Fanuc 0T lathe - G76 threading troubleshooting

[bengineer08]

Hello all,
I'm trying to learn the G76 threading cycle. I'm starting with an M16 x 1.5 external thread. I've got:

G76 P040060 Q30 R0.02;
G76 X14.1 Z-13.0 P950 Q160 F1.5;

As I understand it, the second line's X14.1 should be the thread's minor diameter. I used 14.1, centering it between the extremes in machinery's handbook of 14.34 to 13.93.
Also, the second line's P950 should be depth of thread (0.950mm), which should be 16mm - 14.1 / 2 = 0.95mm (I think?).
the diameter and the pitch appear correct, but threading a nut on isn't happening. It's too tight. I've been toying with the second line's X14.1, taking it deeper seems to do nothing, and I've been playing with the P950, making it larger seems to do nothing either.

Am I misinterpreting anything? Am I getting my values from the wrong columns? Any suggestions would be greatly appreciated. Thanks

 

[Vancbiker]

What’s it measure with a pitch mic or over wires? Major dia correct? Too big of a radius on the tool? So many missing bits of info.

 

[sinha]

Try reducing the workpiece diameter slightly.

 

[angelw]

Hello all,
I'm trying to learn the G76 threading cycle. I'm starting with an M16 x 1.5 external thread. I've got:

G76 P040060 Q30 R0.02;
G76 X14.1 Z-13.0 P950 Q160 F1.5;

As I understand it, the second line's X14.1 should be the thread's minor diameter. I used 14.1, centering it between the extremes in machinery's handbook of 14.34 to 13.93.
Also, the second line's P950 should be depth of thread (0.950mm), which should be 16mm - 14.1 / 2 = 0.95mm (I think?).
the diameter and the pitch appear correct, but threading a nut on isn't happening. It's too tight. I've been toying with the second line's X14.1, taking it deeper seems to do nothing, and I've been playing with the P950, making it larger seems to do nothing either.

Am I misinterpreting anything? Am I getting my values from the wrong columns? Any suggestions would be greatly appreciated. Thanks

As Kevin and Sinha have commented.
The reason changing the P value has no affect, is that the control uses the X value and the P value to determine the Major diameter of the Thread as in:
MD = X + 2P
In your case
MD = 14.1 + 0.95x2
MD = 16

From that calculated Major Diameter, the First Pass DOC specified by Q (radius value) is applied.

In practice you wouldn't do it, but the X Reference Return position could be used as the X Start location and the First and subsequent Threading Passes would be applied the same as if the Threading Tool X Start position was only 1.0mm larger than the Thread Major Diameter.

By making the P value larger simply results in a larger Major Diameter being calculated by the Control. The First Pass DOC of 0.160 is then applied from this larger calculated Major Diameter, resulting in an actual smaller First Pass DOC being made, due to some of the 0.160 being taken up in fresh air. If you were to make the P Value 1110 and left the Q value as 160, then the First Threading Pass would barely touch the OD of the Thread.

Regards,

Bill

 

[wmpy]

In addition to what's been already mentioned, it should be pointed out that you should not change the X on your second line when trying to thread the same part. In other words, don't run the part, realize that the thread is too large, change the X in the program, and then recut the threads on that same part. The control will not pick up the same thread again, and you could ruin your part. It's a better idea to make the change with your X tool offset to re-run the part. Then, once you're happy with the thread, put the offset back to what it was, and adjust your programmed X value by the distance you moved the offset. That way, the program will be good for your next part.

 

[guythatbrews]

If you are not using a full profile insert but a sharper insert, it's likely when you reach the x destination the thread will be oversize. For a multi-pitch you need to make the minor smaller unless you are cutting the smallest pitch for that insert. Same for a sharp vee, only more so.

 

[angelw]

In other words, don't run the part, realize that the thread is too large, change the X in the program, and then recut the threads on that same part. The control will not pick up the same thread again, and you could ruin your part.

