Category Archives: Fanuc

Taking a Screen Shot Fanuc Control

Category : Fanuc Useful Stuff

To take a Screen Shot Fanuc, you will need to have either a data card installed or a USB

Screen Shot Fanuc

MDI

In MDI I/O channel needs to be set (4) data card or (17) memory stick

Screen Shot Fanuc

Stick the Card in (or the stick)

Press and hold the shift key for about 10 seconds. You will see the clock stop. That’s how you know it worked. Time will stand still at this point and all the people around you will appear static.

Try not to panic, the world didn’t end. Your control just needs to ponder a while and think about what you just did.

Stop The Clock

Once it’s done your clock wil start again (phew).

Screen Shot Fanuc

Then press CARDScreen Shot Fanuc

Screen will show what is on the data card

Screen Shot Fanuc

The BMP files are your screen shots. You can then view them on your laptop or PC.

Now I know you are saying “what is the fuckin is the use of that”

Well It’s just so that I can show off my knowledge.

Screen Shot Fanuc

A good use is when you are changing parameters. There’s nothing worse than changing a parameter and trashing a £100,000 machine. Help is at hand, luckily you did a screen shot before you changed the parameter and you can view it and change it back.

Good luck with the massive dent in the guarding and the bent tool. No screen shot will fix that.

Screen capture Fanuc, thanks for reading.

 


Ten Things You Might Not Know About The Fanuc Sub Program

Sub Program Fanuc

Here are ten things you might not know about Fanuc sub programs,

Fanuc CNC controls are the most common controls in the world so it might be useful to have a good understanding of how sub programs are called and used.

(1) You Can Call a Sub Program By Name.

Yes you heard it here the program can be called by it’s name or it’s number. When calling by name don’t use the P.

Just put the name of the program in these things <> with an M98 and your away.

M98<ALBERT>

The only problem with this is that the syntax needs to be spot on so if you have got complicated names for your your sub routines then you might be in the shit.

I always call mine names like ALBERT that are easy to remember.

(2) You can use internal sub routines on a Fanuc Control.

Some people call these local sub programs. It just means it’s tagged on the end of your program which makes them nice n easy to look after. A bit like a pet Goldfish or a pet fly.

I bought mine from the local pet store. I asked the assistant if he sold pet flies and he said no. I said “well there are loads in the window”.

Anyway he sold me one (£15) his name is Paul

 

This is not him this is Steve.

Internal Sub-Routines

By typing M98 Q500 your control will look for N500 within your current program. This is great because you can add the sub programs to the end of your main program. Don’t forget to leave big gaps so you can clearly see where and what they are. Oh and mind your P’s and Q’s.

M98 P500 (Call O500 externally)

M98Q500 (Call N500 in main program.

Oh and read this too.

Sub Program

Just one other thing. Watch your n numbers it’s easy to get them mixed up. Try and use a convention.

This Is What I Do

N1-N99 (Tool change lines)
N26 M6 T26

N100 to N900 (Local Sub routines)

N1000 to N9999 (Anything else)

(3) You Can Jump Back To a Specific N Number

If you put a P at the end of your sub program next to the M99 after completing the sub program it will return to the main program at the corresponding N number.

M99 P800 will make it return to N800 in the main program it came from.

Sub Program

The above example calls sub program O500 when it gets to M99 it returns to the main program. The P800 means it will return at the line N800

Oh by the way I think this is useless but if you can think of a use please let me know.

(4) There Are Two Ways to Call a Sub Program

M98 P500 L4 (Call program O500 four times.

M98 P40500 (Call program O500 four times) watch out as the digits need to be the correct number.

The last four digits are the program number. The digits before them are the number of repetitions.

There must be four digits for the program number so you need the leading zeros (0500).

Sub Program

This method is a bit convoluted but at least I’ve included it and you never know when you might come across it.

I suggest always use the same method.

(5) M99 Has More Than One Use

M99 normally ends a sub-program but it can also be used in a main program to make it continuous. If you replace M30 (Stop and rewind) with M99 the program will constantly loop around. This is useful for multi pallet machines and barfed lathes.

Oh and don’t forget the EOB or you’ll get an alarm.

