G92 crossthreaded after G76

[sinha]

Thank you Bill for letting us know.

 

[SeymourDumore]

Hello Seymour,


I had the opportunity to run the G76/G92 test program I listed in an earlier Post, on a client's 2006 SL-20T today, but with the two line G76 cycle written using the single line format used by HAAS. With the "A" address specified as Zero in the G76 Cycle, the G92 Cycle had the tool track perfectly in the Thread Groove already cut. With the "A" address specified as 60 in the G76 Cycle, the G92 Cycle, starting at the same Z point as initial Z position for the G76 Cycle, wrecked the thread.

Bill

Bill

Haas SL10 - Year 2001 - Version 4.26
Haas Mini Lathe - Year 2003 - Version 5.07

Both machines follow the same path using the A60 definition with G76 and G92
I can show the pictures of finished parts, and perhaps take a video of the coords screen, but I do not know if the single block would help as the machine does not stop anywhere in the thread cycle
other than the start point.

Other than that, I don't know what else to say...

 

[sinha]

Certain things stated in manuals are somewhat different from what is practically observed.
For example, the manual says that the acceptable range of values for Pxx---- is 1 to 99. However, P00---- also works, eliminating finishing passes. This will, of course, leave the finishing allowance unmachined which may not be desirable. Probably because of this reason, the manual suggests P01---- as the minimum value.

I have a query:
How many passes does it execute - 1 or 2?
If it is 1 (since the minimum DOC is Q400), it will not "machine" up to the bottom of the thread (476-400 = 76 will be left out). In such a case, only burrs will be removed, which might be the sole objective.
Even if it executes 2 passes, ignoring the minimum DOC requirement, to reach the bottom of the roughing depth, it will still leave the finishing allowance (R5) untouched.
R5 in the first G76 and R0 in the second will shift the helix, spoiling the thread.

Correction:

Even if P00---- is specified, the control ignores it and executes one finishing pass, as if P01---- is specified.

 

[sinha]

Bill

Haas SL10 - Year 2001 - Version 4.26
Haas Mini Lathe - Year 2003 - Version 5.07

Both machines follow the same path using the A60 definition with G76 and G92
I can show the pictures of finished parts, and perhaps take a video of the coords screen, but I do not know if the single block would help as the machine does not stop anywhere in the thread cycle
other than the start point.

Other than that, I don't know what else to say...

Possibly, it ignores A60 and uses straight feed?

 

[sinha]

Any discussion should come to a conclusion. Therefore, I have compiled what I gathered from the ongoing discussion. Please suggest any modification ...

How to chase a previously-made thread on a Fanuc machine
If a thread made by G76 is to be chased by G92 on a Fanuc, the start Z for G92 must be shifted appropriately to make the two threads coincide, because G76 shifts the threading helix axially.

All roughing passes of G76 shift in Z to ensure single-edge cutting. However, the finishing passes do not shift in Z, and machine both the surfaces. All the finishing passes are at the same X level (target X), and their helices coincide (axially) with the last roughing pass. Therefore, only the first finishing pass cuts material, and all subsequent finishing passes are spring passes. Accordingly, the final helix of G76 shifts by a distance of a tan θ to the left (or right, depending on the direction of the feed) with respect to the initial Z position of the tool, where
θ is the half of the angle of the thread, and
a = (Height of the thread – Finishing allowance/2)
(Assuming, the finishing allowance is on diameter, as usual)

For example, assume that the original thread (10 TPI) is made by (in inch mode)
G00 X3.2 Z-0.5
G76 P020055 Q40 R0.002
G76 X3.5292 Z-2.9 P556 Q100 R0 F0.1
Therefore, a = 0.0556 - 0.001 = 0.0546
Axial shift in the final helix = 0.0546 tan 27.5° = 0.0284 (to the left)
Accordingly, the start Z for G92 should be shifted by this amount to the left of the start Z for G76, i.e., to Z-0.5284, which will make G92 coincide with the thread made by G76. A single pass of G92 would finish the thread:
G00 X3.2 Z-0.5284
G92 X3.5292 Z-2.9 R0 F0.1

On the other hand, if a thread made by G76 is to be chased by another G76, then at least one roughing pass (corresponding to the last roughing pass of the previous G76) and one finishing pass (at the target X) will be required. For this, in the second G76,
1. The same R (finishing allowance) must be used; otherwise, the threads will not match.
2. The first DOC may be made equal to (or more than) the height of the thread, which will result in a single roughing pass.
3. The minimum DOC can have any value less than the height of the thread, as it will not come into the picture.
4. P01---- will execute one finishing pass. Note that P00---- is ignored by the control and interpreted as P01----

Thus, the second G76 can be
G00 X3.2 Z-0.5
G76 P010055 Q40 R0.002
G76 X3.5292 Z-2.9 P556 Q556 R0 F0.1
where the changes from the original G76 are marked in red.

Note that the setup including the tool as well as the RPM must be the same.

Conclusion: Chasing by G92 involves just one pass, but it requires calculation of the axial shift. On the other hand, chasing by G76 is straightforward, but minimum two passes will be there.

 

[SeymourDumore]

Possibly, it ignores A60 and uses straight feed?

That is what I was suggesting in an earlier post.