Hello wmpy,
That's not actually so. Altering the X value has no bearing whatsoever on the synchronization between the Spindle and the Z axis with a parallel thread or a radial taper of less than 45degs. With either of these threads, the tool will track in the same thread groove if the X value is altered.

However, altering the X (minor diameter - male thread) is poor practice. Its tantamount to programming a turned diameter that is specified at, say, 50mm on the drawing, and when you find that the diameter is being cut at 50.25, altering the X value in the program to 49.75. It simply results in a fudged program that is difficult to follow.

Rather than alter the X value to be other than a value that is in the tolerance for the minor diameter of the thread being cut, simply adjust the size of the thread with the X offset for the tool. The most important component of the thread to get right is the Pitch Diameter. The Major and Minor Diameters of an External Thread can be considerably under size (within reason) and as long as the Pitch Diameter is correct, the Thread will be perfectly serviceable.

The Pitch Diameter will generally be too large if a generic, sharp "V" form Threading Insert is used and cutting to the correct Minor Diameter. If its important that the tool not cut deeper than the specified Minor Diameter and the Pitch Diameter is too large, then the Pitch Diameter can be made smaller by widening the Thread Groove with an additional Finishing Pass, or two, with the Z Start Position shifted slightly. The amount of total Z shift required can be accurately calculated by first measuring the Pitch Diameter and determining the amount it needs to be decreased by, then use this value in the following algorithm:

Z = Tan(TA/2) x PE/2
Where:
Z = Total Z Shift
TA = Included Angle of Threading Insert
PE = Error in Pitch Diameter

Regards,

Bill

 

[maguilera]

Some great advices up there already. But one thing I couldn’t help noticing is that your program will take something like 28 passes to cut a 1.5mm pitch thread, and in my opinion, unless you have a serious rigidity problem, this is simply a waste of time.

Here’s a sample program I’d use to cut an M16x1.5 external thread:

G76 P040060 Q70 R0.06;
G76 X14.1 Z-13.0 P950 Q335 F1.5;

This program will do 7 roughing passes and 4 finishing passes, giving a total of 11 passes. Notice the increase in the minimum cutting depth (first line Q), finishing allowance and depth of first pass (second line Q).

Cheers.

 

[angelw]

Here’s a sample program I’d use to cut an M16x1.5 external thread:

G76 P040060 Q70 R0.06;
G76 X14.1 Z-13.0 P950 Q335 F1.5;

This program will do 7 roughing passes and 4 finishing passes, giving a total of 11 passes. Notice the increase in the minimum cutting depth (first line Q), finishing allowance and depth of first pass (second line Q).

Cheers.

I'd increase the First DOC even more. Rule of Thumb, the First DOC is what the Threading Tool and work-piece set up can consistently handle. The Thread is only 13mm long and if there was minimal stick-out from the chuck, 0.5mm First DOC (Q500) would be my start point. Because each subsequent Threading Pass DOC uses the First Pass DOC value in their calculated value, the larger the First DOC can be made, the longer it will take to start using the minimum DOC set by the "Q" address in the first G76 Block and therefore, fewer Threading Passes. The algorithm used to calculate each subsequent DOC is:

DOC = Q x SQR(N)
Where:
Q = First Pass DOC Value
N = Nth number of Thread Pass (1,2,3,4, etc)

From the above it can be seen that the First Pass DOC has a great bearing on the total number of Threading Passes to complete the Thread

A client's recent project that had a 30 x 1.5 Thread (1040 steel), cut high quality threads in 6 passes total. In excess of 500 threads were cut, all in tolerance, with the one insert edge. The Threading Insert was Full Form.

Regards,

Bill

 

[guythatbrews]

If you are not using a full profile insert but a sharper insert, it's likely when you reach the x destination the thread will be oversize. For a multi-pitch you need to make the minor smaller unless you are cutting the smallest pitch for that insert. Same for a sharp vee, only more so.

As angelw pointed out, my statement here is not correct and can get you into trouble.

