Hello Guest it is September 16, 2019, 07:06:25 PM

Author Topic: Problems threading on the lathe  (Read 330092 times)

0 Members and 1 Guest are viewing this topic.

Re: Problems threading on the lathe
« Reply #180 on: March 24, 2009, 06:47:27 AM »
This is from the TURN manual.......assuming it is still valid.

Offline ART

  • *
  •  1,698 1,698
  • Tough as soggy paper.
    • View Profile
Re: Problems threading on the lathe
« Reply #181 on: March 24, 2009, 08:34:53 AM »

  Index debounce will affect the sensitivity of the index signal. IT basically is how many interrupt periods the signal must be present, or not present before a change is actually sensed in that line. SO if set to 2 for example, when the index appears it will be ignored for 2 periods to make sure it isnt noise. Same with when it disappears. Setting debounce too high will make the index go away altogether.

  Since the length of the index is dependent on spindle speed, minimum length is variable, but the time must be at least 1 period at a debounce of zero. SO in 25000, thats 40us. The variation of 5RPM or so is really due to the CPU clock base changing, Im still looking into ways to stop that, but a 5RPM over 300RPM would be .6% of actual rpm being in error at maximum, so you may get a pitch variation of .6% , probably not noticable on the thread. For now, I wouldnt worry about rpm fluctuations if they are less than 2% of total. They should be mathmatically insignifigant.
   If a person notices a dropoff in RPM at a certain speed, they need usually a lower index debounce OR a wider tag. Index inputs from an encoder are usually pretty short and will limit speed readings at some point as you go higher.

  Im seeing quite a few computers that vary CPU clock rate these days, but most seem less than 2% , most less than 1%, so except in long threads this effect should be mimimal. My plan is to continue to work on that as we see what the effect is, so Id like some PP thread results before I jump into further strategies to make things tighter. The changes to MAch3 and the driver over the last few months introduced many errors that we're finally geting rid of, so Id like to see more empiracal results before moving deeper. It loosk like the SS can be considered working fine now, so as results come in on PP threading , we'll discuss the ramifications to the code and the varying CPU clocks happeing in the more modern CPU's.

Re: Problems threading on the lathe
« Reply #182 on: March 25, 2009, 09:29:06 PM »
tested the fix today.I had increased my hp on the lathe before and this made it possible to thread.
I backed off on the torque and no problem.The random x move is gone.I tried a 3/4  x 8 tpi
at 600 rpm and worked fine.I jammed a 2x4 under the spindle and slowed it down 50% and still ok.
good work on the fix!
Now I have another trying problem,getting my spindle to stop with the same orientation every time?

Offline RICH

  • *
  •  7,358 7,358
    • View Profile
Re: Problems threading on the lathe
« Reply #183 on: March 25, 2009, 10:25:10 PM »
"getting my spindle to stop with the same orientation every time?"

Not sure what you mean.


Offline Chaoticone

  • *
  •  5,589 5,589
  • Precision Chaos
    • View Profile
Re: Problems threading on the lathe
« Reply #184 on: March 25, 2009, 10:29:51 PM »
Rich, he is wanting his spindle to stop and orient, like a mill has to do when using auto tool changer. This is critical on some jobs (like being loaded and unloaded for a second op by robot). Think you will need to use an encoder or possibly just a custom macro, prox switch, and a brake.  Really need to start a new topic for this.

« Last Edit: March 25, 2009, 10:31:31 PM by Chaoticone »
;D If you could see the things I have in my head, you would be laughing too. ;D

My guard dog is not what you need to worry about!
Re: Problems threading on the lathe
« Reply #185 on: March 25, 2009, 11:03:59 PM »
Yes I don't want to hijack this thread only a passing comment.This
has been one of the more interesting problems and I'm sure more to come.

Offline RICH

  • *
  •  7,358 7,358
    • View Profile
Re: Problems threading on the lathe
« Reply #186 on: March 25, 2009, 11:38:58 PM »
No problem. So to get this back on threading.

Like, how to pick up a cnc thread once the spindle has been stopped and the piece removed.
Or you stopped the spindle and just want to check the thread anad adjust or take another small
cut. We got it down to a small error just need to think about it some more.

We'll play around a little more than maybe i can ask just right question to Art.


