Fanuc 0T lathe - G76 threading troubleshooting

[angelw]

Maybe it was something else that I changed, and I'm mis-remembering what is was. Is there anything in the G76 lines that, when changed, would cause the threading cycle not to track with the previous cycle (other than the feed, of course)?

Hello wmpy,
I should have qualified my previous Post a little. If only the X value in the second G76 Block is changed, the index of the Thread Path remains the same and the Threading Tool will track exactly. If the Thread Height is also changed to compensate for the modification of the X Value; for example, if the X value was made smaller by 0.25mm and the Thread Height (P address) made 0.125mm larger, then the Thread Start will be indexed and the Threading Tool won't track exactly as before the change.

Regards,

Bill

 

[wmpy]

Hello wmpy,
I should have qualified my previous Post a little. If only the X value in the second G76 Block is changed, the index of the Thread Path remains the same and the Threading Tool will track exactly. If the Thread Height is also changed to compensate for the modification of the X Value; for example, if the X value was made smaller by 0.25mm and the Thread Height (P address) made 0.125mm larger, then the Thread Start will be indexed and the Threading Tool won't track exactly as before the change.

Regards,

Bill

Thanks for the clarification, Bill. That may explain what I had experienced in the past.

 

[sinha]

At the same time, if the finishing allowance is also increased by 0.25, it will keep the roughing depth unchanged, and the thread would be tracked correctly.

 

[guythatbrews]

Hello guythatbrews,
I think you'll find that the radius at the root of an External Metric Thread is not actually specified, other than the implied value that results from a circle that is tangent with the flanks of the Thread and has a chord at the tangent points of P/4, where P = Pitch of the Thread.

Regards,

Bill

Hi Bill,

To clarify, I was referring to a metric thread when I said "M profile". And specifically about external threads.

Referring to MH 25th edition, I'm talking about what it names "American National Standard Metric Screw Threads-M Profile". MH further states this M profile thread has a basic ISO 68 designated profile. I've never seen ISO 68.

Under the heading "M Crest and root profile" below, am I to understand the external root may be completely flat? In the next paragraph for the rounded root thread the root radius is limited to no less than .125P.



I don't understand this. It seems to say a fully flat root is permissible, and a rounded crest and root form also permissible for internal and external threads. Then it goes on to say the minimum radius for external root is .125P. Can we have our cake and eat it too? If the designer wants a rounded root thread, how is that conveyed to the manufacturer? Or am I just completely misinterpreting this whole idea?

The subject of J threads has been mentioned. I have cut tons of UNJ threads, but don't recall cutting any metric J threads. MH 25th edition does talk about the MJ profile, saying it is similar to the UNJ profile defined by MIL-S-8879, which specifies min/max root radius and min/max minor diameter. MH goes on to illustrate the MJ profile and defines min/max root radius and min/max minor diameter, stating the form is defined in ANSI/ASME B1.21M-1978.



All my understanding is informed by these American standards. Can it be they diverge from the metric standards?

Greg

 

[maguilera]

I have the English version of a German book called “Mechanical and Metal Trades Handbook” which states the radius of a rounded root metric external thread for a given pitch.

Cheers.

 

[bengineer08]

Quite a wealth of wisdom here.

I'm using a single, sharp point tool. I've cut the major diameter to 15.8mm. I finally got a set of wire gauges today and measured the pitch at around 15.26mm, which is roughly 0.27mm too large.
I've reread these posts several times, and I'm trying to digest it all. If I'm reading it correctly, since I'm using a single point sharp V, I need to make the root diameter smaller than the handbook says? If I can't go below that value I can try and take another pass with a slight Z shift.
Changing P and Q values really only corresponds to the number of passes it will take?

I've been trying to shrink the root diameter, and it's getting ridiculous. I'm down to 13.0 mm and it nearly wants to thread on, but still not quite. I'm obviously doing something wrong here.
I haven't tried the slight z shift option yet. I'll retry and give that a shot.

 

[sinha]

I am copying some useful information posted by some other member (I do not remember) in a previous thread. This figure explains why depth of thread needs to be increased ...


Modified depth of thread for external threads (to include the additional in-feed) = 1.4 x original depth

The 1.4 figure is based on
1. The basic profile of a metric thread, for which the depth of thread is 0.54127 x Pitch
2. It also assumes that the insert tip has zero radius.

The depth of thread in threading charts is based on design profile of metric threads, which includes the fillet depth also, which makes depth of thread = 0.61344 x Pitch. This is the depth which is used for machining.
Moreover, the insert tip will have some radius.
Therefore, the 1.4 figure is only approximate, but it can be a good starting point.

In case of internal threads, modified depth = 1.2 x original depth

 

[sinha]

The terms major and minor diameters are used with reference of basic profile.

