g76 cycle machine issues

[Rogue_Machinist]

So I recently posted about my one machine not being able to use g76 but able to use g32. However I found the users manual and it can accept the g76. But the program runs on that machine very poorly. Bascially making the first thread pass at what seems like .020".
I didnt write this because I dont like cutting NPT threads but this is what is in a newer machine and it runs like a champ.

N200(THREAD TOOL)
G00 G97 X10. Z10. S250 T0404 M03
X1.5 Z1.
G01 X1.315 Z.2 F.125 M08
G76 P020260 Q0020 R0005
G76 X1.1756 Z-.9845 P0348 Q0050 R-.0305 F.086
Z.5
M09
G00 X10. Z10.
T0400
M30

This is not a production shop so the program isnt written for speed its written for a few parts here and there. Any input would be good. As I said this runs fine on our newer Doosan Machine same tooling. But our older machine doesnt like it.
Oh and this is for a 1" NPT. Thanks

 

[Ox]

What is it exactly that you don't like about it?
The .020 first pass?
You want more or less?

And you are comparing two parts that are all adjusted in X to produce a good part to the ring gauge?

But:

Your P should be 0574
Your Q should be 0157
Your R should be 0740 (or maybe 0370 if R is in R(rad) and not D(diam), but I don't think so?)

Then adjust X to git a good part.

You would need an L2 gauge to check your taper.
(along with your L1)


Not sure I guess what "doesn't like" means?
Won'tr run the line, or doesn't make a good part?
Your older machine may need a 1 line G76?
I have no experience with those.
What is the control on "the old machine"?


---------------------

Think Snow Eh!
Ox

 

[Rogue_Machinist]

What is it exactly that you don't like about it?
The .020 first pass?
You want more or less?

And you are comparing two parts that are all adjusted in X to produce a good part to the ring gauge?

But:

Your P should be 0574
Your Q should be 0157
Your R should be 0740 (or maybe 0370 if R is in R(rad) and not D(diam), but I don't think so?)

Then adjust X to git a good part.

You would need an L2 gauge to check your taper.
(along with your L1)


Not sure I guess what "doesn't like" means?
Won'tr run the line, or doesn't make a good part?
Your older machine may need a 1 line G76?
I have no experience with those.
What is the control on "the old machine"?


---------------------

Think Snow Eh!
Ox

The first pass of .020" is causing insert chipping. I would like more even thread passes.

And the customer doesnt require super precision they just need between 2.5 and 3 turns of a machined stainless 1" female NPT fitting.

And the Older machine is using a FANUC O-T control. The machine is from 1989. And what I mean by dont like it is because for the last 30 years our shop has always just run these 1" pipes through a pipe threader. And now that threader is shot and wont be replaced. So making tapered threads is just something id rather not do.

So the first or second Q do I need to change? And the Machine uses diameter mode. Im pretty sure.

 

[Ox]

So I recently posted about my one machine not being able to use g76 but able to use g32. However I found the users manual and it can accept the g76. But the program runs on that machine very poorly. Bascially making the first thread pass at what seems like .020".
I didnt write this because I dont like cutting NPT threads but this is what is in a newer machine and it runs like a champ.

N200(THREAD TOOL)
G00 G97 X10. Z10. S250 T0404 M03
X1.5 Z1.
G01 X1.315 Z.2 F.125 M08
G76 P020260 Q0020 R0005
G76 X1.1756 Z-.9845 P0348 Q0050 R-.0305 F.086
Z.5
M09
G00 X10. Z10.
T0400
M30

This is not a production shop so the program isnt written for speed its written for a few parts here and there. Any input would be good. As I said this runs fine on our newer Doosan Machine same tooling. But our older machine doesnt like it.
Oh and this is for a 1" NPT. Thanks

So it's not that the older machine won't crunch the code?
Just that you don't like the results?
I Shirley don't know why you would be getting different results between the machines?
Is the tooling exactly the same?

Also - for 30 years your RIGID threader has put the correct taper on the threads, so it would seem that you might want to make sure that the new machine is right too?
Just pick up an L2 used on Ebay. That will just fine for checking your taper. (along with the L1 that you already have - right?)

And now that threader is shot and wont be replaced. So making tapered threads is just something id rather not do.

Not sure what that means?



I JUST posted these in another threading thread this last week, but here they are aggin:
"Open in New Tab" for best results

--------------------

Think Snow Eh!
Ox

 

[Rogue_Machinist]

My newer Doosan machine has no issues with this code the way its written. And has no issues with that first thread being too deep. Yes tool holder is the shank, same seat and same insert. So yeah I dont know why my code would have a different effect. And Ive been at this shop for 4 years and they have always used a ridgid pipe threader for NPT stuff. For the last 15ish years this shop has been less than "ultra precision". 99% of what we do is +/- .005" there is that 1% where we do +/- .0002" so. So I will see. But just thought something what wrong with my x or z for this older machine. And the taper is programmed via CAD and that machine these are being cut on is accurate to .0002" all day.

 

[Ox]

Well, so much for CAM....


-------------

Think Snow Eh!
Ox

 

[Ox]

Per Bill - R in this case is s'posed to be prog'd in radius.

https://www.practicalmachinist.com/...8-npt-g76-threading-cycle-390887/#post3768556


I would still want to check with both gauges to verify tho.

That would make your original R value right - not counting the .200" lead that you have.
Meaning that 1.1845" x .0625" = .074" (D)
Or .037 for rad.
(.0625" taper per inch Z on pipe threads)


----------------------

Think Snow Eh!
Ox

 

[Rogue_Machinist]

think my x value is wrong

 

[sinha]

So the first or second Q do I need to change? And the Machine uses diameter mode. Im pretty sure.

The first Q is the minimum DOC. The second one is the first DOC.