M99 ;

(6) You can use M99 to Jump over a Section of Code

M99 P100 will jump to N100

Impress your mates with this one it saves an awful lot of block skips

/
/
/
/
/
/

Sub Program

(7) You Can Call Sub-Programs From The MDI Screen

M98 P500 L6 (Call program O500 six Times)

This will work fine in MDI

(8) You Can Use a G or M Code to Call a Sub-Program

You can use a G Code alias to call a sub program. By setting certain parameters you can create your own G code which will then call a program specified by certain parameters.

Read this article

(9) You Can Have an Movement on the Line That Calls a Sub-Program

Although I have often shit my pants proving out programs, I mean an XY or Z movement not a a bowel movement.

X50. M98 P500 machine will move to X50. then call out the sub program.

(10) On your check screen it will show you how many times you have entered your sub program.

Each time you enter a sub program your control will show you a count down.

(11) You Can Call Sub Programs that are Not in Your Current Folder

When you call sub programs the control will look in your current folder. If it is in a different folder you can still call it.

<//from cnc memory/folder/folder/program>

Sub Program

The format for this is really important.

Also you will get a format error when you try and type it in. Easy fix….. go to CHANGE EDITOR

I have nearly 27,000 followers on LinkedIn and it has some real perks. One is that when I couldn’t get this to work. A quick post on LinkedIn got me some clues many thanks to Volker Hänig.

Shit, that’s 11 things.

Try to ignore one of them so there are only 10, maybe the one you already knew

 

 


Webster & Bennett with Fanuc 10T

On or Offsite CNC Training
Tel: David 07834 858 407

I Just Love Old Machines

I recently got to train someone on one of these, a Webster & Bennett with Fanuc 10t Control.

Webster & Bennett

It’s what I crudely call a big bastard. But bastard it is not, it can definitely machine some big shit

Webster & Bennett

Like this monster.

Don’t ask me what it is or I would have to kill you. Joking aside I think it’s a water valve. Beware these jacuzzis use a lot of water,

The machine is a Webster & Bennett vertical borer and I think the Fanuc 10t control was possibly a retro fit.

When these start whizzing around even a few RPM it can scare the living shit out of even the most seasoned engineer. And me, well I,m more seasoned than a piece of Nando’s chicken.

G50 on a Webster & Bennett Your Best Friend

Anyway joking aside your best buddy now is definitely G50 get this wrong and it’s fuckin world war three.

Imagine the scenario, you program G96 S180 M3. Spin at 180m/min. Not too fast but…. what if the tool is sat in the middle of the part.

Machine says “come on lads happy days foot to the floor flat out joy riding” and it fucks off like two teenage boys in a stolen Lamborghini.

So without a G50, or the wrong speed, this beast will accelerate to it’s maximum rpm.

Oh and did I Mention it’s harder to stop than a P & O Criuise Ship with 4000 obese pensioners on board?

E Stop….. Good Luck with That One

Hit the e stop and you’ll wait longer than you would for a GP appointment before it comes to rest.

Now not wishing to show off but I’ve been training people on CNC Machines for 30 plus years so I know exactly what to do in this situation.

Grab your immediate belongings and fuckin scarper.

So anyway make sure every program has a G50 at the head and then tattoo it on your scrotum sack. Whatever you need to remember to enter that vital G code.

Fanuc 10t The Old En’s Know Best

It makes you realise that Fanuc hasn’t really come that far with it’s controls (Sorry Mr Fanuc but some things have to be said)

It’s a 10T Fanuc on this Webster & Bennett, most of my readers were probably still shitting yellow when these 10t controls were around or maybe not even born. (What a crude expression that should stir up some complaints).

Webster & Bennett

G71 G72 Turning and Facing, Fanuc 10t

The G71 and G72 are single line. How bloody simple (whatever happened to simple).

Webster & Bennett

P100 first N number. Q110 second N number of the shape.

D1500 is a 1.5mm depth of cut.

U and W is finishing allowance.

F.35 is the feed-rate.

Piss easy.

G72 is much the same

Don’t forget with G72 you program it the other way. Just imagine you are going to machine it straight off as a finishing cut. Then rapid to where your metal starts before your G71 or G72.

Background Edit Fanuc 10t

Now We’re Really Living

This one’s even has background edit

Fanuc 10t

Here’s the button if you don’t believe me.

One of the biggest problems with these old controls is lack of memory I mean if this control was a person it wouldn’t even remember how to wipe its own arse.

But because its only two axis turning the programs are pretty small. They are a bit of a pain to backup but it can all be done with RS 232, a full moon and your laptop pointing to Mecca.

