PDA

View Full Version : Low HP BP face milling QCTP blocks



PixMan
08-27-2011, 04:31 PM
I thought I'd share this with you to show what can be done with older machines. This is my dad's 1960 step-pulley Bridgeport with its OE 1HP motor. The workpieces are No.1 and No.2 style import (China) tool blocks for his Dorian CA (400) size QCTP. They come in just about .120" (3mm) too big to be able to drop a 1" shank tool down to center, so I mill .150" off.

The cutter I used is a 2-1/2" Widia 4-insert 45 lead face mill. I don't own a hardness tester, but my experience tells me these blocks from Tools4Cheap.net (http://www.tools4cheap.net) are up over 40rc in hardness. They may be just a very thick case hardening based upon the pattern left after milling, not certain.

I ran the cutter at 660rpm for an effective speed of 432sfm. The cut is about 1.5" wide, part is 5" long, depth of cut is .050" per pass. I think the feed rate (by hand, broken feed attachment) is about 6ipm, so it's a fairly light chip of about .002" per tooth.

If you have sound on, you can hear the cutter hammering the spindle a bit as it starts the cut, smooths to quiet as it cuts full width, makes noise as it passes over the dovetail cutout, and quiet again for the last bit until it breaks out the other end.

Hard_milling video (http://www.youtube.com/watch?v=WjmQl9ke7I8)

This video is short, just to try and show the finish after milling.

Results video (http://www.youtube.com/watch?v=ZYiP1UzCCLs)

Now here's the before and after (7 blocks, 21 of those passes) of the inserts. They are Valenite SEER43 AFER grade 5020. And they are incredible. Anytime you want to argue about the relative value a $13+ name brand insert vs. a $2 no-name insert, you only need to see the performance like this. A lesser insert would have been a chipped-up piece of refuse under these cutting conditions.

Before:
http://img.photobucket.com/albums/v466/kenm10759/Dads%20shop/IMG_1395-r.jpg

After:
http://img.photobucket.com/albums/v466/kenm10759/Dads%20shop/IMG_1396-r.jpg

Chips:
http://img.photobucket.com/albums/v466/kenm10759/Dads%20shop/IMG_1393-r.jpg

Comments welcome.

aboard_epsilon
08-27-2011, 04:43 PM
observations i made a long time ago ..

about the angle of attack ..cruelty to my milling machine and inserts..and how to over come it..

http://img.photobucket.com/albums/v190/aboard_epsilon/bridgeport/cutterpath2.jpg

i can see by the paternation on your piece that your are doing what ive crossed out in the top picture

i do the bottom pic ..less rattling ..less bang on the cutters..smoother finish....

ive not tried it on the hardened stuff ..but tried it plenty of times on all grades of stainless ..with good results almost mirror finish..and with cheap inserts.

you put the cutter in a position so the tips don't come off the work piece ..on the cut side ..when they re-contact ..they are on the previously milled side so no bang bang bang ..and spindle deflection ..and digging in causing scratches

all the best.markj

PixMan
08-27-2011, 04:56 PM
Well then what you see is not what I did. I did in fact set the Y axis to EXACTLY as you have it in the lower diagram, despite what your interpretation suggests.

You are 100% correct in doing it that way. That method puts the impact squarely into the "meat" of the insert where it has extremely high compressive strength. If I had done it the opposite way (your other diagram), the weaker sharp edge would strike the work first, and not wear as it did.

Thank you for bringing up an important point in face milling.

BTW, I believe what causes the hammering sound is that in certain zones of the cut, there's only one insert doing any work because of the width of the cut vs. space between inserts. Higher-density cutters (such as HSS shell mills) can be smoother-cutting because they've got so many cutting edges working at once. I suppose I could try my 6-insert 3" mill and see if it's any better.

PaulT
08-28-2011, 08:34 PM
Fellas-

What you are recommending is generally the opposite of what is recommended with carbide cutting tools.

Carbide tools work best with the initial chip load starting high and then transitioning to low.

If you do it the opposite way (your recommended drawing) the cut starts out with very small chip thickness, rubbing the carbide tool too much and wearing it out much faster.

This is the same reason that it is recommended to "roll in" an endmill into the initiation of a straight cut, it avoids starting out the cut with a small chip thickness.

Paul T.
www.power-t.com

PixMan
08-28-2011, 09:13 PM
PaulT,

I understand what you are saying and it is largely true. However, there are exceptions to every rule, and this is one of them. I recently had been given some Special High Intensity Training (you do the acronym) from a major carbide insert manufacturer, and this very subject was discussed at great length.

