Category : Fanuc Mill Fanuc Turn Haas Mill Haas Turn
O0001(G28 Example)
(PROGRAMMED BY ANDY MURRAY)
G21 G90 G40
T01 M06(20MM ENDMILL)
G90 G0 G54 X200. Y0 S1500 M3
G43 Z3. H1 M8
G81 G98 Z-5. R1. F100.
X100.
X50.
G0 X25. (No hole drilled here cycle would be cancelled)
G80 (This also cancels the cycle)
Category : Fanuc Turn Haas Turn Mazak Turn Siemens Turn
How to use G50 on a CNC lathe.
G50 in a turning program is a speed clamp. The machine accelerates up to the speed you set (G50 S2000) and will not go any faster.
Now before I get arrested by the “Correct Word and Grammar Police” I know it’s not actually a clamp. The truth is it’s just what everybody calls it, so get off my fuckin case.
Anyway if I start to call it something else all my CNC mates (and I do have some) will be confused.
Just check me out on LinkedIn. Anyway as I was saying my mates wouldn’t know what the fuck I was on about.
You must program a G50 before each tool and at the beginning of the program for safety reasons which I will explain later.
G50 is a modal G code (it stays active). If you have a program where you do not want to clamp the speed you must still put the G50 at the beginning of the program (set the clamp to the machines maximum RPM).
Otherwise it may pick up the G50 from the last program and you may not get the RPM you want. It can have the effect of slowing down production because the speed is being restricted and you didn’t realize.
Don’t use someone else’s G50 get your own.
You wouldn’t wear someone else’s dirty pants. (Americans call underpants underwear I think)
These are mine (sorry I din’t get time to wash them).
Modal G code explanation here.
Historically G50 was used to set the machine datum. This still works so do not put any X or Z figures on this line. You will get some weird shit happening if you do. Oh and you will probably trash your 100 grand machine.
G50 S2000 (SPEED CLAMP 2000 RPM)
Some G code systems, or depending on parameters, may use G92 instead of G50. This is not very common but it works exactly the same way.
On a Fanuc control they are called A type and B type G codes and depends on machine tool builder. Most of the G codes remain the same but proceed with caution.
It is particularly useful when you are facing a part using G96 (constant surface speed). When the tool reaches the centre of the part the machine will be running at maximum RPM. This could be very dangerous on large or out of balance components. When you set a G50 speed clamp, once the machine reaches the clamped speed it will go no further.
Here is a tutorial video about G96 and G97
RULES
This is a Toshiba VTL (Vertical Turning Lathe).
If you want to buy one or fix one go to Leader CNC
Now imagine this revolving too fast you would soon need their services oh and a good trauma team.
More CNC Turning Help (G70 and G71)
Please contact me if you require:
Classroom programmer training.
CNC Training on all controls and machines.
Mazak Training Fanuc Training
Don’t forget we offer training on all types of Mazak Machines and all Fanuc Controls 6m to 31i Oi old to young.
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………………….
So you would put that at the head of your program and it would change the work shift screen as above.
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.
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, if you had one for tool change position you could dump the G10 there.
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 plus
So you have to revert to mental arithmetic.
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?
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
Category : Fanuc Turn Mazak Turn
G74 Drilling Cycle with G96.
On a CNC lathe G96 is used for most machining. It was amazing in the old days when we suddenly discovered G96.
Because you are using a constant surface speed the metal cutting is consistent so you get a great finish.
CNC Programming was a bit of a black art back in the old days and generally speaking we used G96 for everything except for screw cutting and drilling holes on centreline (G74 Drilling Cycle).
When CNC Programming a drilled hole you would always use G97, (this means the speed is in RPM).
If you were to program for example G96 S50 M3 and then rapid to X0 and Z3. ready to drill a hole the machine would just go to its maximum RPM. This would be the speed you set in your G50. (The G code used to restrict the speed.)
Oh by the way that 50 meters per minute is for a B & Q drill.
Don’t get me wrong I love B & Q products but HSS drills are not for grown up engineers they are great for metal work classes at school and making a coffee table for the misses but it’s time to join the big boys and spend some money.
Anyway the machine would calculate the speed at its current diameter. So at zero the spindle would always be flat out.
So you could say G96 is pretty useless for a drill.
Take a look at this bit of code.
The idea is to send the machine to the drill diameter. Because the machine is in G96 it calculates the correct speed. When you then issue G97 it fixes the speed. Now when you move to X0 it has the correct speed.
Mmmmmmm… So all you need to do is send the drill to its diameter and the machine does the arithmetic.
Let the machine do what it’s good at and you do what you’re good at.
What are you good at by the way?
Threading is the same if you were machining an M20 thread at 100m/min calculate the surface speed.
(This is the quickest way I have seen)
20/314.2 =.06365
100/.06365 = 1571 RPM
You could do the same thing let the machine do it’s shit.
Rapid to the diameter of the thread then program G96
G0 X20. Z5.;
G96 S100 M3 (Start Spindle at 100 metres per min);
;
G97 (This will swap to RPM and clamp the speed at the correct RPM);
X21.;
;
G76 P010060 Q20 R.02;
G76 X16.93 Z-25. P1534 Q485 F2.5;
;
ETC
So with this bit of code you can get the machine to calculate your speed.
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
Category : Fanuc Turn Haas Turn Mazak Turn
G94 Facing Example
:Blank Size: 65mm Diameter 85mm Long
:Final Size: 65mm Diameter 82mm Long
This program will rapid to X66. Z3. it will then machine the face down to Z0 in three cuts. The first G94 line tells it to face past centreline to X-1.6 at a feed-rate of F.2 The Z axis moves to Z2.
Cuts
1: Z2.
2: Z1.
3: Z0
The cycle stays in the control until cancelled by a G0 rapid command.
So it remembers exactly what you told it, a bit like my wife, she keeps reminding me of the time I got so hammered I pissed in her wardrobe (some of the shoes still smell to this day).
The G0 G28 U0 W0 will move the turret back to machine reference point.
The G0 will cancel the G94 Facing cycle.
Well personally I think it is.
Now I’ll tell you why. You could say it’s really easy to write the program to face a part.
G0 X50. Z0
G1 X-1.6 F.2
G0 X50. Z2.
So that’s easy to do but….
Some one wrote a comment on one of my posts the other day and he started it by saying “back in the real world”.
Can’t lie and say it didn’t piss me off but being the mature well balanced man that I am I ignored it.
Now my inner nasty, immature, unbalanced me said “look mate I was in the real world when you were still shitting yellow”. Obviously I didn’t post it and if your reading this now thinking it’s you, well it isn’t.
In the “real world” you get to the end of the batch of parts and find that one of them is way too long and you need to face a shit load off the front.
Now had you used the cycle as below and got into the habit of always using it.
G0 X50. Z3.
G94 X-1.6 Z0 F.2
G0 G28 U0 W0
The alteration would be really easy.
G0 X50. Z12. (Imagine You Have An Extra 12mm On the Face)
G94 X-1.6 Z10.5 F.2
Z9.
Z7.5
Z6.
Z4.5
Z3.
Z1.5
Z0
G0 G28 U0 W0
Note don’t forget you must have the G0 rapid move at the end to cancel the G94.
(Just like G0 cancels a canned cycle in milling)
Don’t be tempted to put G0 in the moves as the control will just wiz around in Z and sit there laughing at you.
G0 X50. Z12. (This is what not to do)
G94 X-1.6 F.2
G0 Z10.5 (NO NO NO NO NO NO)
Z9.
Z7.5
Z6.
Z4.5
Z3.
Z1.5
Z0
G0 G28 U0 W0
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
