[spock]

Noticing something in my surface finishes. My diameters are great, very consistent, holding size very well. Also, faces are fine, good finish, holding size right on. But, when generating a radius or chamfer, I get little lines in my finish. It seems to be worse the closer I get to 45 degrees. I have tried leaving more stock for finish, slowing feed WAY down, no difference. I had to have the X axis drive repaired a few weeks ago, and I dont remember this happening before that. Spindle is running very quite and smooth. I wonder if there is something that needs adjusted to keep the X and Z axis "getting along", as they seem to be doing fine when moving alone, just not cooperating well and leaving little marks in part surfaces when moving together. I also tried G65, droop control, same results. Any ideas? Osp-500L control.

[OkumaWiz]

I have seen lines come from feedrate changing due to spindle encoder belt being shot and getting bogus rpm readings. Check that your spindle rpm looks consistent and try feeding in IPM to see if the lines go away. If that doesn't work, go to "Check data" watch RAPA (actual position), RCON (commanded position), & especially RDIF (difference between RAPA & RCON) to see if you have any "slip stick" going on. IF the RDIF is consistent and close to zero all the time, you're probably OK.

If both those check out then It's possible that something is not right in your drive especially since you just had it repaired.

Best regards,

[Algirdas]

could be friction jumps. Check smoothness ox axis with micrometer. Check if guideways are lubricated properly, check gibs tension.

[spock]

Thanks for the suggestions, guys. I had time to tear into it, pulled all the covers and found that the lube system was shot. No damage that I can see on the ways, but not enough oil for sure. I cleaned up all the check valves, ran new line (every single piece). Anyway, lines in finish are about 90% better, I can still see a touch of them. I will give it a while and if it does not get better I will re-investigate.

[Jashley73]

Just curious, what's the material, and what's your feed rate?

[Algirdas]

Could be wrong radius compensation (G42) settings, but the finish cut must be good in that case. Have You checked some 4 finish cuts? Actually, it's easy to see in animation, just magnify the area in question.
Is there any difference if you use G75/ G76 versus G02 G03 using G42 and without it?

[Green Button]

Possible causes:

1.Spindbe bearing (is there some noise ?)
2.X or Z axis ballsrew or ballnut ( is marks in work piece at similar distance?)
3. Rails or more common Rails sleds worn (marks are also same distance)
( if machine is not with linear rails, check wedges).
4. ballscrew support bearings at both ends

Put measuring clock to turret and try to move turret in different ways, there should be no gap.Use for example wood bar to get some force.
Important: clock could move little bit (0.02mm) but it should always come back where it starts. If not, you have found problem.

Also you could check turning surface carefully at x and z direction.
Very good to find if there is some problem is to machine (half) ball.You can easily see any marks there.


Hope that its only lack of oil. Thats cheap

[Algirdas]

I played with G42, G41 recently. I've noticed, that error of toll nose radius compensation can cause (rapid) toll tip retracts to wrong direction. It's eliminated on new controls already. I can check your part program on my lathe. Please, locate the piece of text with issue and I'll check.

[Jashley73]

I played with G42, G41 recently. I've noticed, that error of toll nose radius compensation can cause (rapid) toll tip retracts to wrong direction. It's eliminated on new controls already. I can check your part program on my lathe. Please, locate the piece of text with issue and I'll check.

Errors with G41/G42 tool nose comp, especially on the retract, is caused by a bad tool path, plain and simple. If you are feeding into a corner, and then the next move is a G0 G40 out of the corner, the tool will feed past the corner by the amount of the nose radius. This is caused by the control feeding the tangent point of the insert, to the programmed point, exactly as i's supposed to, while the tool nose radius is projecting ahead of that point. If you are feeding off the part, this is no problem.

However if you are seeing problems, the fix is to feed to the corner, then up/down the face by more than twice the cutter radius. This allows the control to look-ahead and comp the nose radius as it's supposed to. You have to be careful with the last move though. After reaching the corner, if you don't feed up/down the face enough, (more than twice the radius) as the control comps the tangent point of the insert to the programmed point, the cutter will actually move opposite the direction you intended - gouging back into the part - in order to put that tangent point of the tool to the target position. Again, the control is doing what it should, but the programmer/operator has failed to do our part...

If you use a radius to transition out to the retract, just make it big enough, (again, twice the nose radius or bigger.)
If not, you'll end up with a "Data word circle arc calculation error" alarm. The fix for this alarm, of course is to check the start points, end points, and radius. (I've also seen this alarm come up before for other tool path related mistakes, where G1 moves are so botched the control look ahead doesn't know what to do, but it's rare...)

Ask me how I know...

[Algirdas]

thanks, Mr. Jashley73,
the explanation is very nice. I wonder if there is nothing related to W and U (in LAP) ?

[Jashley73]

I don't think Spock's problems with finish/feed lines in his radius are related to his LAP turning cycles... I'm still curious to here what material he's cutting, and what his feed rate and insert geometry is...

While we're on the subject though, in case someone is having problems with their LAP programming cycles...

I've only ever had two problems relating to LAP cycles, and they were either typographical, or start point/end point related.

Here's a quick example of a couple examples of a rough-bar-turning cycle.

