lathe question for ya'll...

Yesterday I was hardcutting stainless on the new lathe, holding extreme tolerances. What I ended up with was the diameters were insanely perfect,
thru 45 pieces (3hrs), the lathe held +-.0001 on a diameter no problem. But the Z wasn't so good. It was strange, the spread from shoulder to shoulder was changing. An example is a shoulder 1.5" from the front. It floated +-.0002. That's strange because the front shoulder repeated on location to within a tenth all day. Same conditions on all the shoulders, taking approx .005/side off. No insert wear whatsoever, im using coated cbn inserts and these things do not wear ever. Everything is real rigid.
Now, my question is are lathe's more accurate in X due to maybe the spindle bearings? The Z axis is pushing on the bearings strait in? Is what I'm getting normal?
Variable: Our lathe chuck is fuxored up, samsung is coming out today. With a gage pin clamped in previously bored steel jaws, boring .3 deep, the gage pin in the chuck all the way to the cut so it's almost clamped on the whole length of the jaws. 250 whatever clamping pressure. I bore and without unclamping it I get .0002-.0003 tir. That should be zero, I never unclamped the chuck? Plus it bounced my indicator a tenth or two. Then unclamp and clamp on that gage pin again and it goes anywhere from .0007 - .002 tir, and each jaw is different. So, maybe this crappy chuck is effecting my accuracy in Z????
Any advice on this matter would be appreciated.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

cutting dry or coolant. If dry, I'd second Gunner and say thermal growth, either the part or lathe iron or ballscrew.
Thank You, Randy
Remove 333 from email address to reply.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Randy wrote:

Vinny, I'm going with spindle growth also.
While the insert might not have appeared dull I'm wondering if it wasn't a bit dull and not cutting when it came to the step before it took off in X?
Ive seen this at times on lathe work that we do. I've corrected this by putting a slight dwell in if the Z lengths are critical. In Fanuc language I would put a G4P100 which gives me 100 milli seconds of dwell. Depending on Parameter settings on a Fanuc you can also give it so many revolutions before it takes off again.
Best, Steve
--


Regards,
Steve Saling
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

RPM's ? The highr the r's, the more likely the jaws can be pulled out by rotational force, and if the chuck has some face runout, and or slop against the mount, the higher rpm will show in runout on the part.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

RPM's ? The highr the r's, the more likely the jaws can be pulled out by rotational force, and if the chuck has some face runout, and or slop against the mount, the higher rpm will show in runout on the part.
********** Thanks to all 3 of ya lol. Ok, the rpm of the chuck is a non issue since I havn't gotten a grasp on how css works on mastercam, so I'm programming strait rpm. The spread on the shoulders were cut at the same rpm, so that rules out runout from rpm increases.
As far as dwells go, I programmed a few extra grand of radii' in the corners, so there is no line/line on corners. Works for milling, I figured it would work for lathe?
As for dull....prolly not. In fact, I wasn't hardlathing, i was just lathing. that insert cut like it was 20 rockwell. Mitsubishi cbn, coated cubic boron captain kirk shit. This insert is insane. It has no chipbreaker, but for a 5 grand cut in 60 rc stainless, it cut like cold rolled on the best carbide insert.
Running wet. Why:? Dont know, the best I could get from the mits website was dry on non interrupted, dry on interupted, 700-800 sfm, .005 per inch. thats hauling AZZZZZZZZZZZZZZZZZZ!!!!
Damn, that might be the most accurate thing I ever cut in my life. On a damn lathe!
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

correction due to drafts for 99 cents at winghouse
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Definately something wrong with your chuck. On one of my wornout Autobloks, the most variation (from open/close/open/close) I will get is .001. This is a chuck so worn that the jaws will move out .005+ when clamping.
Variation of Z value most likely from some thermal change. Spindle, bearings, ballscrew, headstock, bed casting, etc. Not fun to locate it because it might be one thing today and something else tomorrow.
--
Remove "nospam" to get to me.

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

Vinny is running a brand new machine. Having dealt with the Taiwanese and the junk they call machines for years I can say that brand new junk is still just junk. Buy a machine from Mighty if you need proof of that. Complete crap, even with the latest control's from Fanuc. Complete shit, IMHO. That is probably his problem. Well, that and he smacked the chuck......
OTOH, I just spent a month working with a YASDA H40i. Holy shit Batman!
Milling at plus zero minus two tenths all day long and the H40i isn't their "high precision" machine. I'll be working with one of the "high precision" baby's next month.
--
John R. Carroll




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

Now wait, this is korean....uhhh, nevermind. :(

Well, seems the korean chucks are cheap shit. The samsung guy says we need a japanese chuck to hold a tenth all day long, so it seems thats the path we will go down. Sad theres no American company? Wtf. What happened to kalamazoo chuck company? I always heard they kicked azz???? This is the age of buy American, Someone, quick, help me out! Screw these asians bafoons!