Offline Hood

  •  25,849 25,849
  • Carnoustie, Scotland
    • View Profile
Re: Problems threading on the lathe
« Reply #187 on: March 26, 2009, 03:24:50 AM »
 possibly using the start angle feature would be the way to pick up on a thread, think Art would have to give you some way to determine what that start angle would be and it doesnt sound like it would be a five minute job to do that but Art has got things working well so far so you never know ;)
 If there was a way to stop a thread halfway along a pass in a controlled manner then it would probably be easy enough to pick up, you would just start the threading move, have it stop, move out a bit on X and then put the thread in the chuck and jog in on the X and rotate the thread until the tool lined up and tighten the chuck, sounds simple but dont think it will be ;D

Re: Problems threading on the lathe
« Reply #188 on: March 27, 2009, 06:04:04 PM »
Success,          I had a chance to try out the new version today, and although I only had time to cut two threads they both came out great.  I am using the P. Port, and I am not sure if anyone else had had success using the PP, but it worked great for me.  I cut a 1/2-13 in delrin, and a 1/4-20 in cheap alum, and both are beautifull.  Thanks to Art, Brian, and everyone else who had a part in finding, and fixing the problem.  If nothing else it will  make us all appreciate threading a little more than we would have otherwise.  I know I just stood in amazement watching while a thread was cut in a dozen passes just as I had hoped, and with no extra funny moves in between!  Thanks!!!

Offline RICH

  • *
  •  7,358 7,358
    • View Profile
Re: Problems threading on the lathe
« Reply #189 on: March 27, 2009, 07:19:11 PM »
So your done threading a piece and your not satisfied or maybe you just want
to tweek it some, maybe the piece has been removed out of the chuck or you just tried the nut and it's tight.
You can pick the thread up in cnc if you wish and tweak it.

Now just make note that threading depends highly on the mechanical aspects of your
lathe. You can tweek either side of the thread flank or follow the minor diameter lead depending on how you want to pick up the thread.

I am only using a single slotted disc. I align / center the slot to the pickup. Placing an fine scribed line on the disc as a reference would be even better.

The thread has been cut. Before you remove the piece align / center your index slot
and then place a very fine witness line on the piece with the cutter.

The following applies if the piece "has not been removed" from the machine.
The spindle is off, the cutter tip is not in the thread.
1.Align the disc slot to the pickup.
  - If your in MachTurn you may want to use the MDI line for a G80 & G94.
2.Move the thread cutter tip into alignment with the point you wish to pick up.
  - You can use the root at minor diameter of the thread V, front or back flank of the V,
     or even center the cutter tip with crest of the thread.
  - Zero the Z axis DRO
 Note: Move to your point such that backlash is taken out. Here is were that MPG
          with a nice feel and movement comes in handy. I have a 30x microscope attached
          to my lathe so that is a great assist also.

3. With the cutter out of the thread, now make - Z move in increments of the thread
    lead. ie; for 20 TPI you will move 1/20= .050 increments. You should move beyond 
    the end of the shaft by approx  3 to 5X  the lead ( ie; 3x.05=.150"). Single start
    thread so pitch =lead.
  - Zero the Z axis DRO

4.Make an additional negative Z move and return to Z=0 to remove any backlash.

5. With spindel on, now do a G32 -Z *********x  F.050 from Z=0 where *********x is some length of
    the thread and F value is the thread lead.
    - Turn off the spindle, G80 & G90, MDI to Z=0
6.Align your disc slot, do MDI moves in lead increments and see if the the cutter tip aligns      with the pick up point.If all alligned then no need for a Z adjustment. If not adjust the Z    start  value by the amount you may have needed to move to get into alignment with your    chosen point.
Now you can do G32 moves to accomplish what you want to do.

What you have done is the equivilant of picking up the thread on a manual lathe with an indexer dial. This dosn't take 5 minutes, and if you know what your doing it is rather quick to do. Simply put, you have closed the half nuts, picked up the thread using the coupund slide, tested it by dry running.

This applies if the piece has been removed from the machine.
1.Align disc slot.
2.Put the piece into the chuck and align the cutter to the reference line you put on the   piece. 1 & two must match.
3. Now do the same as if the piece wasn't removed.   

Sorry for the detail and hope it's right. My testing showed this to be accurate.