G76 Chamfer End of Thread

G76 Chamfer End of Thread

Tags :

Category : Fanuc Turn

G76 Chamfer, this is another myth exploding article about the G76 threading cycle.

It’s so easy to use cycles like G76 day in day out and never really fully understand how they work.

I certainly did and then one day I thought “Fuck this I need to know more” 

That’s when I sorted out the number of passes thing. If you don’t know how to calculate the number of passes in a threading cycle then you should read the article above.

(G76 Chamfer) I want to talk about the P

G76 P011560 Q20 R.02
G76 X16.93 Z-25. P1534 Q485 F2.5

G76 Threading Cycle First Line
P01   One spring pass       15   Chamfer        60   Thread angle
Q       Minimum depth of cut
R       Finishing allowance

G76 Threading Cycle Second line

X         Core diameter of thread
Z         Thread end point
P         Depth of thread (as a radius no decimal point)
Q        Depth of first cut no decimal point.
F         Pitch of thread

Six Figure P Number Holy Shit

G76 P011560 Q20 R.02

First two digits are easy, spring cuts. No it’s not the latest haircut for April.

It’s how many times it goes over the thread when it’s done. It just shaves off those last pieces of metal.

Oh and the last two are the thread angle like 60 degrees or 55 degrees.

But the middle two…….

G76 Chamfer

Do I need to say anymore.

I have read so many articles on this and they all gloss over this bit or just plain ignore it.

Here is an extract from a manual.

 

Now I know I’m a bit thick but what the fuck does that mean?

First of all why would you want a chamfer at the end of your thread? Well it’s obvious really.

Oh and by the way it’s not really a chamfer, which itself is confusing.

It’s the thread running off the part.

If you kept tightening a bolt it would eventually shear. That shear point would be the weakest part of your thread. That is the point where the thread runs out.

 

G76 Chamfer

Those middle two digits are to give you this run out. The tool comes out of the thread at an angle.

Now you might be thinking “I’ve done this for years and nobody gives a shit about this”.

Well you are wrong, if you ever worked for Rolls Royce you will know that aircraft threads are really strict on this.

This means if you screw a nut onto it, then it will tighten up as it gets closer to the end.

And obviously this takes away that shear point and makes the thread stronger.

The middle two numbers of the P value are multiplied by the pitch of the thread. The result would be the length of the run out.

There is no decimal point so P011516 the middle two numbers (15 ) would be taken as 1.5

So in the example:

G76 P011560 Q20 R.02
G76 X16.93 Z-25. P1534 Q485 F2.5

The pitch of the thread is 2.5 (F2.5) and the middle two digits of the P number are 15 it would be

1.5 x 2.5 = 3.75

This means the tool would run off the part over a distance of 3.75mm

G76 Chamfer

If enter 00 in the middle two digits P010060 you get 45 degree angle.

Older Controls Oi 6T etc

On a 6T control you set this value in parameter 64

On the Oi control it’s parameter 5130 and 5131

Haas G76 explanation

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 program CNC Milling Machines

Look no further Contact CNC Training Centre

 

 


1 Comment

Dave Hutchins

August 23, 2020 at 6:07 pm

Thank you for making this process clear.

Log out of this account

Leave a Reply

CNC Training Centre
WP to LinkedIn Auto Publish Powered By : XYZScripts.com