The minor diameter limits are to be followed if you are producing threads to a drawing specification. However, in practice, if I'm making a low stress screw thread for my neighbor's tractor some other mundane item with no drawing requirements, I ignore the minor diameter limits. That is as long as the minor diameter is small enough to function, which it will be with a tool nose radius that is small enough.

Another consideration when moving the tool axially to widen the thread space and hence decrease the pitch diameter is the actual size of the threading tool radius. I believe the minimum allowable radius is .125P, so a conforming M profile thread cannot be cut with a tool radius less than .125P, even by widening the thread axially.

Please correct me if this is incorrect! It is usually not a consideration for me since for customer parts I use full profile inserts of the correct pitch. But I have run into trouble when the thread was special, and the customer and I couldn't agree on d1 and d3. I don't remember the final resolution but my calculations of d1 and d3 agreed with on-line calculators, and the customer's calculations did not. I think that there was enough overlap in our numbers to allow me to cut the thread to pitch diameter high limit and still maintain the customer's minor diameter tolerance. The customer is always right! That is as long as you keep good records of what you were told to do.

 

[wmpy]

Hello wmpy,
That's not actually so. Altering the X value has no bearing whatsoever on the synchronization between the Spindle and the Z axis with a parallel thread or a radial taper of less than 45degs. With either of these threads, the tool will track in the same thread groove if the X value is altered.

However, altering the X (minor diameter - male thread) is poor practice. Its tantamount to programming a turned diameter that is specified at, say, 50mm on the drawing, and when you find that the diameter is being cut at 50.25, altering the X value in the program to 49.75. It simply results in a fudged program that is difficult to follow.

Rather than alter the X value to be other than a value that is in the tolerance for the minor diameter of the thread being cut, simply adjust the size of the thread with the X offset for the tool. The most important component of the thread to get right is the Pitch Diameter. The Major and Minor Diameters of an External Thread can be considerably under size (within reason) and as long as the Pitch Diameter is correct, the Thread will be perfectly serviceable.

The Pitch Diameter will generally be too large if a generic, sharp "V" form Threading Insert is used and cutting to the correct Minor Diameter. If its important that the tool not cut deeper than the specified Minor Diameter and the Pitch Diameter is too large, then the Pitch Diameter can be made smaller by widening the Thread Groove with an additional Finishing Pass, or two, with the Z Start Position shifted slightly. The amount of total Z shift required can be accurately calculated by first measuring the Pitch Diameter and determining the amount it needs to be decreased by, then use this value in the following algorithm:

Z = Tan(TA/2) x PE/2
Where:
Z = Total Z Shift
TA = Included Angle of Threading Insert
PE = Error in Pitch Diameter

Regards,

Bill

Well that's embarrassing. I really thought that was the case. I think that years ago I changed something in a threading program and ended up scrapping the part because the re-threading didn't track with the existing thread. 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)? I know that Z starting point and spindle speed will cause the thread not to track... unless I'm wrong about that, too!

 

[Vancbiker]

IME, the most common cause of folks wrecking a thread by bad lead is changing the spindle speed and then re-cutting.

Changing the infeed angle and re-cutting will trash a thread

 

[sinha]

Well that's embarrassing. I really thought that was the case. I think that years ago I changed something in a threading program and ended up scrapping the part because the re-threading didn't track with the existing thread. 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)? I know that Z starting point and spindle speed will cause the thread not to track... unless I'm wrong about that, too!

You possibly changed the finishing allowance. There are other possibilities also.

 

[angelw]

Another consideration when moving the tool axially to widen the thread space and hence decrease the pitch diameter is the actual size of the threading tool radius. I believe the minimum allowable radius is .125P, so a conforming M profile thread cannot be cut with a tool radius less than .125P, even by widening the thread axially.

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

 

[Vancbiker]

Hello guythatbrews,
I think you'll find that the radius at the root of an External 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

Some thread specs do have requirements for root radius. UNJ comes to mind.

 

[angelw]

Some thread specs do have requirements for root radius. UNJ comes to mind.

