G76 Threading Start Point (Where Do you Start?)

G76 Threading Start Point (Where Do you Start?)

Tags :

Category : Fanuc Turn New Stuff

G76 threading start point, when you use a G76 threading cycle on a CNC Lathe the position that you start the tool at is really important.

This is the position you rapid the tool to just before you call the G76 threading cycle.

For example how does the control know if you are producing an internal thread or an external thread.

Actually I learnt this the hard way. It was on an old machine.

G76 threading start point

Maybe not that old. Anyway I couldn’t get it to perform a G76 threading cycle. It was cutting an external thread but the tool was working it’s way outwards.

What to do Next?

Everything rushed through my head, senile dementia, flashbacks from a misspent youth, did I feed the dog?

Anyway I suddenly realised I didn’t have a dog and that the start position of the tool was wrong.

G76 threading start point how was it wrong?

Well that’s how the machine knows whether you want an internal or external thread. Your start point needs to be inside or outside the thread. What a fuckin dipstick I was.

I had the tool just below the external diameter of the thread. If you do this the machine thinks the thread is internal and therefore cuts outwards.


G76 threading start point

So providing the tool is initially placed outside of the maximum diameter it will do exactly what you want.

IncorrectG76 threading start point

Put it here and you are in deep shit. The tool will work from this position backwards and you will be totally confused.

Don’t say I didn’t warn you.

Here is a example of a 20mm external thread.

G0 X21. Z3.
G97 S1200 M3

G76 P010060 Q20 R.02
G76 X16.93 Z-25. P1535 Q485 F2.5

This thread has a core diameter of 16.96 (X16.93) the thread depth is 1.535 (P1535).

Soooo…… 16.93 + (1.535 x 2) = 20

G76 threading start point

Therefore you must first position the tool outside that 20mm diameter.

If you don’t do this then your tool will try and cut away from the 20 mm diameter.

Wrong as Below

G0 X19.95 Z3.
G76 P010060 Q20 R.02
G76 X16.93 Z-25. P1535 Q485 F2.5

So be careful because you might not notice that tiny amount.

Of course if you have a Siemens control Sinumerik 828 840D then this does not apply because you have to specify if the thread is internal or external in the cycle.

Front Clearance (G76 threading start point)

Now let’s think about how far in front of the part you need to be with the threading tool.

Maybe you never thought about it?

Well now’s the time.

Spare a thought for people like me who lie awake at night ruminating about these things. If you don’t know what ruminating means then maybe you shouldn’t be reading this article. Or maybe you just like the pictures.

This is my puppy his name is Donald he is learning to programme a G71 woofing cycle.

Lets take another look at the code.

G0 X21. Z3.
G97 S1200 M3

G76 P010060 Q20 R.02
G76 X16.93 Z-25. P1535 Q485 F2.5

The spindle starts at 1200 rpm and the feedrate (which in the case of a thread is the pitch) is 2.5 mm per rev.

2.5 x 1200 = 3000

So the machine will be feeding at 3000 mm per minute along the thread.

So at the start of the thread you have 3 mm of clearance (Z3.)

Therefore in that 3 mm the machine has to accelerate up to 3000 mm per minute.

If it does not accelerate quick enough you will get a pitch error, your thread will be wrong.

Strange Behaviour

Ever had a thread where you can’t get the gauge on then suddenly it goes on only to find the thread is really loose further down?

Maybe you had a pitch error.

Taking it further if I double the speed

G0 X21. Z3.
G97 S2400 M3

G76 P010060 Q20 R.02
G76 X16.93 Z-25. P1535 Q485 F2.5

2.5 x 2400 = 6000

Now I need to feed at 6000 mm per minute so this pitch problem will be twice as bad.

Can you see where this is going?

Eat more fish.

No not really, well it is good for you but it’s not what I meant.

The faster you go and the courser your thread pitch the quicker the machine will have to feed.

If you have a coarse pitch thread in aluminium you probably will end up with a super high feed-rate your machine can’t even achieve.

This will all depend on the age of your machine but you must always make this calculation just in case you are trying to cut a thread at the speed of light.

G76 threading start point in Z Axis

This start point distance is really important because it will allow the machine to get up to speed.

I can’t give you exact figures for this, not because I can’t be arsed but because it will vary depending on your machine.

The machine will have a maximum feedrate and it will be in the manual.

You know that old book that you use to prop  the door open.

The bigger you make this Z figure the more time your machine will have to get up to speed.

So don’t forget if you are starting at Z1. then the poor old machine doesn’t have much time to get up to speed.


G76 threading start point

Thanks for watching and reading

If you have been affected by any of the issues in this post or need CNC Counselling then contact me.

Siemens 828 840 Sinumerik Training

Or call us

If you want to learn to programme CNC Milling Machines

Look no further Contact CNC Training Centre





Alan ball

December 11, 2022 at 5:20 pm

Would the machine not do the g97 before the threading cycle so it would be upto speed already?


    December 15, 2022 at 3:07 pm

    The spindle would be OK but it has to accelerate up to the correct feed-rate

Log out of this account

Leave a Reply

WP to LinkedIn Auto Publish Powered By : XYZScripts.com