In a case like this where the cutter has to mill the entire face and the cutter diameter is not excessively larger than the workpiece, you're going to get a varying chip thickness no matter how you do it.

Try to picture the 2-1/2" cutter squat in the middle of the 1.550" wide work. The chip thickness is gradually thinner at both entry and exit of the cut, but thickest at the midpoint. Shift to one side by the maximum, and average chip thickness doesn't change by much at all. So in a case like this, and especially with upsharp edges in fairly hard materials, you'll get better life out of the inserts with the approach angle I used. That fact is borne out by the results I showed. If I was using double-negative inserts and cutter, what you are suggesting is exactly how I would do it. That takes horsepower this machine doesn't have.

FWIW, I did in fact try other ways before as I have done 3 other blocks in the past with the same cutter and machine (though different, flat-topped inserts.) I have also tried to get a "pretty finish" with a light finish pass, but all I got out of that was a pretty shiny finish for 3/4's of the cut and trashed inserts for the last 1/4. I rightly decided the bottom of these blocks didn't matter. If I decide in the future that pretty counts, I'll throw them all on the surface grinder en masse and do it nice.

P.S. - I always prefer climb milling with carbide. It's something you have to be VERY careful doing on a non-ballscrew machine!

Forrest Addy
08-28-2011, 09:16 PM
Yup. That's how it's done.

PaulT
08-28-2011, 10:08 PM
I could see that with highly positive inserts, it may be that the "start with the thickest chip possible" approach may not give the best results.

But I'm not sure even in that case that setting up for the thinnest possible initial chip thickness is also the way to go. Even with highly positive inserts, the radius of the cutting edge comes into play, if you start as thin as possible and are trying to start cutting a chip thinner than the cutting edge radius you'll just rub.

I'm assuming the inserts you used on that steel holder can't be super sharp, are they? Generally only special carbide inserts for aluminum are made with really sharp cutting edges.

Here's some more background on this issue.

http://www.myyellowcoat.com/featured-articles/rollin-technique-milling/

I've found the method describes above works well for me when cutting steel with carbide endmills on my not so rigid clone BP CNC mill. On that machine anything that makes cutting easier really helps.

Admittedly I haven't done much comparison with this method and facemilling so I'm curious about your results using an approach opposite to the above.

Paul T.
www.power-t.com

PixMan
08-28-2011, 10:40 PM
I think you can SEE my results in the photos I posted. Also, you can see the insert's edge. It's not dead sharp, it has about a .001"-.002" edge prep to it. However, with a 20 clearance angle and about a 12 top rake angle (owing to the molded-in chipbreaker), that should be an inherently weak insert. It's not bad at all, though I wouldn't bother with it on a CNC machine with 3 or more HP.

Fortunately, it's an incredibly good grade of carbide and multi-layer PVD TiAlN/TiN coating. In my close-up photos of the insert you can see that little edge hone (probably just erosion of sharpness from the coating process). You can also see that after 21 passes like the one in the video, the inserts aren't any worse for the wear. There's barely a discoloration of the coating.

Also take note of the chip form. It's beautiful, as milling chips go. If the cutter were struggling in any way or vibrating, you'd see it in rough-looking chips. The fact the the surface of the part looks somewhat torn is really the only confusing thing here. It feels quite smooth, and you don't feel any transitions.

You state that your machine is a CNC. That fact (ball screws!) allows you to do things I simply cannot do on the old manual Bridgeport. The whole purpose of this exercise was simply to show the many of us that have these old manual machines with little power or rigidity that the machines are capable of some pretty amazing things with the right tools. Think about how long that sub-one-minute cut would take with a HSS shell mill, if you could do it at all considering how close in hardness the part is, as compared to a HSS cutter.

Arthur.Marks
08-28-2011, 11:00 PM
Frankly, when you mentioned what you were doing, I was expecting a chipped insert :) I was a little confused by the two pictures until I read your full post. I say good going---and you've sold me on, "Anytime you want to argue about the relative value a $13+ name brand insert vs. a $2 no-name insert, you only need to see the performance like this." HAha.

aboard_epsilon
08-29-2011, 06:46 AM
You state that your machine is a CNC. That fact (ball screws!) allows you to do things I simply cannot do on the old manual Bridgeport. The whole purpose of this exercise was simply to show the many of us that have these old manual machines with little power or rigidity that the machines are capable of some pretty amazing things with the right tools..

