particular part, and product line, and when everything works I don't mess with it anymore, because it was so seldom that everything would be going right at the same time.
Right now buying stuff off the shelf is about the only option that I have with all that's going on around here. So far this year we have made almost exactly twice as many production parts as we made in the whole year last year, and it's only July. Have open orders for another 60% of last years production, with more every day. Last year we did 2 1/2 times the production we did the year before, etc. Got nowhere near enough dudes in the shop, and we're running machines 24/7, literally.
BTW, we have a BN20 coming in some time next week, but maybe you know as much about that as I do. Thanks for pointing it out to us, I saw one that Traver was showing at a small local toolshow also. Can't wait to see it here.
--
Bryce

----== Posted via Newsfeeds.Com - Unlimited-Unrestricted-Secure Usenet News==----
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Turning wipers are usually a secondary radius set behind the corner radius. But in the PCD turning application we just had them give us a "flat" or 90 degree corner after the radius. The flat was about .015" IIRC.
Which makes me wonder if you couldn't turn with a pcd tipped groover.

The idea is that you can usually double your feed rate. By having a flat lapped on the tip you may be able to go even faster.

It must be that bad economy that Cliff is always going on about. We have been short handed here for a while.

Independent cross slides will change your life for the better. Pinch turning can solve a lot of problems with tool life, surface finish, and chip control. Plus that thing is fast.
The only downside to that machine is that the tool zone is tight. Make sure that you buy stubby end mills and drills for the live cross tools. But it will be 30-40% faster than your BS19 on most parts.
Have Traver show you the programming software for that machine. It's called BN Abile. I think that you might like it.
--

Dan

Scopulus est usquequaque nefas
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Our application is a slightly tapered face (not perpendicular), tipped back about 3 from being square. That's why I was curious about the secondary radius thing, also because our feedrate is so slow.

I've thought about that or something similar many times, might work extremely well.

Having a lapped flat like this application would lend itself to a variety of feedrates, but out of curiousity, with a standard wiper is there an optimal feedrate for the secondary radius to be most effective? For some reason I had thought that it was 1/2 the primary nose radius value, is that right, or not?

Good to know about the tool zone. I guess that makes perfect sense if you're trying to pinch turn, can't have things hanging out everywhere. It's pretty hard to find any jobber drills anywhere near our swiss machines. <G>

I think somebody mentioned it, but we haven't seen it. I'll ask about it more next time I see him. Thanks.
--
Bryce

----== Posted via Newsfeeds.Com - Unlimited-Unrestricted-Secure Usenet News==----
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Yup, should work nicely. Just make sure the shank is thick enough to offset the side forces from the 3 angle (unless you have the option to turn the slide to the 3). 4 - 5 mm carbide should be enough if you can turn the slide, 5-8 if you can't.
I would suggest the pcd be what was the old GE1800 series, both GE and Debeers diamond divisions have been bought out now. (I found out today while discussing some things with our tool technology guy.) They have renamed all the stuff, even though it is identical.
--
Anthony

You can't 'idiot proof' anything....every time you try, they just make
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

Well technically it's more of a modified radius blended into the first. Usually it's molded into the insert.
<http://www.coromant.sandvik.com/sandvik/0110/Internet/I - Kit1/se02673.nsf /Alldocs/Wiper*Inserts*2AWiper*Technology> >

The other thing to consider is that there is a limit to how good of a finish a PCD insert can produce. Polycrystaline Diamond (PCD) literaly means many crystals. So the crystal size has an impact on the finish. The coarser the grain the higher the least possible Ra value will be. A single crystal natural or synthetic diamond will be capable of a better surface finish.
Here is a company to look at for some alternatives:
<http://www.technodiamant.com/

I don't know of any company offering a wiper on diamond inserts as a standard catalog item. I got a lot of resistance from the tooling guys when we did that project. So I took a worn PCD insert and lapped it on an Accufinish grinder by hand using a porcelin wheel and we did some test cutting.

Heh. You got that right away.
--

Dan

Scopulus est usquequaque nefas
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

The TFD inserts we are using now from SP3 (http://www.sp3inc.com/hometool.htm ) are supposed to be a binderless composition from what I've been told. They are working extremely well so far, and run about $70 an insert. Is synthetic diamond a better solution yet? How expensive is it?

Sorry, I guess I should have indicated that I was wondering about carbide wiper inserts and their geometries, as we use a few of those also for other things. Is there a sweet spot for feedrate that is related to the nose radius, or can you take any feedrate of a normal insert and double it, and have the wiper work to its best advantage?
Thanks for all the info Dan, and Anthony.
--
Bryce

----== Posted via Newsfeeds.Com - Unlimited-Unrestricted-Secure Usenet News==----
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

I don't know if a single crystal diamond would be better or not. It would really depend on whether or not you are on the borderline of being able to hold the finish you need. IOW, if you are right at the best finish a PCD insert can do, then it may be worth trying out a monocrystal, either synthetic or natural.
As far as price, I haven't bought one in a long time, but they were more than double the cost of a PCD. But of course it's cost per piece that matters most, and you'll need to talk to a salesman and arrange for a test to find that out. They will usually provide test tooling for free. It just takes some time.
I think that there is good potential in your application for improvement. If you could get to .001 IPR feed, the cut time for that tool would be half, and the tool nose would see half as much material passing by it each cycle, which should improve tool life considerably.
Consider this example:
Turn a 1" diameter by 1" long. For each revolution of the spindle the tool nose travels through 3.14159" of material (1 x pi). So at a feed of .001" the tool will see 1,000 revs when turning a 1" length. Therefore the tool nose will travel through 3,141.59" of material during that cut. Kick the feed up to .005 IPR and the tool will make the cut in 200 revs. Which translates to 628.318 inches of material that the tool nose passes through. A difference of over 2,500 inches.
If your tool wear is normal, then having the tool nose travel through less material will result in better tool life.
Most people like to think about tool life in terms of time. It's usually better to consider it in terms of distance.
So being at a five tenths per rev feed rate, I'm thinking there is room for improvement all the way around. But you know how it is, there may not be, due to your application and conditions. Testing, unfortunately, is the only way to find out for sure.

There is not really a sweet spot per se. The secondary radius is offset by roughly the radius amount. So anything more than double the feed rate you will see an increase in surface roughness, as you start to lose the wiping effect.
Anything less than that distance and the secondary radius will cut the high spot. I suppose in theory being at a feed rate that divides evenly into distance between the nose radius and the wiper radius would give the best results. IOW, for a .015" radius a feed of .003 or .005 might yield a better result than say .0027" or .0047". I don't know for sure and I'm not up for the math today.<g>
My guess is that you'll see it in the profilometer trace, but it won't affect the calculated Ra value by very much if anything at all.

Any time.
--

Dan

Scopulus est usquequaque nefas
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.