Starting a thread in position

[DavidB]

Hi guys whats the best way to get a Lathe Internal thread to start at a C axis position.

I have a job that has 3 Internal keyway which I broach on the machine at 120 degree spacing then the Thread must start in one of these internal keyways.

[Watcher]

Hi guys whats the best way to get a Lathe Internal thread to start at a C axis position.

I have a job that has 3 Internal keyway which I broach on the machine at 120 degree spacing then the Thread must start in one of these internal keyways.

 

Hi David,

 

I hope these formulas may help you to achieve it:

 

 

The translation was done by a German dude so it's not perfect... but basically where he mentioned "Position sign (Indicated point)" is the Z coordinate where the internal keyways are intersecting with the thread. This cycle was written for one of our machines for a very similar application.

 

I hope it helps...

 

Best,

 

 

(Edited: I removed the reference to my problem to put an image here - I was using ImageShack and getting errors from this board.)

[DavidB]

Not sure mate I use photo bucket and never have a problem.

 

Cheers Dave

[Watcher]

Not sure mate I use photo bucket and never have a problem.

 

Cheers Dave

 

Photobucket solved the problem...

 

Tks

 

Daniel

[crazy^millman]

If it has to be timed to an external feature and your machine has the ability to do threadmilling with the C axis I would recommend threadmilling it. That way you can time the external feature or cross holes to the exact place without hoping you can get some formula right that is going to lock you to a certain speed and feed on the threads. We use to make spray knozzels years ago and they had to be within .5 deg of print when tighten in place. Was a pain, but threadmilling everything made ti a breeze once we got the set-up right.

 

HTH

[Watcher]

If it has to be timed to an external feature and your machine has the ability to do threadmilling with the C axis I would recommend threadmilling it. That way you can time the external feature or cross holes to the exact place without hoping you can get some formula right that is going to lock you to a certain speed and feed on the threads. We use to make spray knozzels years ago and they had to be within .5 deg of print when tighten in place. Was a pain, but threadmilling everything made ti a breeze once we got the set-up right.

 

HTH

 

+10000

[DavidB]

It's a 4&1/4" x 3 TPI Acme Thread thats 4" deep

[crazy^millman]

David they make threadmilling tools for that, but not pratical. Then you might have to fall back to a threaded mandrel and thread the part on to it then do all the timing work to that fixture component.

 

HTH

[Bruce Caulley]

Dave,

On my little fanuc c-axis lathe I used to adjust the entry of a timed thread by changing the Z start point on the threading cycle. e.g. if I had a 1mm pitch thread that I needed to "rotate" 180 deg, I would add 0.5mm to the Z start point.

 

The only catch with this method is that it was trial and error for the first couple of parts. Not a problem on little stuff, but maybe you could use an acetal setter to get it right before risking the real job?

 

HTH

 

Bruce

[Watcher]

Dave,

On my little fanuc c-axis lathe I used to adjust the entry of a timed thread by changing the Z start point on the threading cycle. e.g. if I had a 1mm pitch thread that I needed to "rotate" 180 deg, I would add 0.5mm to the Z start point.

 

The only catch with this method is that it was trial and error for the first couple of parts. Not a problem on little stuff, but maybe you could use an acetal setter to get it right before risking the real job?

 

HTH

 

Bruce

 

The formulas above helps to make it right in the first shot. You can precisely calculate your start Z with them...

 

I admit I was skeptical about them when the WFL AE delivered the machine, but we're in the O&G business with very odd threads and often we have just one shot to make it right... and thanks to God the math has proved again to be of help...

 

The tutorial above was written and delivered with the machine for a part we designed for the machine acceptance...

 

By looking at the part drawing, you can see from where the values in those formulas were taken from and probably figure out how to do it in other circunstances...

 

 

 

 

 

By the way: The start Z there was a negative coordinate (-285) because we cut this thread towards Z+ - But the math works for all situations...

 

Cheers

Daniel

[Flycut]

I've just found out that you can control the start point of a thread in a G92 cycle using a "Q" value in .001 increments.

This controls the "C" position start point without changing your "Z" position start point.

The only problem is "Q" has to be on every subsequent line of the threading cycle or you end up with a double start.

Anyone know if this is possible in a "G76" or any other threading cycle?

[Colin Gilchrist]

Adding a "Q" value is fairly easy if you know how to edit a Post. I would use the Miscellaneous Real Numbers to set a value, and use that in the thread cycle output. I don't know if it is possible in any other thread cycle besides G92, but adding the functionality is super easy.

 

First, you need to add a Format Assignment line for the Misc Real that you want to use. In this example, I used mr5$:

 

fmt  "Q"  2  mr5$ #Angle output for G92 Thread cycle

 

Then you add the output of 'mr5' to the 'pthrg92_3$' post block:

pthrg92_3$	   #G92 threading
  copy_x = vequ (x$)
  pcom_moveb
  pcan1, pbld, n$, sgfeed, sthdgcode, pfxout, pyout, pzout, pcout,
    [if thdrdlt & thdpass$ = one, *thdrdlt], pfr, *mr5$ strcantext, e$
  pcom_movea
  prv_gcode$ = m_one

 

This will give you the Q value that you enter in mr5$. Note that you could potentially use any of the MR values, as long as the Format Assignment matches the MR you use in the output...

[slyym]

I've done something similar to what your doing and what I did was take 1 skim pass with the thread FIRST maybe like .005 deep or so and then time the keyways to the thread which is very easy then when you done broaching run the complete thread which should pick up the same lead. Easy pesy japanesey!!!