Help with Small Boring Bar

This is for a True Life Test I'm going to be running and I need some
advice from the people who have done this or think they have the
answer anyway.
My question is when you have a CNC Lathe set to Metric Dimensioning,
will it truly give you smaller increment control than if you have it
in INCH dimensioning. I would think that 3 decimal places in Metric
Mode is calculating at a finer resolution than 4 decimal places in
INCH Mode.
The last week of July I am traveling to New York to help with a
project that has a .019" diameter hole drilled in it and needs a
profile (radius-undercut recess) machined .004" per side into it,
about 1/8" inside the bore. The neck diameter of this tool is around .
010" and actually has what looks to be a helical flute on it for chip
flow, if you can believe it or not.
I had Performance Micro Tool make some sample of a boring bar to
formatting link
is their website. If you want to see some really
small stuff check out the site and look at NANO TOOLS button on the
left side of the page.
So my question is when I want to take depths of cut in the tenths (.
0001") and feedrates possibly in millionths (.00001") can it be done
in either mode accurately?
Thanks for the help in advance, it's greatly appreciated.
Reply to
Loading thread data ... get to do the fun stuff! No sarcasm there, I actually like that little stuff. Although, my eyes aren't what they used to be and I now have to use a 10x visor to make tools like that. Kinda nice to know you can have them made now, but I'm such a cheap bastard that I'll continue to make my own:-}
Yes. The control is capable of making accurate moves of .0001" & .001mm, as long as the machine can handle it. No problem on my Tornos. I run +/- 1 or 2 tenths parts all the time. Switch to metric mode quite often to get the 50 millionths adjustment.
Hope you have a tool presetter that's adjusted properly. Centerline will have to be absolutely perfect! If you have to center it on the machine, make sure you start below center, and work your way up. If it's above center in the slightest, the pressure at centerline (zero sfm) will snap it off.
Reply to
Matt Stawicki
JRWheels wrote in news:c1a3953c-8567-488d-96ae-
Yes, 0.001 mm = 0.000039" so the control is finer. Whether your machine can actually *move* that amount reliably is another ballgame altogether.
Reply to
JRWheels wrote in news:c1a3953c-8567-488d-96ae-
It truly depends on the control and servo drive/motor system. I have a machine in stock that has a 3" six jaw chuck that will run up to 15,000 rpm. The resolution of the machine is 0.01 micron. Or 0.00000039" if you prefer Imperial.
Anyway, you have to consider spindle run out and vibration as well. On the machine I'm talking about the spindle is better than 4 millionths. The chuck is a balloon chuck and is built in with no actuator to influence or vibrate the spindle.
The machine has nano interpolation. So the "pulses" or the minimum increment the servo motors are interpolated at is a nanometer (a billionth of a meter). With this set up there really would be zero difference between metric input or "inch" input.
Not knowing the machine, control, etc. it's hard to say for sure. If it is a late model Fanuc with nano interpolation or HRV control there is zero difference.
If it doesn't work out on the machine the customer has, I would be happy to arrange for you to use our demo machine for testing. With this set up there is as close to zero influence on the results from the machine tool as you can get.
Reply to
D Murphy
Thanks so much from all of you so far. It's a citizen L Series, fairly new.
The reason I'm not just sending the tools there for them to run them is I want to see the setup happen in front of me, how the centerline is set, etc.... so thanks for the tips.
I beleive the current process has a drill opening up the hole where this tiny boring bar is going into. I though about using a smaller dril like .015" have a .019" 3 flute mini endmill plunging in there before this boring bar goes just to true it up as nice as possible, thinking the boring bar will at least have an even cutting pressure while contacting the material for the first time. Thoughts ?
Dan, actually the last few places I have been to (out of Indiana) I have made sure the shops stop by and see you at IMTS.
I tell the story during the last IMTS when most all of the Swiss Lathe Manufacturers were showing off their Whirling Capabilities on Bone Screws, you said "here's you little crankshaft that we whirled" which I thought was pretty cool. I'm actually tired of seeing bone screws since I live in Warsaw. Ya know what I mean ?
Thanks again guys. JR
Reply to
JRWheels wrote in news:a6a7139b-f591-4b00-a7ab-
I'm assuming they are running fairly small diameter stock then?
Here is the issue with running very small parts on a 20mm machine: The distance from the collet in the headstock where the bar is actually chucked out to the end of the guide bushing is long.
If the bar is bent at all, the bar will run out more and more the further it is away from the guide bushing. So as they drill the small hole the drill enters a bar that is running concentric but as they feed the Z1 axis out the bar will run out more the further it sticks out. This causes the drill to be yanked around by the bar more the deeper it goes. Of course this does the drill no good at all.
Another problem is that if you run the bushing tight, the bar wants to bow in between the collet and the carbide in the bushing. This can cause the stock to stick then release which means the drill and/or boring tool can see wildly inconsistant feed rates.
Best bet is to use a Serge Meister brand guide bushing or at the very least hone the bushing being used with diamond lapping compound. The guide bushing needs to be snug but not so snug that the bar sticks.
The other tip would be to stick the stock out of the guide bushing using the Z1 axis (main spindle headstock), then do all of your drilling and boring using the X2/Z2 axes (sub spindle slide). This way the run out of the bar will have zero affect on your ID tools.
That sounds like a plan to me. Even a 2 flute would work well.
Thanks. I appreciate it.
BTW, it looks like we won the deal on the little hard milling job. I ended up taking the rough passes with the 1" end mill down to one pass per side from three. It didn't seem to make any difference in the sound of the cut. I also kicked the SFM up to 220 as I was seeing just the slightest trace of welding on the inserts under the microscope.
I kicked up the SFM on the turn to 400. I never would have thought to use the grade insert on my own. The finish at 0.0025" per rev looked like a rainbow. The insert seemed happy and could probably take a little more.
I hear you. I came up with the idea and one of our guys in our office here ran with it. Then he sent the tooling to CT to be put on the machine for the show. The guy who set it up "improved" the demo which amounted to tripling the cycle time. Sheesh.
Reply to
D Murphy

Site Timeline

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.