Yes, the feedback in noise, vibration etc...then surface finish, because of this ..sort of teaches you what not to do on these old machines.

all the best.markj

PixMan
08-29-2011, 06:57 AM
It's nothing really. I've heard MUCH worse noises from fly cutters, boring heads and shell mills using HSS, but no one seems to think those are no-no's.

You cannot possibly judge the surface finish from the photo. It's really quite flat and smooth. It feels NOTHING like it looks. My dad's a retired tool maker, and I've been at this (on a full time basis in job shops) for over 30 years. If I were doing anything bad to his machine he would smack me in the head.

If you don't want to run tools like that on an old machine, that's a choice you are free to make. I am open to suggestion though, so I would appreciate hearing how you would remove that .150" (3.8mm) with that machine.

aboard_epsilon
08-29-2011, 07:05 AM
It's nothing really. I've heard MUCH worse noises from fly cutters, boring heads and shell mills using HSS, but no one seems to think those are no-no's.

You cannot possibly judge the surface finish from the photo. It's really quite flat and smooth. It feels NOTHING like it looks. My dad's a retired tool maker, and I've been at this (on a full time basis in job shops) for over 30 years. If I were doing anything bad to his machine he would smack me in the head.

If you don't want to run tools like that on an old machine, that's a choice you are free to make. I am open to suggestion though, so I would appreciate hearing how you would remove that .150" (3.8mm) with that machine.

I'm not having a go at you ..i believe and agree ALL what you say ..I'm just agreeing more , what you said in the answer you gave comparing CNC to Bridgeport manual.

BUT ..I'm not rich enough to spend that much on an insert ...no matter how good it performs....my tpun ones seem to break-up from fatigue and not from wear in the end .

all the best.markj

PixMan
08-29-2011, 07:59 AM
I guess I took your comment wrong then, and I'm sorry I misinterpreted.

I'm not rich enough for the $13 inserts either. They cost me...good will. The cutter(s) and a (potentially) lifetime supply of inserts were a gift from a friend who retired from selling them. All I had to buy was the R8 shell mill adapter. I know this something that few people get, but after running them like this I know I would pay for everything without question.

BTW, I don't think your TPUN inserts can "fatigue". AFAIK, carbide doesn't do that. There are different grades for different materials, but some are "more universal" than others. If you tell me what size you use, what materials you cut the most, I can help you find a "three dollar" insert (instead of $2 or $13) that might hold up to the chipping you describe. I know you don't have access to the same stuff we have in the North American marketplace, so I can find European brands.

aboard_epsilon
08-29-2011, 08:49 AM
Just had a look

SORRY

They aren't TPUN

They are TPU 322

Anyway ..they usually end their life by cracking up the middle .

This may be because, I didn't rotate them enough in the past ...meaning that they were becoming dull ..and when dull ..they get more of a shock loading in any slightly interrupted cut ...me being a tight wad ..tried to push them when they become beyond worn perhaps...I've since started rotating them ..and the problem is less ..get to use all three sides before they break up ..before ..i didn't get to use all three sides ..and realize now, to get the max benefit ..I have to start using the other sides sooner.

anyhows ..I've got something like 50 or 60 of them and they will have to be used up before I move on to something else ..

My milling adapter for them is about two inches wide and takes three .

ALL THE BEST.MARKJ

PixMan
08-29-2011, 09:14 AM
Well, they really are TPUN despite the package showing no "N". That last alpha character is the ANSI/ISO designation for "flat top, no hole".

They should fail at the cutting edge, never crack in the middle. If they are cracking up the middle and that's where the clamp lands, I suspect a poor seating surface and perhaps over-tightening of the clamp. Or perhaps just a REALLY brittle (low cobalt binder content) grade of carbide. Or all of the above.

flutedchamber
08-29-2011, 09:11 PM
I did a similar cut a few days ago on my Aloris CA 16 toolholder. It was .090 above center at it's lowest setting.

I squared it in my Bridgeport vise and used a 1/2 inch carbide endmill. The cutter lasted two passes taking .030 off at .375 wide @300 rpm.

Next I used a flycutter with a carbide unsharpened toolbit. Took a .030 cut at full width @400 rpm and got a smooth finish. No chipping of the toolbit, which surprised me.

Wish I had tried the flycutter BEFORE I tried the carbide endmill.