Finish issues with tiny boring bar in 4140HT

[Eric U]

Update.

I spent a few hours yesterday trying to implement some of the suggestions listed above. I dialed in the orientation and center height of the insert as best I could. No change in finish. I also tried upping the speed/feed/DOC but that didn't change anything.

Today I threw a different boring bar in the machine, and it worked like a charm. 45/45 parts were on size first time...no scrap. The finish was like glass for the first dozen or so parts and then gradually took on a matte finish. No issues with BUE, smearing, chip packing, or other major calamities and thus the parts were still good. Progress! I kept the speed/feed/DOC changes from yesterday and they will at least cut down some on cycle time. Looks like I owe Frank a beer, as it does indeed look like the insert pocket was loose.

I'm still looking forward to hopefully hearing from Kyocera tomorrow on the cermets. I'm definitely curious.

Anyway, up and running again so that is a good thing.

Thanks for all the suggestions!

 

[fmari --MariTool-]

" Looks like I owe Frank a beer, as it does indeed look like the insert pocket was loose"

Yep, been there, done that. You really need to baby those small indexable boring bars. Problem is you torque those screws a little too much and they dont come loose or strip. Too loose and the insert moves within the pocket giving you different diameters and depths on the part. Glad to help.

I used to run a shit ton of small brass fittings. Other than the od turning, threading, and grooving tools my entire turret setup was all solid carbide. Nothing indexable. Ground my own trepan tools, rolled my own radiuses with a 600 grit diamond file and oil. Sometimes finished up with a stick of wood and paste for a really fine finish. Ran lights out for years with minimum maintenance.

 

[thermite]

Update.

I spent a few hours yesterday trying to implement some of the suggestions listed above. I dialed in the orientation and center height of the insert as best I could. No change in finish. I also tried upping the speed/feed/DOC but that didn't change anything.

Today I threw a different boring bar in the machine, and it worked like a charm. 45/45 parts were on size first time...no scrap. The finish was like glass for the first dozen or so parts and then gradually took on a matte finish. No issues with BUE, smearing, chip packing, or other major calamities and thus the parts were still good. Progress! I kept the speed/feed/DOC changes from yesterday and they will at least cut down some on cycle time. Looks like I owe Frank a beer, as it does indeed look like the insert pocket was loose.

I'm still looking forward to hopefully hearing from Kyocera tomorrow on the cermets. I'm definitely curious.

Anyway, up and running again so that is a good thing.

Thanks for all the suggestions!

Here's one more:

QC problems ages ago dropped dramatically when the "FNG" bought about thirty 20 power binocular and 40-power MON ocular Bausch & Lomb Old Skewl purely "optical" "bench" microscopes. So folks coud SEE WTF was afoot.

The modern-day equivalent can be a "live" camera system. And MANY of us can benefit from that sort of magnification for routine, not just problem analysis, at far lower cost than prevailed "back in the day"

EG: Had you the bionic "vision"? You'd have SEEN the insert could - and did - shift in the pocket as it was torqued or had done after you ran it, then had to pull tool - observe what had changed.

Scrap cost reduced/avoided, time and head-scratching saved chasing it?

Wudda paid for the "eyes", first time, right outta the box.

Horses for courses...smaller OR larger(deep, DEEP, space telescopes? SEM's?) s**t gets than sumthin' to see, go fetch, then EAT?

The more crutches we "eye brain not nose-brain hunter gatherer" omnivore humans need.

Design AND evolution thing.

"Augment what you got!"

 

[Oldwrench]

Got here late; thanx to Jashley for giving me a heads-up. I agree with Frank 100%. FORGET insert bars for any hole smaller than 1/2 inch or thereabouts, there's simply not enough mechanical support for an assembled cutting tool. Either the little screw loosens, or it's a gnat's eyelash away from stripping. And as for adequate damping via contact with the insert, you're lucky if it actually touches more than 10% of the pocket. We use solid carbide bars for a lot of tiny stuff, including boring recessed center holes for parts to be ground. It's got to the point I only keep the Darex endmill grinder around so I can offhand-sharpen those tools (it happens to have a diamond wheel on it). Solid boring tools are like turning back the clock 100 years but solidity is a hard property to beat!

I have never tried any Kyocera solid cermet or ceramic bars. Micro 100 has always worked for us in 4140.

 

[Eric U]

Following up on this thread after having made over 6000 bushings since the 2nd week of January.

-I tried the small solid bars, but they just wore out too quick to be economical. I tried Frank's and a couple Kyocera solid ones I got as samples.

-The quality of the small inserted boring bar matters. I tried a few different ones (5mm) and the carbide Kyocera EZ Bar Plus has been the winner. They are pricy, but have lasted more than 4x as long as the previous one I had been using that cost 80% as much. Even the insert screws and torx wrench Kyocera supply are far superior to the other ones.