For example, my manual talks about various infeed methods, but it says it is not yet implemented.
P1 = single edge, load constant
P2 = Two edges, load constant
P3 = Single edge, depth constant
P4 = Two edges, depth constant

P2, P3 and P4 not implemented, defaults to P1

So, it possibly does ignore the A word, but then how could it cut a good Acme thread?

 

[sinha]

That is what I was suggesting in an earlier post.

For example, my manual talks about various infeed methods, but it says it is not yet implemented.
P1 = single edge, load constant
P2 = Two edges, load constant
P3 = Single edge, depth constant
P4 = Two edges, depth constant

P2, P3 and P4 not implemented, defaults to P1

So, it possibly does ignore the A word, but then how could it cut a good Acme thread?

Please check the manual. Does it talk about A-word? If not, it is simply ignoring it, without generating alarm.

As regards ACME threads, these can be cut using both 29 degree and 0 degree (in fact, any value less than or equal to 29 degree).

 

[angelw]

That is what I was suggesting in an earlier post.

For example, my manual talks about various infeed methods, but it says it is not yet implemented.
P1 = single edge, load constant
P2 = Two edges, load constant
P3 = Single edge, depth constant
P4 = Two edges, depth constant

P2, P3 and P4 not implemented, defaults to P1

So, it possibly does ignore the A word, but then how could it cut a good Acme thread?

Hello Seymour,
Run the program you Posted earlier in fresh air and with Dry Run turned on. This will allow you to slow the program down in the area where the First and subsequent DOCs are applied. If the "A" word is being used, you will see an initial movement in X and Z; if not, then its being ignored by the control. If the latter, then it's understandable why G92 would work to chase the thread machined using G76, as both would be starting at the same Z position, applying each DOC perpendicular to the Z axis.

Both machines follow the same path using the A60 definition with G76 and G92

Are you meaning to say that both G76 and G92 are using a A60 definition? I know for absolute certain that neither the Fanuc, nor HAAS control are able to apply a Tool Tip angle to compound Thread cut with G92.

Regards,

Bill

 

[sinha]

Any discussion should come to a conclusion. Therefore, I have compiled what I gathered from the ongoing discussion. Please suggest any modification ...

How to chase a previously-made thread on a Fanuc machine
If a thread made by G76 is to be chased by G92 on a Fanuc, the start Z for G92 must be shifted appropriately to make the two threads coincide, because G76 shifts the threading helix axially.

All roughing passes of G76 shift in Z to ensure single-edge cutting. However, the finishing passes do not shift in Z, and machine both the surfaces. All the finishing passes are at the same X level (target X), and their helices coincide (axially) with the last roughing pass. Therefore, only the first finishing pass cuts material, and all subsequent finishing passes are spring passes. Accordingly, the final helix of G76 shifts by a distance of a tan θ to the left (or right, depending on the direction of the feed) with respect to the initial Z position of the tool, where
θ is the half of the angle of the thread, and
a = (Height of the thread – Finishing allowance/2)
(Assuming, the finishing allowance is on diameter, as usual)

For example, assume that the original thread (10 TPI) is made by (in inch mode)
G00 X3.2 Z-0.5
G76 P020055 Q40 R0.002
G76 X3.5292 Z-2.9 P556 Q100 R0 F0.1
Therefore, a = 0.0556 - 0.001 = 0.0546
Axial shift in the final helix = 0.0546 tan 27.5° = 0.0284 (to the left)
Accordingly, the start Z for G92 should be shifted by this amount to the left of the start Z for G76, i.e., to Z-0.5284, which will make G92 coincide with the thread made by G76. A single pass of G92 would finish the thread:
G00 X3.2 Z-0.5284
G92 X3.5292 Z-2.9 R0 F0.1

On the other hand, if a thread made by G76 is to be chased by another G76, then at least one roughing pass (corresponding to the last roughing pass of the previous G76) and one finishing pass (at the target X) will be required. For this, in the second G76,
1. The same R (finishing allowance) must be used; otherwise, the threads will not match.
2. The first DOC may be made equal to (or more than) the height of the thread, which will result in a single roughing pass.
3. The minimum DOC can have any value less than the height of the thread, as it will not come into the picture.
4. P01---- will execute one finishing pass. Note that P00---- is ignored by the control and interpreted as P01----

Thus, the second G76 can be
G00 X3.2 Z-0.5
G76 P010055 Q40 R0.002
G76 X3.5292 Z-2.9 P556 Q556 R0 F0.1
where the changes from the original G76 are marked in red.

Note that the setup including the tool as well as the RPM must be the same.

Conclusion: Chasing by G92 involves just one pass, but it requires calculation of the axial shift. On the other hand, chasing by G76 is straightforward, but minimum two passes will be there.

Since this is an important topic, I have copied it on the description page of my book on threading. One can read it without purchasing the book. Google "G76+sinha" in the "book" category of amazon.com to reach the book page CNC Programming Skills: Understanding G32, G34, G76 and G92 on a Fanuc Lathe, Sinha, S. K., eBook - Amazon.com

 

[SeymourDumore]

Are you meaning to say that both G76 and G92 are using a A60 definition? I know for absolute certain that neither the Fanuc, nor HAAS control are able to apply a Tool Tip angle to compound Thread cut with G92.

Regards,

Bill

No Bill

I said that using the A60 definition in the G76 cycle will still result in the same toolpath in the follow-up G92 cycle.

I will look into somehow capturing the actual start positions in the cycles.