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.
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)
WARNING THIS IS NOT THE SAME ON ALL FANUC CONTROLS
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.
Conclusion
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.
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 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…….
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.
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
