Fanuc 6T G76 single line code gives an error

[BodoW]

Hi,
I'm trying to find the right syntax for the G76 cycle on a Fanuc 6T.
I wrote this but I get an alarm message with just program but I don't know what is wrong.
The alarm pops up when the G76 Part is reached. I wanna make a UNS 2-10 Thread.
Here's my code:
% TABLE-POST THREAD UNS 2-10
O1500
N1 G50 S2000
N2 G00 T0202
N3 G97 S250 M03
N4 G99
N5 G00 X10. Z1.5 M08
N6 X1.998
N7 G76 X1.8552 Z-5. I0 K.0714 D.020 F.100 A60
N8 G00 X2.5
N9 X 6. Z10. M09
N10 T0200
N11 M05
N12 M30
%

Can somebody who knows the G76 single syntax give me please some advice.
In the Operators manual is an F or an E for the Lead of the Thread mentioned but nothing about the difference
between both. Only that it's with E more accurate. I think they have to write an explanation book for the manual or I'm just to stupid.

Greetings
Bodo

 

[Dan from Oakland]

Have you programmed a single line G76 on this machine before? Are you sure the control does not require a 2 line G76? If you had posted the error code it would make it easier to help you solve the problem.

 

[DouglasJRizzo]

Every 6T I've seen wants the single line G76.
I always used the "F" for thread lead.
One issue I used to see a lot was people starting the tool too close to the work and clipping the threads.

 

[BodoW]

Hi,
I've tried around and the error came from the D-value.
I had D.020 and I got the error (program).
When I changed the value to D0200 it cuts the Thread without error.
It seems that to go with decimals is ok except the value for D for the first cut depth.
In the operators manual is an example in metric but there is all without decimals.
All is in microns (metric). For Imperial it seems to be in 10th.

For you Dan, this 6T model B has no double line G76. Only single line and I'm just trying my first Threads with this machine.

Thanks so far
Bodo

 

[angelw]

...

I've tried around and the error came from the D-value.
I had D.020 and I got the error (program).
When I changed the value to D0200 it cuts the Thread without error.
It seems that to go with decimals is ok except the value for D for the first cut depth.
In the operators manual is an example in metric but there is all without decimals.
All is in microns (metric). For Imperial it seems to be in 10th.

For you Dan, this 6T model B has no double line G76. Only single line and I'm just trying my first Threads with this machine.

Hello Bodo,
I got called away when I was about to answer your first Post, as I was going to suggest that its the Decimal used in the D value that is probably causing your problem.

The Least Programmable Increment for your machine in Metric Mode is 0.001mm and 0.0001" in Imperial Mode. You can specify the value with more decimal places, but the Control will simply only read 3 decimal places for Metric and 4 places for Imperial, it doesn't round the value.
.
Having your X Start position the same as the Major Diameter (External Thread as in your example) of the Thread is not good practice, for unless the Threading Insert is Full Form, its likely to scrape the Thread OD on the return to the Z Start position. The OD of the Thread is calculated by the Control using the X value (Minor Diameter in this case) and Thread Height specified by K in the G76 Block as follows:

MD = X + 2K
MD = 1.8552 + 0.0714 x 2
MD = 1.998
Where:
MD = Major Diameter

Accordingly, the X Start position can be any value greater than the Major Diameter of the Thread (for an External Thread). Not that it would be practical, but a value such as X10.0 would work to cut the Thread successfully, for the Control calculates the Major Diameter as explained above and applies the first and subsequent DOC from there, NOT from the X Start position that the Threading Tool is parked at. Therefore, specify the X Start as a value that clears the OD (Male Thread) by at least, say, 0.040"

The Spindle Speed of 250RPM is way too slow, if the Threading Tool is Carbide. The main limiter of RPM when Screw Cutting is the actual maximum slide velocity of the machine (Thread Lead x Spindle RPM). My typical start up RPM for something like a M30 x 1.5 Thread in circa high 30's RHC (150M per Minute) is circa 1500 and I go from there. Cutting with such a slow RPM on such a small diameter as in your example is likely to result in a poor finish and built-up edge of the insert if carbide.