-Holding small boring bars in a collet is for the birds. I broke down and spent big bucks (to me) on a Kyocera boring bar sleeve that is made to work with the EZ Bar Plus. The boring bar has a flat on top, but also an angle ground into the back of the bar that mates up to a pin in the sleeve to ensure proper alignment. The sleeve also has two coolant holes that aim straight down the boring bar and flow well down into the hole.

-I'm so happy with the 5mm setup that I also bought a 4.5mm version for my smallest holes (less than .251"). Love it.

-The vast majority of my parts are in the .251"-.375" sized bores. For these bushings I started running a roughing boring bar and then a finisher. This cut way down on the scrap and produced pretty good finishes. I'd run new insert edges on the finisher, and used ones on the rougher. The first 10-15 parts would look like glass and then gradually the finish would start to look slightly matte, but still smooth. When I'd get too many that had poor finish or were scrapping parts on size I'd swap edges. I could usually get around 50-60 good parts on a finisher edge this way, but with a scrap rate in the 10-15% range. Better than before but still not great.

-While the Mitsubishi inserts I started with worked better than other options tooling reps sent me to try, I was still not happy with the scrap rate. A couple months ago I ordered some Kyocera cermets to try out. Unfortunately Kyocera had to make them since they didn't have any in stock...and it took nearly two months to show up. Today I got to try them for the first time. Winner! My scrap rate wasn't perfect, but at less than 7% over 215 pieces, I was quite happy. I was still running the Mitsu inserts as roughers and the Kyocera ones as finishers. The finish was absolutely superb. I swapped out the first edge after 108 good parts when I got even a faint hint of tooling lines in my part. They were still better than all but maybe the first 2-3 bushings on a new edge with the carbides. I could have probably run it longer. Its funny, these are uncoated cermets, but its almost like they need to break in a little bit before they settle in. Out of the 215 parts I made today, my scrapped ones were 90% in the first 20-30 bushings on a new edge. After that it was magical. Good news is these cermets actually cost less than the carbides they are replacing...if you can wait the 8 weeks. I think it is just because I was using the smallest insert they make and they probably don't sell that many.

-So, in conclusion: Kyocera carbide bar in Kyocera sleeve with Kyocera cermet, with a rougher run before it. That's what I'm running with from now until this contract is up.

Thanks for all the help and suggestions!

 

[Milland]

Thanks for the update!

 

[Orange Vise]

-So, in conclusion: Kyocera carbide bar in Kyocera sleeve with Kyocera cermet, with a rougher run before it. That's what I'm running with from now until this contract is up.

Looks like a pretty solid process.

If you get another contract, consider taking a spring pass with the finishing bar to some predetermined, undersized ID. The finish might suffer, but then hit it with a Cogsdill roller burnisher to get the bore on size with a much better finish.

Also, any chance the customer would take a 4140HT substitute? Niagara Lasalle etd150 is a lot more consistent than generic 4140HT with very similar properties.

 

[Mike1974]

I didn't read all, so apologies in advance if I repeat other suggestions.

Solid carbide bar, "upsharp" insert (polished, high rake)... Circle makes some good bars in my experience in the 3/8" and under range.

 

[Dan from Oakland]

If your tolerances are real, and need repeatability, honing would probably salvage a lot of your scrap. A few swipes on a hone and a few tenths later you would have a perfect finish and to size.

 

[implmex]

Hi Dan, and all others who have made these kinds of recommendations:
The OP has a bazillion different sizes to make, so diamond honing, roller burnishing, ballizing etc etc are all expensive to implement and seemingly not very practical for the quantities of each he has to deliver.
Here's a snip from Post #1:
Material is 4140HT. My machine is a Doosan Lynx 220 LYA. The part is .5" OD and the ID varies from .221" up to .375", with about 130 sku's total. Because of the number of sku's the bores are made by boring.


So boring it probably has to be and has to remain unless there's enough meat in the project for internal cylindrical grinding.

Fortunately the OP has found a solution he's satisfied with.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

 

[CBlair]

I never had good luck with 1/4" or smaller indexable boring bars. Insert moves in the pocket. Looks like that is what is happening to you. Check out internal tool and Micro100, they have some nice solid carbide boring bars. Also this would also work...

Multi Extension Boring Bar 3/16 Shank X 2.0 Long X .007 Radius MariTool

I used your tool for a job that came up recently and it worked great, small deep flat bottom hole in SS with a thin wall. That tool saved my hair...ha ha.

Charles

 

[fmari --MariTool-]

Awesome to hear !!

 

[EmGo]

The finish might suffer, but then hit it with a Cogsdill roller burnisher to get the bore on size with a much better finish.

No, no, no. Roller burnishing does not work this way.

The size of a roller burnished hole is totally dependent on the pre-burnish size and finish. If your pre-burnished size varies, then so will your post-burnished size.

The preburnish finish is also important. It has to be controlled and the right roughness. Just like with thread rolling, the material has to have some place to go. Too rough or too smooth and you won't get the size or effect you want.

