Otc lathe threading Single G76

[Johnhudson]

Running a single line G76, Having problem getting the thread close enough to a shoulder, Code X starts @ .35 S500 Z.2
G76 X.262 Z-.14 K0260 D0100 A29 F.04167 (5/16 X 24)
I only have half of pitch to stop . Machine 1990 Mori SL-25
I know that increase the thread relief will work but just curious if there are different settings for G76 or parameters
Thanks in advance
John

 

[SeymourDumore]

Nothing in G76 that I know of will help you, but since you are using the single line G76, there is no way to define the "chamfer out of thread" amount.
So, the question is if there is a setting or a parameter on your machine that controls that?

For example, Haas also programmed with the single line G76, but it has M23 - ( chamfer out of thread on ) and M24 - ( chamfer out of thread off )
Also, it has 2 setting values where the chamfer out can be defined. One of those is the angle of the chamfer, the other is the number of threads to chamfer out over.

So in your case, may want to look into the manual and see if something along those lines exists.

 

[William Lynn]

As mentioned, see if you can use the two line G76, but that still will not help much. What threading tool and insert are you using? If for instance you're using a Kennametal top notch threading tool, use an NTK insert. The K means that the tool nose is not centered to the insert body, instead it is offset to the shoulder side. Using this insert on a 3/8"-24 thread will allow you to thread almost to the shoulder. Do note that this insert will chip much easier than a normal NT insert.

 

[angelw]

Using the two Block G76 to specify an End of Thread Chamfer or via a MTB supplied M code is not going to help the OP at all. All that does is make his issue worse by starting the pullout of the Threading Tool a greater distance back from the specified Z end coordinate. Accordingly, if the OP's aim is to finish with a Full Depth of Thread as close to the face of the shoulder as possible, then having no chamfer specified is his best option.

With regards to setting a Chamfer amount when using the one Block G76 cycle, I think from memory the parameter is number 0109.

Having problem getting the thread close enough to a shoulder,

What is the issue getting close enough to the shoulder? Do you mean that the mating part won't crew right up to the shoulder. In the actual cutting of the Thread, you should be able to safely have the leading edge of the insert go to within 0.002", or less, of the shoulder without issue.

At the start of the Thread, there is a distance where the Lead of the Thread is incorrect due to acceleration. Given your spindle speed of 500 rpm and a lead of 0.04167", the error will be, coincidentally, 0.04167"(one Lead). To avoid this error being part of the start of the Thread, you need to start at least the calculated length (0.04167) away from the end of the Thread in fresh air. You're starting at Z0.2, therefore you have the start covered.

There is also an error in the Lead of the Thread at the finish end of the Thread due to deceleration. For your spindle rpm and Thread Lead, the error distance will be 0.01146". To avoid this error impacting on the length of the Thread that will engage with the matting part, you would have to have a Thread relief of 0.01146, plus the distance of the Thread Form back from the leading edge of the insert.

Regards,

Bill

 

[Johnhudson]

Thanks Bill,
Your memory is spot on #109 parameter, It was set to 5.
Book says it can be set with programmed command also. Would that be R 0 ( book skips around between double and single format but no examples)
Thanks in advance
John

 

[angelw]

Thanks Bill,
Your memory is spot on #109 parameter, It was set to 5.
Book says it can be set with programmed command also. Would that be R 0 ( book skips around between double and single format but no examples)
Thanks in advance
John

The book would be referring to the Two Block G76 Cycle, there is no way to set the Chamfer amount programmatically when using the One Block G76 Cycle (FS15 Format).
Setting that parameter to Zero is going to help your cause, having any number in there is simply going to start the pullout of the tool further away from the shoulder.

Regards,

Bill

 

[SeymourDumore]

Using the two Block G76 to specify an End of Thread Chamfer or via a MTB supplied M code is not going to help the OP at all.

Bill

Actually Bill, on a Haas that is exactly how it works!
M24 is the code to turn off the "chamfer out of thread " .
It basically tells the control not to chamfer out, regardless of what is in the parameters or settings.

 

[Vancbiker]

Actually Bill, on a Haas that is exactly how it works!
M24 is the code to turn off the "chamfer out of thread " .
It basically tells the control not to chamfer out, regardless of what is in the parameters or settings.

You will still have some pitch error due to the deceleration of Z before the X move to clear the tool from the thread.

 

[SeymourDumore]

You will still have some pitch error due to the deceleration of Z before the X move to clear the tool from the thread.

Vanc, I was replying to Bill's comment about the M-code or lack thereof.
The Haas establishes a taper out or straight pull by M23 and M24 respectively.
Beyond that, there is nothing one can do to program out of that paper bag.

 

[Vancbiker]

Un

Vanc, I was replying to Bill's comment about the M-code or lack thereof.
The Haas establishes a taper out or straight pull by M23 and M24 respectively.
Beyond that, there is nothing one can do to program out of that paper bag.

Understood. I added that because some folks do not realize that even with chamfering off you still have some imperfect thread right at the endpoint in Z.

 

[sinha]

It is a bad design, needing threads up to a shoulder.

 

[angelw]

on a Haas that is exactly how it works!
M24 is the code to turn off the "chamfer out of thread " .
It basically tells the control not to chamfer out, regardless of what is in the parameters or settings.

Yes, I know how those M Codes work. Many machines pre the two Block G76 Format used a similar system, with the amount of chamfer set via parameter, as I explained to the OP.
I thought you were suggesting to the OP to use the chamfering feature, which, as I pointed out, would work against him.

Regards,

Bill