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

Try ProHold or Microcentric. I think they are still made in America.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Vinny, whats the issue with CSS in M/C?
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Vinny, whats the issue with CSS in M/C?
****** I don't know.... It has a spindle setting, and a max spindle setting, and a css/rpm switch. Ok, so I set it on css. Type in the rpm I want of the largest diameter. Then I type in a max rpm. Whatever I type in, it uses for the rpm in the gcode. Sucks considering the default was 5 grand and stupid me...lol, good thing i'm cautious, lets just say that.
I just don't have the concept yet, I only programmed 4 proggys so far, the front and back both soft/hard. Went good, I just typed in the same number for max rpm and rpm. I'm not even sure it slowed down at all on the small diameters, I dont think so. I think it ran 1800 the whole way thru. Maybe you can explain what I'm doing wrong. I got the max rpm gimmic, but I don't get the rpm css deal, how does it know when to go that fast? If it asked for a surface feed I can see how it would know how fast to turn, but how does it know at what diameter I want it to go that rpm?
HEY! Stop laughing! :)
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

***** CORRECTION:
First time I ran the conversational I didn't know to set max rpm, it defaulted to 4 grand, top speed. So it cuts good in the dryrun and first piece because I was paranoid holding the rapid to 5%, then I dropped the rapid to 100% and hit go with no worries. WHOLLY CRAP that spindle went to 4 grand instantly while it rapid'd at light speed. DAMN THAT SCARED THE FUIODP:PJJT OUT OF ME!
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

if the output is correct, you should have something like so: G97 SXXXX M03 fire up spindle G50 S2000 set max rpm at 2000 G96 S400 set constant surface speed to 400 sfm.
RPM's will change according to dia being cut, based on X value, up to 2000 rpm
G50 is your friend, or your biggest enemy if you forget to keep it real.
Check your job setup in M/C to set your max spindle RPM for your post.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

if the output is correct, you should have something like so: G97 SXXXX M03 fire up spindle G50 S2000 set max rpm at 2000 G96 S400 set constant surface speed to 400 sfm.
But mastercam never asks you the SFM? It asks rpm, and max rpm? hmmm, I will look at it again....
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

you can switch between CSS and RPM on that line in the parameters, take another look. :)
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

you can switch between CSS and RPM on that line in the parameters, take another look. :)
************
Ok.... I click on css. I type in 1000 for spindle speed. I type in 4000 for max spindle speed.
That's all there is. There is no SFM question anywhere. So my question is how does it know what diameter I want to run at 1000?
Even if when I clicked css the spindle speed is ignored and it only uses Max rpm, it still needs a SFM number? Unless... It gets its number from the stock setup for steel type. That has sfm numbers in it.
frig... I think I got it. So by clicking css, it ignores rpm and uses the sfm in the stock setup and max rpm? Am I right?
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Not having ever used mastercam, I don't know what their mathod is, but in Edgecam when CSS is activated the RPM (you entered) becomes SFM.
Edgecam has the ability to determine the correct RPM at the point where you want CSS to take over.
Example: Assuming G97 active (default setting) G41 (gear select) M03 S179 (speed at 8.4 inch dia. to make 400 sfm.) G0 X8.4 Z5. T505 G50(G24/G92/G_whatever control uses for max speed) S198 G96 S400 (calls for 400 sfm.) blah blah G97 S179
--
Remove "nospam" to get to me.

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

So, if I hear you right, you are hard turning at 1000 sfm? Both M/C and your machine will conceivably max the rpm if the diameter is small. http://www.tapdie.com/html/sfm_to_rpm__surface_feet_per_m.html As you can see on the chart, if your cutting a 3/4 diameter, at 1000 sfm, your spindle will want to be at 5089 rpm, if your max is 3000, you have pinned it. What you are seeing in Mastercam output is the result of your ###'s for css and the dia you are cutting, calculated in M/C, for a cheap thrill, change your css to say 350, post and check the starting rpm that it spits out, now we are at 1781 rpm, takes a little getting used to, but once you can trust the #'s, it gets a little more comfortable, a little.
Alphono's example is dead on to what MC will post out
Going back to an earlier subject, I have made the switch from MC 9.1 to MCX, and quite frankly, I like it, there are some features in X4, MU3 that have already become second nature, for the life of me, I have no idea why JB has so many problems with it!!!
"D"
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

You'll run into serious problems when you tell Mastercam to select all of those .1875 holes, and it only selects the .1875 holes and not the . 1873 holes. Just wait and see. You'll be back here ranting and raving with a pizza & literature filled briefcase in no time! LOL!
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.