G71 and G70 Use to Rough and Finish Turn

G71 and G70 Use to Rough and Finish Turn

New video about the G71 roughing cycle on a Haas or a Fanuc control, also covers the G70 finishing cycle.

Call David: 07834 858 407


G71 is sometimes known as a canned cycle when in fact it is a multi repetitive cycle. The G70 cycle goes with it and can pick up the same lines to finish.

The N numbers are important as the cycle uses these as the points of reference to jump to.

G71 cycle interprets the shape between these two N numbers and then breaks up the shape for roughing.

“Read More”

G84 Rigid Tapping Program Example

G84 Rigid Tapping Program Example

For On-site CNC Training Contact David: 0783 858 407

G84 is a tapping canned cycle.

G84 taps holes.

This simple part has four M12 holes, drilled, countersunk and tapped. The datum is the centre of the part so the holes positions are.

X55. Y55.
X-55. Y55.
X-55. Y-55.
X55. Y-55.

G84 Rigid Tapping Program Example

G84 Rigid Tapping Program Example

Here is the CNC code

G84 Rigid Tapping Program Example

The machine first moves to X-55. Y-55. and rapids the Z axis to 3mm above the part.

G84 Rigid Tapping Program Example

The G95 selects feed per revolution which means we only need to program the tap pitch for the feed-rate.

See full rigid tap G84 Rigid Tapping Program Example

The M29 engages the rigid tapping mode and the S800 is the speed. (It does not start the spindle)

It then rapids the Z axis down to 1mm above the part R1.

The G84 Cycle instructs it to tap a hole 17.mm deep (Z-17.) at a feed of 1.75mm per revolution (F1.75) 

So it feeds at 1.75mm per revolution with the spindle turning clockwise to depth.

At the bottom of the hole it reverses the spindle and feeds back to the initial point.

This initial point was in the line.

G84 Rigid Tapping Program Example

This is because of the G98.

If it were G99 it would return to 1mm above the job (R1.)

See explanation of G98 and G99

Once the cycle is active each time it sees a position it repeats the tapping process.

When the G80 is programmed it no longer taps holes.

Single block and feedhold do not work in a tapping cycle.

Why? You ask.


Now watch the video to see it all in action (not breaking the tap).


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

If you want to learn to program CNC Milling Machines

Look no further Contact CNC Training Centre




G10 Using G10 on a Fanuc Type Control


I am always amazed that so many companies still don’t use G10 in their CNC programs. If you know you know.

I must admit I fuckin hate a lot of the things that young people say like “can I get a Latte”. (Get behind this fuckin counter and make it yoursef if you want to “get it”).

Anyway I kind of like “If you know you know”

No G10… Is this you?

I am sure you have your reasons which I will accept. But if your reason is that you don’t understand it then that’s just not good enough.

So you make a part, it’s all setup and you need to break it down.

If you can fix the work holding in such a way that you can reload it in exactly the same place then you need G10.

Let me explain, watch this video to see how single point location works.

G10 No need to spend loads of money.

You could just bolt a sub plate to your machine table so that vices and chucks etc can have dowels to locate them.

But the main idea is that you can relocate your work holding in exactly the same place every time.

Using G10 on a Fanuc Type Control

This is your work offset page on a Fanuc control.


These figures are written in by hand or by automatic setting.

If you had written this line in your program.

G90 G10 L2 P1 X-440.500 Y-265.200 Z-443.00

They would have been written in automatically when you ran the program.

So the work offset page could have any values in G54 but as soon as you run your program this G10 command will replace them with its preset values.

Make Sure Your in Absolute

Try not to forget the G90 (Absolute) because you may accidentally be in G91 (Incremental). What would then happen is it would add these numbers to what is already in the work offset. Oh dear me.

In G90 it will always replace them.

You can write to G54 G55 G56 G57 G58 or G59 just by changing the P number.

G90 G10 L2 P1 X-140.600 Y-265.923 Z-400.00 (G54)

G90 G10 L2 P2 X-125.500 Y-236.865 Z-313.865 (G55)

G90 G10 L2 P3 X-800.500 Y-563.200 Z-125.00 (G56)

G90 G10 L2 P4 X-440.500 Y-265.200 Z-169.369 (G57)

G90 G10 L2 P5 X-440.500 Y-265.200 Z-123.568 (G58)

G90 G10 L2 P6 X-410.500 Y-235.200 Z-443.00 (G59)

The code above would setup all six work offsets.

What about the L2 you ask?

What’s that for?

L2 means you are writing to the work offsets (G54- G59)

But you can also write to the tool length offsets in which case it would be

G10 L10 P1 R200. (200 length into tool 1)

G10 L12 P1 R10.(10mm radius into tool 1)


Look David, I Have Shit Loads of Offsets

Don’t need your stupid G10.

Now I know some of us do have more offsets than you can shake a cheap memory stick at, but……..

With G10 it’s fixed in program so if some daft bastard alters your precious work offset you don’t give a flying monkey’s shit. Your program just reloads it.


G10 means your datum positions are saved with your CNC program.

The vice or fixture needs to be in exactly the same place when you next set it up.

You can use special single point location fixturing or just make a sub plate.

It’s great for horizontal machines.

Haas G10


G0 Cancels Canned Cycles

G0 Cancels Canned Cycles, this is not a news flash it’s always been the case.

G0 Cancels Canned Cycles

O0001(G28 Example)
G21 G90 G40


G90 G0 G54 X200. Y0 S1500 M3
G43 Z3. H1 M8
G81 G98 Z-5. R1. F100.
G0 X25. (No hole drilled here cycle would be cancelled)
G80 (This also cancels the cycle)

“Read More”

G76 Chamfer End of Thread

Tags :

Category : Fanuc Turn New Stuff

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

G76 Threading Cycle Explained

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

If you want to learn to program CNC Milling Machines



WP to LinkedIn Auto Publish Powered By : XYZScripts.com