The first R is on diameter. The second R is on radius.

 

[KennyBoi]

Seems your X value is not far off but:
1. F should be F.087 (1/11.5=.08695)
2. 2nd G76 line P should be 0696, this could be why the big first cut
3. Taper, 2nd G76 line R should be R-.037, need to account for Z.200 start position

Unless you are turning the tapered major OD of the pipe thread first, the threading tool will be taking heavier cut at start of thread due to taper. Usually have to always walk in the X till you get the gauge to go for the first one. I usually always run a quick cleanup pass with the turn tool over the tapered OD to clean the crest of the threads and make easier to deburr.

 

[Rogue_Machinist]

Seems your X value is not far off but:
1. F should be F.087 (1/11.5=.08695)
2. 2nd G76 line P should be 0696, this could be why the big first cut
3. Taper, 2nd G76 line R should be R-.037, need to account for Z.200 start position

Unless you are turning the tapered major OD of the pipe thread first, the threading tool will be taking heavier cut at start of thread due to taper. Usually have to always walk in the X till you get the gauge to go for the first one. I usually always run a quick cleanup pass with the turn tool over the tapered OD to clean the crest of the threads and make easier to deburr.

I did some tweaking and got the program to run fairly well. And yes we are turning the OD of the pipe to a taper of 1.79° We got about 30 pieces before the insert chipped. Which I am ok with. Female fitting threads on 2.5 to 3 turns. Someone smarter than me needs to actually dimension pipe threads properly and have a guide. That person would be a life saver. LOL

 

[Vancbiker]

…..Someone smarter than me needs to actually dimension pipe threads properly and have a guide. That person would be a life saver. LOL

Isn’t that pretty much all in Machinery’s Handbook??? In any case that’s where I’ve gotten NPT data for the past 40+ years.

 

[Fancuku]

Someone smarter than me needs to actually dimension pipe threads properly and have a guide. That person would be a life saver. LOL

It's been there for over 100 years. It's called the Machinery's Handbook and in these modern time there are a few apps that will help you with that.

 

[Rogue_Machinist]

It's been there for over 100 years. It's called the Machinery's Handbook and in these modern time there are a few apps that will help you with that.

I have the latest edition and doesnt have any of that. Doesnt show thread start minor or root diameter. Sorry to break it but its NOT there. Its a very abstract guide. Im speaking the definitive numbers. Just like any other thread. But for a taper thread everything be based off the small end, i.e. root diameter, minor diameter(bottom most point of the thread. Just giving you L1 and L2 and D1 and D2 and no actual values.

 

[Rogue_Machinist]

So does this look correct for a 3" npt male thread?
If not ill be able to tweak it this weekend.


N300(3IN NPT THREAD)
G00 G97 X10. Z10. T0404 S350 M03
X4. Z1.
G01 X3.6 Z.2 F.05 M08
G76 P020060 Q0030 R0005
G76 X3.341 Z-1.2 P0373 Q0030 R-.0437 F.125
G00 X2. M09
G00 X10. Z10.
T1000
M30

 

[Ox]

It's prolly not a big deal, but I wouldn't want to be in G97 mode when turning a tapered thread.


---------------------

Think Snow Eh!
Ox

 

[David Ferguson]

I figured you would want G97 (constant surface speed off) for all threading to keep the feed/pitch of the thread constant.

 

[Ox]

I figured you would want G97 (constant surface speed off) for all threading to keep the feed/pitch of the thread constant.

OH yeah, my bad!
Free help - and worth every penny!

I think that I feel heat stroke commin' on?

--------------------

Think Snow Eh!
Ox

 

[angelw]

So does this look correct for a 3" npt male thread?
If not ill be able to tweak it this weekend.


N300(3IN NPT THREAD)
G00 G97 X10. Z10. T0404 S350 M03
X4. Z1.
G01 X3.6 Z.2 F.05 M08
G76 P020060 Q0030 R0005
G76 X3.341 Z-1.2 P0373 Q0030 R-.0437 F.125
G00 X2. M09
G00 X10. Z10.
T1000
M30

You're rather inconsistent with regards spindle speed and the data specified so that the control can calculate the Major Diameter of the Thread (for Male Thread). In your first listed code for the 1" NPT Thread you use S250 yet for the 3" NPT, you go to a greater spindle speed; normally you would decrease the spindle speed as the workpiece diameter increases. However. in both cases the actual surface speed is quite slow, particularly for the 1" NPT,

The Effective Major diameter of a 1" NPT is.1.2563". You will note that there is no reference required to be specified to alert the control of what the Major Diameter is. That's because it calculates that from the Minor Diameter (Male Thread) and the Thread Height specified by the following algorithm:

MD = X + 2P
Where:
MD = Major Diameter
X = Specified Minor Diameter
P = Thread Height in Radius (P value in the second G76 Block)

Therefore, from your listed code for the 1" NPT Thread:
MD = 1.1756 + 0.0348 x 2
MD = 1.2452" - Well below on the 1.2563 that it should be

The first DOC specified by Q in the second G76 Block is used in conjunction with the Major Diameter calculated by the control to determine the X coordinate of the First Pass of the Threading Cycle. In the above example, the Major Diameter is 0.0111 down on the actual MD, if the blank was turned correctly and so your first DOC (radius value) will be 0.0055" before the specified First Pass DOC is applied.

For the 3" NPT Thread, you have the numbers specified correctly for the control to calculate the Effective Major Diameter.

Regards,

Bill

 

[Rogue_Machinist]

The 1" was for a smaller machine with a weaker motors so the RPM were slower. I do adjust at the control as necessary and then save the program. But yeah I used all the data from the Machinist Handbook for the 3" and thats going into a newer bigger machine that can run much better. Sorry for the inconsistency.