In design profile, the fillet depth is subtracted from minor diameter and called core diameter (in external thread). Minor diameter is same as bore diameter in the design profile of internal thread.

On the other hand, major diameter is used for both basic and design profiles of external threads. In case of internal threads, fillet depth is added to it, and it is called root diameter in design profile.

 

[SeymourDumore]

I'm down to 13.0 mm and it nearly wants to thread on, but still not quite. I'm obviously doing something wrong here.
I haven't tried the slight z shift option yet. I'll retry and give that a shot.

Whatever you're doing, it is definitely wrong!
If you went down to 13mm on the minor for a 16 x 1.5 thread, then there is something drastically wrong!!
The Z-shift is a hack to get you by something for once in a blue moon, otherwise it should not be used as a SOP.

Check your inserts, check the shape of the thread on a comparator!

 

[guythatbrews]

This deal about the external minor diameter limits has been bugging me.

Here is a quote from ISO 965-1 regarding minor diameter:

"External threads on fasteners of property classes below 8.8 should preferably conform to the requirements stated above. This is particularly important for fasteners or other screwed connections which are subjected to fatigue or impact. However, there are in principle no restrictions other than that the maximum minor diameter, d3 max, of the external thread shall be less than the minimum minor diameter of the Go-gauges according to ISO 1502."

And here is a link to ISO 965-1. The quote above is from page 14:

https://regbar.com/wp-content/uploads/2019/09/ISO-965-1-1998-%C3%96NEML%C4%B0.pdf

So, by strict reading of the specification, unless the thread needs to be above property class 8.8, or is subjected to fatigue or impact, the thread root may be sharp. However, the spec also states this is not preferable.

Also, on page 14 the minimum allowable radii for threads above class 8.8 is specified as .125P.

I interpret this to mean there is some wiggle room regarding the minor diameter/root radius question. The rub is to defend your position you need to know the grade of the fastener and/or it's intended use. To err on the safe side, conform to the minor diameter and root radius limits. For low duty applications you can use less than a .125P root radius and the thread will still conform to ISO 965-1, even though it is not preferable to do so.

If you use full a profile insert this all becomes automatic. That is as long as the insert itself is manufactured correctly!

To speak more the the OPs question, It is interesting many insert manufactures offer multi-pitch threading inserts meant to be suitable for more than one metric pitch. The inserts are so sharp they will undercut the published minor diameter limits for the larger pitches they are intended to cut. Even if you maintain the minor dia. limits and widen the thread space to hit the pitch diameter, the radius will be under .125P. These multi-pitch inserts may not be the best thing to keep on hand if you need to conform to the minor diameter limits.

 

[angelw]

If you went down to 13mm on the minor for a 16 x 1.5 thread, then there is something drastically wrong!!
The Z-shift is a hack to get you by something for once in a blue moon, otherwise it should not be used as a SOP.

The OP states that he is using a sharp pointed tool. The Pitch Diameter is the most important diameter to get right, so with a sharp point tool he has two choices, either cut the Thread deeper, which also widens the Thread Groove and makes the Pitch Diameter smaller, or cut to the correct Minor Diameter and widen the the Thread Groove by shifting the "Z" start position the required amount.

Cutting the Thread deeper until the Pitch Diameter is right, with little, or no reference to the Minor Diameter is the biggest hack of all, which results in weakening the fastener via a reduced Minor Diameter and a dead sharp stress point. Given only these two choices, I'd opt for shifting "Z" every time.

Regards,

Bill

 

[NAST555]

Get yourself a ZEUS book or equivalent. It is very handy for quick referencing. My program would look something like this...

G76 P020060 Q150 R50
G76 X14.16 Z-13.0 P920 Q250 F1.5.
As others have said, if you have a normal open form 60 degree tool then you might have to go deeper on your offsets or side cut a bit in Z. With full form 1.5 pitch insert you can turn the OD 0.1mm larger than 16 and run your threading tool to the point where it just starts chamfering the OD and if you mic it, it goes a bit undersized.

Make sure that your tool is square to the part, that could also be messing you around.

 

[sinha]

This chart in only for standard coarse pitches.
For M16x1.5, formula needs to be used.

 

[sinha]

An issue with shifting Z is that machining time would double, unless the programmer is smart enough to cut down on roughing passes.

 

[angelw]

unless the programmer is smart enough to cut down on roughing passes.

All that's required is a First DOC to be slightly less than the Thread Height.

Regards,

Bill

 

[sinha]

Yes. That will give two roughing passes.
Equal to thread height will give one roughing pass.

 

[NAST555]

This chart in only for standard coarse pitches.
For M16x1.5, formula needs to be used.

Yes, but simple to use the standard 1.5mm (M10) and convert all the sizes to a M16 x 1.5. Very easy

 

[sinha]

That is correct. The person has to know that all dimensions are pitch-related.
Some calculation would still be needed.