Best Al cutting solution..

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.

Reply to
Bryce
Loading thread data ...

Bryce wrote in news: snipped-for-privacy@4ax.com:

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.

Reply to
D Murphy

Bryce wrote in news: snipped-for-privacy@4ax.com:

Bryce, Here is where you make your tool vendor applications people earn the check they back up to every week. I learned this the hard way..trying to do testing and keep up with all the production stuff, plus the project stuff. Worked myself nearly to death. Now...I give them specific criteria to meet, generally I will set the bar a bit higher than what I can really live with, just to see if they can meet it, which is a plus and added value on the productivity side if they do. Just write out specifically what you need for the application, invite a few in for an hour and lay it out. Make them meet your criteria as best they can. Invest as little time as you can afford, meaning let them keep up with all the paperwork, other than maybe putting a tool tracking sheet on the machine for the guys to jot down dates and pieces produced and reason for change. Let the tool applications people put it in a db and decypher the data and present you the reports along with recommendations. That is what they are getting paid to do...You aren't.

Reply to
Anthony

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.

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

Reply to
Bryce

Bryce wrote in news: snipped-for-privacy@4ax.com:

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.

Reply to
Anthony

Bryce wrote in news: snipped-for-privacy@4ax.com:

Well technically it's more of a modified radius blended into the first. Usually it's molded into the insert.

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:

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.

Reply to
D Murphy

The TFD inserts we are using now from SP3

formatting link
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.

Reply to
Bryce

Bryce wrote in news: snipped-for-privacy@4ax.com:

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.

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.

Reply to
D Murphy

Bryce wrote in news: snipped-for-privacy@4ax.com:

The last one we tried, from Sumitomo, was about double that of PCD. The test wasn't very productive in that the tool life was just slightly more than PCD, but not enough to justify the cost. The geometry of the tool didn't lend itself easily to a monocrystal design. In other applications, it would have probably been great.

Your welcome

Reply to
Anthony

We've begun using pcd endmill on some of our products for this exact reason...(needing a crisp, sharp edge--with absolutly no discernable raised burr).

No other tooling holds up even near as long over the long haul.

Reply to
PrecisionMachinisT

Hi Sam, do you mind sharing where you get them from, and a few pointers for anybody thinking of purchasing PCD end mills? It's so much easier to learn from others' experiences than to create your own. You getting around much, or how's the recovery?

Reply to
Bryce

Bryce wrote in news: snipped-for-privacy@4ax.com:

No other tooling holds up even near as long over the long haul.

Bryce, What deepth/dia do you need to mill? There are a few designs we use also.

Reply to
Anthony

Oh, I don't necessarily have an application off the top of my head, but we do make a lot of cosmetic surfaces with a 1/2" dia. x 3/4" length end mill. Usually finishing a profile just over 1/2" deep or so. Sometimes we rough and finish with the same tool, sometimes we use two tools. 6061-T6 AL in wrought condition, either round bar or rec. bar.

We haven't done a lot of production milling in the past, but it has been picking up a lot lately. We have a Mori NH4000 that has a 14K spindle, and is one year old now. That should push a PCD end mill fairly well I would hope.

Reply to
Bryce

Bryce wrote in news: snipped-for-privacy@4ax.com:

I'll admit, most of what we use is custom stuff. However, since you use such short tooling, it would be relatively cheap. The cost is in the carbide, not in the diamond. My suggestion would be a 2-flute, straight flute carbide shank EM with PCD, since you may need to go 3/4" deep. You can have a 5°-7° rake on the flutes to help with chip evac, and still have decent support on the cutting edge. More than that and your relief angles on the flute faces get too sharp and the edge has little support. This will reduce your tool life. Normally, you can single pass with PCD, provided you have the appropriate cutter diameter. Get in touch with Citco. See the following links:

formatting link
These are good folks, and provide a good product.

Reply to
Anthony

Hi Bryce,

Almost missed this one....these endmills were manufacturer samples, SP3 but as time progresses will probly integrate more into our programs.

Doing exceptionally well, thx.

Reply to
PrecisionMachinisT

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.