Regards,

Bill

 

[BodoW]

Hi Bill,
thanks for your advice.
As I mentioned in a different Thread I am new to the CNC stuff and I'm trying to handle the machine just by practical learning, Youtube, Practical Machinist aso.
I didn't get a course in this and I have nobody else to ask questions I have.
Not an easy situation but I'm ok so far.

For the speed, I made before a Thread on a manual Lathe and there I had to keep it slow not to go to far against a shoulder. So I could react and the Thread went well.
You say on a CNC I can run it much faster. I will try it tomorrow.
But what is with an internal Thread. Can I run it faster too?
I have a 1" HSS Boring Bar with a carbide insert and have to make a Nut for my OD Thread.

Before I used Camworks for the internal Thread but Camworks knows only G92 cycles...
Camworks parked the Boring Bar as I did with the external Thread.
That's how I came to this way to position it.
If it's not necessary then I can handle it in a different way as you told me.

I've tried the internal Thread and with around 400rpm I got chatter.
This was from Camworks the code.
But the result was not so good, means out of 4 only 1 Nut works with my external Thread.
I guess I have to try more.

Btw. Do you or somebody else knows a NC Editor which can simulate G76 single line cycles?
The Camworks NC Editor doesn't understand the G76 code for the external Thread.
I have GWizard Editor too but although no simulation result for G76 single line.
Is G76 single line too old for these Editors?
I mean it would be nice to see on a screen what's going on before I hit the cycle start button.

Regards and Thanks
Bodo

 

[William Lynn]

Run the thread cycle with a slow spindle speed and with out a part to get familiar with the tool path. Watch it closely, assuming you can have the door open while in cycle. Does your lathe have a graphics function?

 

[DouglasJRizzo]

The "D" may want the decimal eliminated. So for a DOC of .02", perhaps try D0200.

 

[maguilera]

Just as a sanity check, your program is in imperial units, right?

If that’s the case and assuming Z0 is at the face of the part, starting the threading at Z1.5 will result in a lot of unnecessary air cutting. From advices I’ve seen in this forum and real life experience, a good rule of thumb is to keep the Z starting point away from the part face by 3 times the thread lead in order to give the machine enough time to accelerate to the required linear velocity before engaging the part.

But what is with an internal Thread. Can I run it faster too?
I have a 1" HSS Boring Bar with a carbide insert and have to make a Nut for my OD Thread.

I've tried the internal Thread and with around 400rpm I got chatter.

How much overhang does the boring bar have? For a steel boring bar it is usually recommended to keep the overhang at 4xD, more than that and it will be prone to chattering.

Btw. Do you or somebody else knows a NC Editor which can simulate G76 single line cycles?

It’s easy to write a program in Python (or some other programming language, for that matter) to calculate the X and Z values the G76 cycle will spit out.

 

[BodoW]

The "D" may want the decimal eliminated. So for a DOC of .02", perhaps try D0200.

Hi Doug,
yes, that I already found out.
Regards
Bodo

 

[BodoW]

Run the thread cycle with a slow spindle speed and with out a part to get familiar with the tool path. Watch it closely, assuming you can have the door open while in cycle. Does your lathe have a graphics function?

Hi William,
That's the way I do now if the simulation doesn't show me what I need to know.
I although do the first run with a part with single block and watch the position where it tells "way to go".

graphics function would be nice to have but 1984 it wasn't available.
Regards
Bodo

 

[BodoW]

Just as a sanity check, your program is in imperial units, right?

Yes

If that’s the case and assuming Z0 is at the face of the part, starting the threading at Z1.5 will result in a lot of unnecessary air cutting. From advices I’ve seen in this forum and real life experience, a good rule of thumb is to keep the Z starting point away from the part face by 3 times the thread lead in order to give the machine enough time to accelerate to the required linear velocity before engaging the part.

I will change that but it was just my first Thread on a CNC so I wanted to be safe.

How much overhang does the boring bar have? For a steel boring bar it is usually recommended to keep the overhang at 4xD, more than that and it will be prone to chattering.

I keep it at 3" overhang, max 3.5 x D.

It’s easy to write a program in Python (or some other programming language, for that matter) to calculate the X and Z values the G76 cycle will spit out.

If I have some time I will try that.
Thanks

Regards
Bodo