G92 Threading Single Line Method

G92 Threading Single Line Method

G92 threading Cycle is something that concerns me. It’s sadly neglected. Now I know your’e probably saying “no one uses that old shit anymore”

Well you could be wrong.

G92 Threading works exactly the same as G76 except you need to program every pass. This would be a pain in the arse but hear me out.

The Haas G76 cycle does not have any facility for a spring pass. This is where you add extra cuts at the end of a threading cycle to take out any metal left from the tool pushing off.

On a Fanuc control you can put these extra spring passes in as part of the G76 cycle.

Read this if you need to know more.

If you want this on your Haas control or an old Fanuc control then you can do this.

G76 X16.93 Z-25. K1.534 D.485 F2.5

G92 X16.93 Z-25.
X16.93
X16.93

Just add the G92 after your G76 cycle and whatever X figure you want to go to.

The G92 is modal so you will need a G0 move to cancel it. The code above would give you three spring passes.

Here is a load more interesting stuff.

I hope you have enjoyed reading this article.

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

 

 


G76 Chamfer Haas end of Thread

Tags :

Category : Haas Turn

G76 Chamfer Haas, this is another myth busting 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.

Haas make this simpler as they just use one line as appose to the two lines on Fanuc.

Haas

G76 X16.93 Z-25. K1.534 D.485 F2.5

Fanuc

G76 P010060 Q20 R.02
G76 X16.93 Z-25. P1534 Q485 F2.5

These days people say “It’s not rocket science”. Sorry but this really is fuckin rocket science it’s so complicated.

“It’s not rocket science” what on earth is that all about.

I hate these phrases that people pick up on these days.

I was watching my favorite TV show “How to Look Ten Years Younger”.

It’s this TV program where they take a miserable old bastard like me and make them look 15 again.

Now I don’t have a problem with people saying “Oh my god”. I mean people have said it since God was a lad.

But this woman kept saying “Oh…………….My…………..God”  with long gaps between each word.

I thought about how annoying it was and suddenly realized everybody is fuckin doin it and it drives me bloody shitless.

Back To G76 Being Complicated

Remember I was on about how people use these cycles everyday without really understanding them.

Anyway I didn’t fully understand it so 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 G76 threading cycle then you should read the article above.

G76 Chamfer Haas, Setting 95 and 96

G76 Chamfer Haas

I have read so many articles on this and they either gloss over it, bullshit or just plain ignore it.

Why would you want a chamfer at the end of your thread anyway?

Well it’s obvious really.

Oh and by the way it’s not really a chamfer, which in 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

Setting 95 and 96 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 it”.

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.

Next time you are on a plane and it lands successfully without either of the wings dropping off you’ll know why.

G76 Chamfer Haas Setting 95

This is the number of threads you want it to run out over.

For example if you put 3.00 in here.

It would run out over 3 thread pitches. If your thread pitch was 2mm it would run out over a 6mm length (3 x 2 = 6)

G76 Chamfer Haas Setting 96

This is the angle of the thread run off.

If you put 20 in here it would run off at 20 degrees over the 6mm length above.

Be careful because the control doesn’t necessarily make sense of your figures. It’s up to you to make sure that the angle and the distance make sense.

See Below

G0 X22. Z3. G97 S1200 M3

G76 X16.93 Z-25. K1.534 D.485 F2.5

The one above has 5.00 in setting 95 and 45 in setting 96. 

So because setting 96 is 45 degrees it runs off at 45 degrees.

Setting 95 is 5.00 and the pitch is 2.5  (F2.5) so the length of run out is:

5 x 2.5 = 12.5.

It still finishes at Z-25. by the way.

The example above is a load of bollocks so please don’t try this at home.

No screw threads have been injured or destroyed in the making of this post.

You will notice the tool jumps back in the X axis. It is going back to its start point. That is the X22. on the line before the cycle.

Now Another Example

G0 X22. Z3. G97 S1200 M3

G76 X16.93 Z-25. K1.534 D.485 F2.5

The one above has 1.00 in setting 95 and 45 in setting 96. 

So because setting 96 is 45 degrees it runs off at 45 degrees.

Setting 95 is 1.00 and the pitch is 2.5  (F2.5) so the length of run out is

1 x 2.5 = 2.5.

It still finishes at Z-25. by the way.

This means your run-out will be in one thread pitch.

If you’re concentrating  you will notice the tool jumps back in the X axis. It is going back to its start point (X22.).

G0 X25. Z3. G97 S1200 M3

G76 X16.93 Z-25. K1.534 D.485 F2.5

Notice above that by putting a bigger X figure (X25.) you get more clearance.

Just One More Before You Go

 

The above one has 3.00 in setting 95 and 10 degrees in setting 96

What If I Don’t Want All This Shit?

M23 means you will get a chamfer.

M24 means you won’t get the chamfer.

Please note M23 is active unless you program M24.

M23 is the default

So if you hit reset or switch the machine off it will always do the chamfer unless you program M24.

So if you don’t want it you need an M24 just before the G76 cycle.

Note: This works for G92 as well.

Here is what Haas have to say.

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

 

 


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

 

 


G76 Threading Start Point (Where Do you Start?)

Tags :

Category : Fanuc Turn

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 realized 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 backwards.

Correct

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.

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 program 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 Behavior

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 you can’t even achieve.

This will all depend on the age of your machine but you must always make this calculation just in case your 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 program CNC Milling Machines

Look no further Contact CNC Training Centre

 

 

 


Using G10 On A Fanuc CNC Lathe

Tags :

Category : Fanuc Turn Haas Turn

This article is about using G10 on a CNC Lathe to set the work shift or work zero offset as it is known on a Haas control.

If you have ever used Mazak machines you will know that when you call a program the work offset is kept with it.

Obvious really……

I mean if you were teaching your dog or your cat to program a CNC Lathe and you told him that he had to reset the workshift every time he called a new program what would he say.

I mean nothing really but he’d probably give you a strange look.

But you can do it on a Fanuc control or on a Haas control.

You just put this………………….

G10 P0 X0 Z-98.1

Using G10

So you would put that at the head of your program and it would change the work shift screen as above.

Advantages

No need to set workshift everytime.

Automatically sets X figures so there’s no chance you could alter it by accident.

 

Well there is a slight catch.

It’s obvious really but from now on you can only change the workshift from the program.

If you altered it on the workshift screen it would just change back when you run the program.

Now I know your not stupid enough to do that but I bet the bloke on nights is.

The Big One

When you restart a program you must remember to read this line.

Imagine if you tried to re-run the threading tool after altering the G10 you would just jump to that tool and run it. (Your new offset wouldn’t work)

Therefore you must remember to make the control read it in before running any tools.

Now the clever bastards will have a solution to this.

(This songs hilarious by the way)

What you could do is use a subprogram, the tool change position might be a good place to put it.

That way each tool would read it.

 

Oh yea and it’s probably a bit more tricky to alter as you can’t use input plusUsing G10

So you have to revert to mental arithmetic.

Ok So Why Do I Need All This Crap

Do you use the same chuck day in day out?

Do you keep the jaws for each job?

Well if the answer to these questions is yes, your workshift value is the same every time you set up this part.

Do you really want to reinvent the wheel?

 

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.

Or call us

If you want to learn to program CNC Milling Machines

Look no further Contact CNC Training Centre

 


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