Setting Datums Webster & Bennett Borer

Setting the Z0 is quite easy. It’s even got G54 through to G59 (an extra in those days) honestly you don’t know you’re fuckin born these days with your extended offsets and your G54.1’s.

Workshif, Workshif I’m Happy With That

Anyway stick G54 up your arse cos I didn’t use it. I think on a two axis lathe the old work shift will suffice. None of your mamby pamby G54 shit.

Fanuc 10t

Easy to do. Position tool at required Z zero input Z0 then press MEASURE

Fanuc 10t

All done “good to go” as your favourite celebrity chef would say

Setting tools is going to be the good old cut and measure, just in case you are wondering what we used to do before tool measurement arms.

Fanuc 10t

Fairly standard stuff to measure tools.

Cut a diameter then move Z but not X (DO NOT PASS GO DO NOT COLLECT 200 POUNDS) to make a MONOPOLY analogy.

Type in the value X225.6 (if that’s what it measures) and the press measure.

Fanuc 10t

 

Job done, who needs a fuckin sissy boy measurement arm?

You can reset your relative display just like on a newer machine. It’s even got MDI, a bit crude in that you have to enter each character separately but this machine is a buddle of joy.

To think people pay me for this job, admittedly lower than the minimum wage but I get to work on these beautiful pieces of machinery.

If I win the lottery tomorrow I will buy one of these, a cake shop, a chip shop and a pub.

Oh and if there is any cash left I’ll buy the misses a new coat from Marks & Spencer.

 


Fanuc Subprogram (Local Subroutine)

Category : Fanuc

On or Offsite CNC Training
Tel: David 07834 858 407

Fanuc Subprogram (Local Subroutine)

If you have ever used local subroutines on Heidenhain or Yasnac. Then you will know how convenient it is to save all your programs in one go. No need to remember to save all those shitty little external sub programs.

What’s He On About?

If you are now saying “what the fuck is he on about”. Here is an explanation.

A local subroutine or subprogram is where you stuff all your subprograms at the end of your main program.

So on a Fanuc control if you were making this part below.

Drill spot drill then tap.

Fanuc Subprogram

Programme would look like this.

Fanuc Subprogram

 

Thing is the code is just repeated three times. I have nice round numbers in here like X40. and Y20. so it’s easy to notice mistakes. But if it was X40.392 for example you wouldn’t spot a slight mistake.

So if you call a subprogram it looks like this.

Fanuc Subprogram

And then your Subprogram is like this.

Fanuc Subprogram

Fanuc Subprogram

The M98 P500 calls the external Fanuc Subprogram. Read this if you don’t know about sub programmes.

Saves you having to repeatedly write shit loads of code.

So that’s why we use a Fanuc Subprogram. But……

You have to look after these bloody things and they seem to be able to just get lost on their own.

You find them at the back of the fridge sometimes along with a piece of mouldy old cheese. At least you can make a meal of the cheese.

Fanuc Subprogram No More Lost Programs

So this is how it looks with a Local Subroutine.

All you need to do is replace P with Q. So mind your P’s and Q’s as they say.

The Q corresponds to any N number. So you could have loads of these stacked up at the end of your programme and you only need to save it once. All this shit will go with it and you don’t need to worry about it ever again.

Haas To The Rescue

Of course Mr Haas sorted this out years ago with M97, this calls a local sub. M98 calls an external program. It’s on all Haas machines and you definitely do need to fuck with any parameters.

Just A word Of Caution.

There are PARAMETERS involved. Arrrrrrrrrrrh……..the dreaded PARAMETERS

To call a subroutine on your Fanuc control. You first need to make sure that Bit 0 of parameter 06005 is set to 1

Fanuc Subprogram

This should make it work. If it doesn’t then maybe you should call the Samaritans.

It’s only on the newer controls by the way.

Sub programs on a Siemens control.

Thanks For Reading My Articles We Love you all .

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

 

 

 

 


CNC Programming Examples Turn and Mill

Category : Fanuc

Click CNC Programming Examples

These are the different CNC programming examples we have both turning and milling.

CNC Programming Examples

CNC Programming Examples Turning

G94 Facing

Milling

G81 Drilling Cycle

G73 Peck Drilling Cycle

G83 Deep Hole Peck Drilling Cycle

G82 Drill With Dwell Cycle

G84 Rigid Tapping

Examples from Haas


WP to LinkedIn Auto Publish Powered By : XYZScripts.com