(LAP EXAMPLE PROGRAM)
N10 (ROUGH-TURN)
G0 G90 G50 S2000 M42
X100.
Z100.
T010101
S750 M3
X6.0 Z.25 M8
G85 NAT1 U.02 W.003 D.25 F.012 (ROUGH BAR-TURNING CYCLE)
NAT1 G81 (PART SHAPE/TOOLPATH)
G0 G42 X3. Z.1
G1 Z0. F.008
X3.2 Z-.1
Z-1.
G2 X3.5 Z-1.15
X3.8
G3 X4. Z-1.25
Z-2.
X5.
G0 G40 X5.25
G80
G0 X100. Z100. M9
M01

Typographical errors will most often come in the G85 line, or the NAT1 line. On the G85 line, the G85 word must come first, then the NAT1 (or N--) next. The control is very picky about this. The following U W D F words can be in any order, but the first two much be in order. For G85 & G86 cycles, you must have a D and F word in this line as well. If either the U and W values are Zero, they can be omitted if you choose.

The control is also very picky about the NAT1 line above as well. The NAT1 must come first, followed by a G81 or G82. A G81 specifies longitudinal (Z-Axis feed) cutting, and a G82 specifies traverse (X-axis feed) cutting. The NAT1, G81, and a (MESSAGE) are the only three things allowed on this line. The next line begins, the tool path shape designation. The G80 specifies the end of tool path shape designation, and is the only thing allowed on this line. Other typographical errors include negative values in the U W D F words, or a D or F word that is equal to zero. That pretty much covers the bulk of the typographical errors I've had before.

--------------------------------------------------------------------------

Start point/ End point mix ups will cause some funny problems, but are easy to fix... I'll use our example from above, but make some changes that will cause some silly problems once we cut a part...

(START POINT / END POINT PROBLEM EXAMPLE)
N10 (ROUGH-TURN)
G0 G90 G50 S2000 M42
X100.
Z100.
T010101
S750 M3
X6. Z.25 M8
G85 NAT1 U.02 W.003 D.25 F.012 (ROUGH BAR-TURNING CYCLE)
NAT1 G81 (PART SHAPE/TOOLPATH)
G0 G42 X3. Z.1
G1 Z0. F.008
X3.2 Z-.1
Z-1.
G2 X3.5 Z-1.15
X3.8
G3 X4. Z-1.25
Z-2.
X5.
G0 G40 X6.
G80
G0 X100. Z100. M9
M01

In the example above, on the line before the G85, we are positioning the cutter to X6. Z.25, as highlighted in green. From this point, we begin our rough turning cycle. The problem comes from the G0 G40 X6. line before the G80 line, in red. Once our rough cutting is done the G0 G40 X6. line will turn off cutter comp and rapid to X6., but this is the same position that we started from - and here's where the problem occurs, because we have specified in our G85 line, that we want to leave .02 stock on all the diameters, as specified by the U.02 in blue... What it does when our start
points and end points are the same, is actually cut material OFF the part by the U.02 (in blue) amount, instead of leave material like we want. I don't know why this doesn't cause an alarm, but I've seen this happen on several generations of Okuma controls, and haven't discovered exactly why and how to fix it until recently. The fix, easy enough, is to simply make our start point (in green) bigger, or the end point (in red) smaller - that's it. You can see this take place by watching position screens while running, or in simulations. The trouble it causes though, if you're not sure what's going on is sure a pain in the butt...

That's all I can muster up for now. I know I've drifted off point from the OP's question, but if I can help with any more questions, let me know...

[underthetire]

If your getting lines on an angle, but not on the face or OD, its one of 2 things. Stick slip, or drive tuning. You need to program a slow feedrate on each axis and see what the droop is (also known as LAG on every other machine) and see if the X and Z match.

[spock]

OK, after running a while now with the lube system fixed, I get same lines. There is oil everywhere! I also adjusted the X axis gibs, they were very loose. No change. I can run a 45 degree angle and watching the RDIF, at a very very slow (.001" per rev.) feedrate and I get about .002" in X, and Z value is up and down between what looks like zero and minus about .0023". As the RDIF value ramps up and down, the sound of the cut moves in time with it, and you can watch the chip change from thin/thick/thin in time.
Also, I can watch the encoder belt pully rotate when I cut the angle, and it is choppy motion, jerky. I watch the X axis and it is smooth as silk! I think Z is the culprit. If this is a tuning issue, can someone give me a place to start?

Also, for those who asked, it does this on plastic, steel, alum, etc..... at normal feed rates that would leave awesome finishes on a lathe running well. I have been running CNC lathes for 20 years, it's not a feed rate/doc/material issue. The RDIF value goes back and forth even when cutting air.

[underthetire]

See if the X and Z motors are the same and swap either those, or the BDU. If this is an early machine, Okuma also used shear pins in the axis coupling. I have seen those half broken causing similar issues, or the bore for the pins wobbled out.

[OkumaWiz]

Did you try it in IPM instead of IPR? This will eliminate the possibility of spindle encoder. Does Load for the axis also go up and down with the DIFF value? if yes check for mechanical binding.

Best regards,

[spock]

update: problem solved! Culprit was the Z axis motor. I removed it and when you turn it it was "cogging" or catching really bad. A buddy told me it might be shorted?
I found a used replacement (smooth rotation) and installed, smooth as silk now! Good thing is that all the stuff I fixed on the way to solving the line issue needed fixed anyway. Now I hope she will run a while.....