Denford Software & Machines

I am still having intermittent issues with G76 threading. As a test I threaded a 1.5'' bar with an 18 TPI using this code.

N140 G99 G97 F0.055 S500
N150 M03
N160 M08
N170 G00 X1.53 Z0.03
N180 G76 P010060 Q15 R0.0005
N190 G76 Z-0.5 X1.4339 P764 Q38 F0.0555

Worked great as far as I could tell.

Now, try again with same bar but 9TPI

N140 G99 G97 F0.111 S400
N150 M03
N160 M08
N170 G00 X1.53 Z0.03
N180 G76 P030060 Q15 R0.0005
N190 G76 Z-0.5 X1.3791 P1146 Q38 F0.1111

Goes along happily, maybe 15 passes and then tries to make a very deep cut that stops the machine cold. This has been an issue in almost all threading operations. It is a Novaturn, fully updated, VR turning 1.16

It seems to take random cut depths quite a bit. I think I have programmed it right with a maximum first cut depth of 38 microns and a minimum of 15.

Any help would be much appreciated. Thanks!

Dave

Sorry we can't look into it in too much detail at the moment - its always a tricky subject and can take a lot of setting up and testing.
There could also be a problem with the spindle motor (brushes?) or the drive if a full contact thread cut is stopping it - you normally hear a dip in the speed as the thread starts cutting, but shouldn't stop.

We recently cut a range of Metric threads from M4 to M16 and found that the X offset needed altering to get the thread to cut properly. Here is the program for an M16 thread for you to examine, and the X offset value we had to change in the LatheCAM setup file in order to get the correct GCode for them to cut properly. Hope this helps in the short term:

What material are you cutting?

9 TPI is going to be close to the maximum capability of the machine as the spindle

2.8mm Pitch is more than we would normally cut and will be on the limit.
With the spindle running at 400 RPM the slide has to travel at 1.12M/Min.

With the depth of cut and spindle speed it is difficult to know what will happen.

I think the Max pitch we recommend is either 2mm or 2.5 mm pitch.

In softer material this could be increased.

Slowing the spindle down would help but would reduce the torque available. Increasing the speed would improve torque but then the feed would not be available.

Thank you Steve and Denford Admin! I appreciate all your help.

First, the offset of .2mm will come in handy as it has not been cutting my threads deep enough.

I have spent easily 60hrs just testing the threading cycle. The pieces I am running now are just tests of what the machine can do and to get it to cut properly. I realize that a 9tpi is at the limits of what the machine can do at the speed it need to go to generate enough torque to make the cut.

I am using both Delrin and free machining aluminum for the test. Delrin it can make it through. Aluminum it cannot. If I use a high TPI like 18 then it can make the thread but I think the behavior I have targeted is this.

The first cuts are great even at 9 TPI but somewhere along the process the machine tries to take a very deep cut, maybe twice what it should. One that not only stops the machine but typically on a deep thread like a 9 TPI will actually knock the part out of the chuck.

Even on higher thread counts it seems to take too deep of a cut somewhere about half way through that causes the machine to seriously slow down or even stop momentarily.

I am wondering if the only option, which is not all that bad is to stop using the G76 as either I am programing it wrong or the controller is interpreting it wrong. If it is the controller, I cannot trust it to make a thread without ruining the part.

I am open to all suggestions as I realize that still this is most likely my fault.

Thanks!

Dave

O.K.

well since the G76 route will not work well for me I tried a G32 but the control reads the Z axis wrong and goes the wrong direction, heading instead all the way back to home in the Z.

Is there another method, other than the G76 I can use?

Please! without a fix I essentially have no threading capabilities.

I can't keep crashing parts for hours on end.

Dave

P.S. I will run the above thread on the M16 and see what happens.

One thing I noticed was the chamfer angle you have set to 0deg:
I think this could be adversely effecting the calculation for cut depth on each pass. If I remember correctly, the tool moves in Z slightly each pass in order to keep the leading edge cutting (and not rubbing) and root 2 of tip angle
seems to ring a bell in the calcs, but the chamfer angle will also play a part - something like a divide by zero could be happening somewhere in the cycle

Could you try it with a chamfer angle eg:
N180 G76 P016060 Q15 R0.0005
N190 G76 Z-0.5 X1.4339 P764 Q38 F0.0555

If thats not possible because of a shoulder, then could you try a chamfer angle of 1 (ie not zero)


Had to remind myself of the G76 code:
G76 P (A) / (B) / (C) Q (Min) R ;
G76 X(U) Z(W) P (DEP) Q (1st) F ;

P (A) is the number of thread finishing passes (1 to 99).
P (B) is the chamfer amount. This is the angle at which the tool leaves the billet, at the end of the thread cutting cycle.
P (C) is the angle of the tool tip (8Ø°, 6Ø°, 55°, 3Ø°, 29° and Ø°). Note - (A), (B) and (C) are all specified at the same time by the address P, eg, PØ36Ø6Ø = number of cuts is Ø3, chamfer amount of 6Ø and tool angle of 6Ø°.
Q (Min) is the minimum cutting depth (in microns). When the depth of the cut calculated by the CNC control becomes less than this limit, the cutting depth is clamped at this minimum value.
R is the finishing allowance. This is the final, or finishing, cuts applied to the thread. The number of stages to complete this finishing allowance is determined by the value of P(A), ie, the value of R divided by the P(A) number of finishing passes equals the value of each finishing allowance stage.

X(U) is the end position of the thread in the X axis (the core diameter).
Z(W) is the end position of the thread in the Z axis.
P (DEP) is the depth of the thread as a radius value (in microns).
Q (1st) is the depth of the first pass as a radius value (in microns).
F is the size of the thread pitch.

Dave,

The Nova is designed as an educational machine and the thread you are trying to cut is beyond its limit. The thread cycle cuts on the leading edge of the insert so the tip moves both forward and in while cutting a thread. this means the surface area making the cut is suposed to increase as the thread gets deeper.

The smaller the pitch the higher the feed and as a result the more likely you are to stall the spindle.

I dont think there is anything else we can do. ADMIN has checked the programming and the cycle is correct.

I would not normally try to cut a thread beyond 2mm with the machine.

You may improve things if you buy 2011T3 free chipping Aluminium

Good Luck

I'm starting to think Steve is right about this being too much for the machine - the cut depth figures look ok when I run your G76 cycle through simulation - and as I mentioned before, apart from the 0.2mm "fudge factor" we can happily create various metric threads.

I can only guess that these heavy cuts are a result of the first passes pushing off (the tool or billet or both), then the cutter eventually digs in and the resulting cut area is too much for the spindle.