Roller burnishing is not a magic tool, "just push this thing through there and the bore will come out on size and shiny too !" In fact, it's harder to control than several other methods. Not a good idea for this part, not at all at all.

 

[Orange Vise]

No, no, no. Roller burnishing does not work this way.

The size of a roller burnished hole is totally dependent on the pre-burnish size and finish. If your pre-burnished size varies, then so will your post-burnished size.

The preburnish finish is also important. It has to be controlled and the right roughness. Just like with thread rolling, the material has to have some place to go. Too rough or too smooth and you won't get the size or effect you want.

Roller burnishing is not a magic tool, "just push this thing through there and the bore will come out on size and shiny too !" In fact, it's harder to control than several other methods. Not a good idea for this part, not at all at all.

Doesn't matter anyway because I missed the part where the OP had 130 different SKUs.

Nevertheless, let's pretend he only had one SKU. I am curious as to why you think the method I outlined wouldn't work?

The idea was to decouple sizing and surface finishing. When you combine the two together in a single finish boring operation, you basically only have one shot because the insert requires a minimum DOC. A spring pass can get your ID tighter, but you end up with a matte finish unless the material is HRC45+ (OP's is not, closer to HRC25-32).

So the procedure would be as follows:
1. Drill
2. Rough bore
3. Finish bore
4. Finish bore spring pass(es)
5. Roller burnish

The pre-burnished bore would be held to a tight, repeatable tolerance and surface roughness. Exact diameter would have to be dialed in through trial and error.

 

[Rogue_Machinist]

Typically when I run 4140 under .375" its going to be 1700 RPM at .003"/rev and leave .002" finish. And I get a decent finish on 4140 and 4130. Im also using solid carbide boring bars.

 

[EmGo]

Nevertheless, let's pretend he only had one SKU. I am curious as to why you think the method I outlined wouldn't work?

Because I've done roller burnishing ...

The idea was to decouple sizing and surface finishing. When you combine the two together in a single finish boring operation, you basically only have one shot because the insert requires a minimum DOC. A spring pass can get your ID tighter, but you end up with a matte finish unless the material is HRC45+ (OP's is not, closer to HRC25-32).

So the procedure would be as follows:
1. Drill
2. Rough bore
3. Finish bore
4. Finish bore spring pass(es)
5. Roller burnish

The pre-burnished bore would be held to a tight, repeatable tolerance and surface roughness. Exact diameter would have to be dialed in through trial and error.

The pre-burnish finish has to be rough. It cannot be smooth. But it also has to be consistent, so "rough" is not a good word to describe it either.

You know the wave borders on Greek or Cretan wall frescos ? The ones that look sort of like a 60 hz oscilloscope trace except not as tall ? That's what you need for roller burnishing. Like thread or gear rolling, the tall parts get pushed into the low parts. You don't want a matte finish or a shiny finish, that doesn't matter, what you need is a controlled surface like a full-round tool at a high feedrate.

If any of your parameters is off - size or finish, then your burnished hole will neither hold size nor will it get the hardened burnish effect.

It's actually pretty difficult to do correctly. I know the literature does not sound like this but if you actually buy a tool, try it, fail and call their tech people crying "Why are my bores burnished with your tool such shit ?" they will explain it to you.

In the end, I got it working (bearing bores in aluminum hubs in this case), but it was not the free-and-easy size control that the literature leads you to believe. For just size and roundness control, honing is so much easier and more predictable.

 

[CORONA VIRUS]

If you don't take enough of a cut your going to get a lousy finish.
If you don't take enough of a cut your going to be rubbing and wearing our your tools edge.


CCMT is nice and sharp, stay away from coatings as the reduces sharpness.


Something that small...I'd give a solid carbide bar a try. It should hold up well in 4140, very sharp and the size you need is right in line with insert cost. True you'll need to adjust bar compared to changing inserts...but if it works they have them with holders and flats that are quick to replace after the bushing is set...just release set screw to move bar and screw orients the bar.
Mari sells the standard boring bars as does Lakeshore and others.

We do a bunch of small tight tolerance jobs and that is my guys go to for Alloys, SS 316 etc. In 4140 I'd expect it to hold up for a minimum of several hundreds parts. Just going to have to find that sweet spot of cutting enough not to start rubbing and wearing the edge...but not pushing to chip edge with required finish.

But that's alway the trick to machining.

Correct on the DOC. 4140ht likes a deep doc for a finish pass. Don't be afraid to take a .015-.03doc. Try a cermet grade. Get rid of that .008"rad insert and use a .0156"rad. Increase your sfpm if possible. Also correct is no coatings on small diameters. You want to increase the heat to get a nice finish on 4140ht. You will never get the sfpm you need with coated inserts and small diameters. Also, with small bars, they will twist. You you want to run off center about .01" so when the bar does twist the tip ends up on center.

 

[Eric U]

Hi all. I do appreciate the continued interest in helping me conquer my small bore issues. I came back here last week (post #25) to tie a bow on it. I’ve got it “solved” good enough.