Hello Kevin,
That's correct, and the Metric Thread is no exception, but the Radius is not specified. Its whatever Radius that results from it being tangent to the Flanks of the Thread and having a Chord at that tangent point of P/4.

The Root Radius of a UNJ External Thread states a maximum radius that is derived from an arc tangent to the Flanks of the Thread Form, with a Chord Length at the tangent points that results from a line drawn 0.3125 X H up from the sharp "V" intersection at the root of the basic "V" form of the Thread, where H is the height of the basic Thread Form from the "V" intersection at the Crest and Root of the sharp "V" form.

The OP's Thread is Metric and guythatbrews referred to an "M profile thread"; I assumed the "M" to mean Metric. I should have been more specific in my Post and stated that it was for a Metric Thread.



Regards,

Bill

 

[Vancbiker]

Hello Kevin,
That's correct, and the Metric Thread is no exception, but the Radius is not specified. Its whatever Radius that results from it being tangent to the Flanks of the Thread and having a Chord at that tangent point of P/4.

The Root Radius of a UNJ External Thread states a maximum radius that is derived from a Chord Length that results from a line that intersects the Flanks of the Thread Form, 0.3125 X H up from the sharp "V" intersection at the root of the basic "V" form of the Thread, where H is the height of the basic Thread Form from the "V" intersection at the Crest and Root of the sharp "V" form.

The OP's Thread is Metric and guythatbrews referred to an "M profile thread"; I assumed the "M" to mean Metric. I should have been more specific in my Post and stated that it was for a Metric Thread.



Regards,

Bill

Thanks for the explanation. When I had to do UNJ threads, the prints called out a max and min root radius so no research or calculations were needed.

 

[SeymourDumore]

I think that years ago I changed something in a threading program and ended up scrapping the part because the re-threading didn't track with the existing thread. 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)? I know that Z starting point and spindle speed will cause the thread not to track... unless I'm wrong about that, too!

Spindle speed absolutely affects the tracking. You cannot thread with one RPM and then chase with a different.

 

[SeymourDumore]

The Root Radius of a UNJ External Thread states a maximum radius
Bill

Bill, unless I misunderstood your post, the J specification clearly states a pretty darn tight Min/Max Root Radius.
For example a 12 pitch UNJF is .0125 - .0150R

In the meantime, while it does not state a flat at the crest of the thread, it does also control the minor diameter within a min/max limit.

 

[angelw]

Bill, unless I misunderstood your post, the J specification clearly states a pretty darn tight Min/Max Root Radius.
For example a 12 pitch UNJF is .0125 - .0150R

In the meantime, while it does not state a flat at the crest of the thread, it does also control the minor diameter within a min/max limit.

Hello Seymour,
I'm referring to a Male Thread for consistency in this Thread.
I know that there is a Radius at the Root of the Thread, but the diameter at 6 o'clock on the Radius is smaller than the Minor Diameter of the Thread. The Standards that I refer to shows the Minor Diameter as a Flat 0.25H up from the intersection of the flanks of the Thread at the Root of the "V", with H being the Height from the intersection of the Thread Flanks at the Root of the "V" to the intersection of the Thread Flanks at the Crest of the "V". It also gives the distance across the truncated "V", 0.25H up from the intersection of the flanks of the Thread at the Root of the "V", as 0.25P.

Both these calculated values correspond exactly if you draw the sharp "V" Form and put the line in 0.25H up from the intersection of the sides of the "V" at the root.

Take a #10 x 32 for example, where the following applies:
1. The Pitch in mm is = 0.79375
2. The height of the sharp "V" form is 0.68741
3. 0.25H = 0.17185
4. The distance across the root of the "V", where the line 0.25H up from the intersection of the "V", should equate to a value of 0.25P
5. 0.25P = 0.19844

If you draw the above geometry, the distance across the root of the "V" where the line 0.25H up from the intersection of the sides of the "V" is in fact, 0.19844.

6. If you draw a circle that is tangent to the flanks of the "V" where the 0.25H line intersects, the radius is 0.11457.

Regards,

Bill