Lathe Threading Question

[Greg_J]

Hello,

I've been threading parts but if I change the rpm and re-run the part to get rid of chatter the machine looses pitch, I didn't actually do this cause I knew before hand that this will happen.

 

My question is why? and is there a way to change the rpm and re-run with out loosing pitch? Is there any relation to the rpm and start point?

 

I ran a lathe with a Heidenhain control on it and before the threading cycle I would put a code to set the spindle orientation to 0 then the machine always new where the start of the thread was, just like a mill doing rigid tapping does internally.

 

Does anyone know the codes to do that on a Fanuc?

 

I'm using a Doosan Fanuc i series(not sure where to look to get more specific Fanuc info).

I have two lathes with live tooling and two with out I'm sure the ones with live tooling have the options to do this cause you need to control the spindle (c axis) to do milling.

 

Anyway any help is appreciated.

 

TIA

 

Greg

[SlaveCam]

Completely agree that this is a major annoyance on Fanuc lathes. I have asked this exact question on another machinist-related forum years ago, but never did get any info on how to adjust the starting Z point to adjust for the new RPM. There has to be some formula, I'm sure of it. I'd love to know it myself!

 

What I've had to do, if needed to lower the RPM to reduce chatter, is use radial infeed in threading and watch closely that the threading inserts begins to track the existing thread and adjust Z accordingly if not...

[Machineguy]

Unless your on a manual lathe, no.

The RPM, start point, and chuck location are tied together. If you change the RPM, you change the timing location for the start point. Its a matter of Kenetics.

Once you set the pitch feed and RPM, they are tied together. Its how fast the tool will start moving at a timed rotation of the chuck.

 

As opposed t a Mill, you can change the RPM to whatever the SFM needs. You just cant do it once you start the process, as in your case your getting chatter.

[gcode]

I was researching triple start threads on the Machining thread and got this reply

 

http://www.emastercam.com/board/topic/88060-triple-square-modified-10°-thread/

 

 

 

 

You don't necessarily have to shift your start point for a multi-start thread.
Sometimes clearances will not allow for this.
You can use "Q" to shift the start angle.
This works with canned threading & long code threading. (G32)
So for a triple start thread you would use:
G32 ............Q0.
G32 ............Q120.
G32 ............Q240.

or;

G76X_Z_I_K_D_F_A_P_Q_;
I : Difference of radiuses at threads
K : Height of thread crest (radius)
D : Depth of the first cut (radius)
A : Angle of the tool tip (angle of ridges)
P : Method of cutting
Q: Shift angle of thread cutting start angle

Depending on your control, you may not be able to use decimal points for the "Q" value.
Q120. could need to be Q120000 or similar.    

 

 

      

 

It's possible that adding a Q0 to your G76 line might allow you to change RPM

I don't know and haven't tried it.

It would be a simple test

Add a Q0 , back your tool offset off till you're just getting a witness cut

change the rpm and run it again.

If it works, it works, if it doesn't, no harm done

[Greg_J]

Thanks G-code I'll give it a try let you know.

 

I gave Fanuc a call and the person who I talked with had no clue what they were doing, they thought I was talking about G76 boring cycle for the mill. I also called the Doosan rep and he told me that in their new machines they had a thread repair cycle and if I had that option I could use it to recut the thread, so no real help either.

[Reko]

Hello,

I've been threading parts but if I change the rpm and re-run the part to get rid of chatter the machine looses pitch, I didn't actually do this cause I knew before hand that this will happen.

The reason you can not change RPM on the same part, is that, the CNC lathe's encoder sends a start signal at the beginning of the thread cycle at a particular RPM. When you change to a different RPM, there is a time delay or mismatch that changes the tool's angular entry point... there is no way I know of to account for or calculate that change. That is why using G96 on a thread is a no-no... you should always use direct RPM, G97.

 

I always set up a new part using a very low RPM so that I don't lose the first part because of chatter on the threads... then, you can increase the spindle speed between each part, until you reach the optimum RPM without chatter.

[Greg_J]

My typical threading cycle.

 

G76 P010000 Q100 R0.

 

G76 X4.474 Z-2.75 P1350 Q100 R0. F.25

 

 

 

First block of the G76 Threading cycle

 

 

G76 : G code for threading cycle.

 

 

P : P actually consists of multiple values which control the thread behavior

 

01 : Number of spring passes

 

00 : Thread run out at 45 degree

 

00 : Flank angle or Infeed angle

 

 

Q : Depth of normal cut

 

R : Depth of Last or Finish cut

 

 

Second block of the G76 Threading cycle

 

 

G76 : G code of the threading cycle.

 

X : The end value in x-axis

 

Z : The end value in z-axis

 

P : Thread depth

 

Q : Depth of first cut

 

F : Thread Pitch

 

R : Thread Taper

 

 

gcode it looks like the Q value in degrees that you mentioned wouldn't work with this cycle it's the depth of first cut.

[SlaveCam]

My typical threading cycle.

 

G76 P010000 Q100 R0.

 

G76 X4.474 Z-2.75 P1350 Q100 R0. F.25

 

 

I always define the second Q parameter larger than the first so that the first cuts take more until the minimum depth of cut is reached. Q100/Q500 works quite well and saves a lot of time as well in larger threads... the manufacturer (Sandvik does this) may have labeled the recommended number of passes in the box of inserts.

[tc24]

I've had success with this formula

[evitalond5]

interesting information [