[eliot15]

I'm trying to calculate the number of threading passes my first use of a G76 threading cycle will make for a 1-4/3 x 12 UN 2A external thread.

I have no basis for comparison, having never cut threads before, but the number I'm comming up with seems large to me. Could someone check this???

Here are my G76 blocks:

G76 P020060 Q20 R0.
G76 X1.6398 Z-2.275 P511 Q120 F.083333

The formula I have is from Peter Smid (CNC Programming Hdbk):

n = ((P-R)/Q) ^ 2

where:

n = Number of threading passes
P = Depth of thread per side
R = Depth of the last threading pass
Q = Depth of the first threading pass

So I get:

number of passes = ((0.0511 - 0.002) / .012) ^ 2
number of passes = 16.74

which seems like an aweful lot. Is that right????

I'm thinking the Q value in the first line of the G76 format gives the depth of the last threading pass (R in my formula), and
I'm thinking the Q value in the second line of the G76 format gives the depth of the first threading pass.

Thanks

[Geof]

Your math is correct but I think your first pass at .012 is shallow for 12 tpi. If you increase this it has quite an effect on the number of passes. For instance taking the first pass up to 0.015 reduces the number of passes to 11 (10.7) which starts to seem reasonable.

[eliot15]

Thanks for checking that Geof. Appreciate it. I'll have to experiment with the first pass depth.

[sinha_nsit]

Q in the first block is the minimum depth of cut.
If the calculated depth of cut comes out to be smaller than this Q, the remaining passes use the same Q without further calculations.
The depth of cut is manipulated so as to remove the same amount of material in every pass.

Why do you worry about the number of passes? Just specify the two Q values properly, and the control would do the rest.

I have a doubt that the given formula is correct, though I am not 100% sure.

[eliot15]

Why do you worry about the number of passes?

I'm going to be doing a lot of external threading on a new "turn/mill" at work soon, and am just reading up on single point threading while waiting for the parts I'll be dealing with to come back from various outside processes.

One CNC programming book I read pretty regularly does the passes calculation while demonstrating how to program external thread cutting manually using G32 mode. No, I don't plan on using G32 mode. There's the stuff you read in books, then there's the way it really gets done (with some overlap along the way.)

It will still be a bit before I actually bring this information to bear and cut some steel, but just gathering info. in the mean time.

Thanks very much for your reply. You make it all sound much simpler.

[sinha_nsit]

More information:
It can be proved that in order to remove same amount of material in every pass, the level of cut (measured from thread's crest) in nth pass would be [SQRT(n) x first depth of cut].
This forms the basis of the given formula, but it would be correct only when the calculated depth of cut is always more than the minimum depth of cut (Q in first block)
The depth of cut in nth pass = level of cut in nth pass - level of cut in (n-1)th pass
Incidently, R in the formula is the specified finishing allowance (radial value). Thus, in your calculation, it would be 0, not 0.002.

[eliot15]

Incidently, R in the formula is the specified finishing allowance (radial value). Thus, in your calculation, it would be 0, not 0.002.

Thanks for that. This point is a little less than clear in Smid's presentation of the formula in "CNC Programming Handbook".

He writes:

"Well, ther is one more programmlng decision to make...it is to select a last pass known as a finishing allowance - for example 0.004 for the following calculation."

He then calculates:

n = ((0.0511 - 0.004)/0.021) ^ 2 = 5.03 = 5 passes (excluding the finishing allowance pass, which is a 6th pass).

This is all programmed in G32 mode.

The confusion arises later when he presents G76. The code looks like this:

G76 P011060 Q004 R0.002
G76 X2.8978 z-1.6 R0 P0511 Q0210 F0.0833

I think the first line of the G76 format either has some errors as printed, or isn't intended to correlate with the previous example (the number of passes calculation). The Q in line one would give a minimum cutting depth of .0004. The R in line one I would expect to be 0.004 from his calculation example.

The finish allowance (0.004) in the calculation is a radial value, yes, but it would still be written as 0.004 in the G76 block, and not 0.002, wouldn't it? I mean, 0.0511 and 0.021 are raial values also.

I understand your point, though, about why the subtraction in the calculation is subtracting the finishing allowance.

Thanks

[sinha_nsit]

The finishing allowance is specified on diameter, though it can possibly be on radius also depending on some parameter (I am not sure). My notes say it is a diameter value. Then, for the given calculation to be correct, the first block of G76 should have R0.008.

Thread height and depth of cut are radial values.

And, 5.03 does not mean five passes. It would be six passes, the depth of cut in the sixth pass would be suitably adjusted to leave the specified finishing allowance. Thus, there would be total seven passes.

Smid is not always correct.

[g-codeguy]

Here's a little trick to keep in mind. Say you are getting the correct number of threading passes as determined by one of the insert catalogs using .018 DOC for your first pass. BUT the insert keeps chipping so you decrease the DOC for the first pass to something like .012 DOC. Insert no longer chips, but now you are getting way too many threading passes.

Set it back to .018 DOC and increase the P-value for thread height. You will still get an increase in the number of passes, but it won't be as many as decreasing the first pass gave you. This will decrease the actual DOC of the first pass stopping your insert from chipping, yet keeping the total number of passes within reason.

[sinha_nsit]

What you have said can be mathematically verified. I believe you must be correct, having verified it experimentally.
But, how did you hit upon this idea? I am impressed.

[angelw]

What you have said can be mathematically verified. I believe you must be correct, having verified it experimentally.
But, how did you hit upon this idea? I am impressed.

Hi Shina,
This method has been around for quite a while. In software, the Fanuc G76 cycle determines the Major and Minor diameter of External and Internal threads respectively, whether real or hypothetical, by applying the P and X values passed by the G76 cycle in the program. This diameter is then used as the start point from where the first cut value is applied, and the depth of successive cuts are reduced using this first cut value in the first calculation for the next cut. This method takes advantage of a reasonably large first cut value to be subsequently used in the "reduction of cut" calculations, but applied only part of first cut to actually cutting metal and the rest to fresh air.

Regards,

Bill

[g-codeguy]

What you have said can be mathematically verified. I believe you must be correct, having verified it experimentally.
But, how did you hit upon this idea? I am impressed.

Trial and error. Bill has already explained how it works. Try it yourself. Count the passes. You'll see I'm right.

[eliot15]

Alright,

Sorry to take so long to get back.

I cut 200 components this past week. And with the exception of a sh&^%y circuit breaker, all went well. Pitch diameter, after heat treat and plating, is what I was most concerned about controlling. Turned out awesome!!!

Based on the following G76 input, I was predicting 16.74 passes, and 2 finish passes:

G76 P020060 Q20 R0.
G76 X1.6398 Z-2.275 P511 Q120 F.083333

Guess what, got 19 passes, and perfect external threads on a brand spankin' new PUMA 2000 SY turn/mill w/FANUC Series 31i - Model A control.

Life is good.

Thanks for all the input.

[g-codeguy]

Love the smell of a new machine! :banana::wee: