Using Macro System Variables

Macro System Variables, I often get random emails from people asking me all sorts of questions.

I got one only the other day it began “Hi David, your articles are shit”

I don’t answer every email I get, but I try to answer when I think there is an appropriate response or I feel I can help.

Macro System Variables

Anyway someone called Neil from America (I think) asked me if I would create a tool setting macro. This involves using Macro System Variables

There is a really annoying thing on a Fanuc control (well actually there are quite a few). This one really pisses me off because I find myself making excuses for the control. I mean like I designed the fuckin thing.

For one, I am nowhere near clever enough and don’t even work for Fanuc. (I am available Mr. Fanuc, sorry I dissed your control)

To set a tool length it’s a really convoluted procedure. You first zero out the Z on the REL display.

You then bring down a tool and get the control to record the Z position by pressing Z then the soft key INP C.

Here’s a couple of videos showing you how.

Origin Z

Use INP C to Enter Offset

Once the Z has been set you can measure as many tools as you want. Just bring each tool down to the setting block and press Z then  INP C.

Here comes the problem…..

If you turn turn off the machine or, for some reason, you have to reference it again you will lose your REL Z position. You will now have to set it again.

Oh and if you don’t notice you’ll be in deep shit. (Your tool length will be wrong!!!)

There are ways around this by using a work offset, but to be honest it’s all a pain in the fuckin arse.

Oh and one other thing. Make sure you write the offset to the correct tool because you can write it to any tool.

Warning

Check the Z zero position each time before setting tools.

A good guide is to slap a good old steel rule or a tape measure against the tool for a rough check.

Macro System Variables to the Rescue

For years I have used a work around on Fanuc Controls. First of all you need to establish where your setting block is. In my case it’s a table probe.

Oh and you need macro (it is an option so if you don’t have it look away now.

To do this you need to note down your machine position in Z when you touch your block or setting probe.

This will later be stored in a variable to be used to calculate the tool length.

Try to set your block in a known position so that each time the Z figure is the same. You may even be able to fix it to the machines table. Don’t weld it, the boss won’t like it.

Read on to see how this variable can be written to automatically with a calibration programme.

The Programme…  OK Let’s Do This

1. Bring the spindle nose down to touch your setting block. this is the value you will write into #102 (Mine says -500.877)
2. Call your tool to be measured into the spindle in MDI (T06 M06;)
3. Bring the tool down to the setting probe.
4. Run the programme below.

O9001(Tool Measurement Macro)
1.  #100=#4120 (Grab Tool Number);
This will cause the machine to store the current tool number in #100

2. #101=#5023 (Store Machine Z Position);
This will cause the machine to store the current Z position in #101 

3. #102=-500.877 (Setting Block Z);
This is the figure you recorded from the position of the setting block.

4. #150=#102-#101 (Calculate Tool Length);
Now we can calculate the tool length by taking the known position from the current position.

This will give us a minus figure, we will reverse this in the code below.

5. #150=-#150 (Reverse Z Figure);

6. G90 G10 L10 P#100 R#150
This puts the tool length into the correct offset.

7. G28 G91 Z0 (Return Z To Zero Return);
8. G90;
M30;

More Explanation (Macro System Variables)

System variables know shit.

What I mean by this is that system variables contain information about the system. Some are read only and some you can write to, like the tool offsets for instance.

You can ask the system loads of stuff like.

• What speed do you have stored?
• What’s the tool in the spindle?
• What position are you in?
• What modal G codes do you have.
• How old is my auntie Joan?
• Do I have a fat arse?

These are all stored in special Macro System Variables except the last two.

You can read them and sometimes you can write to them. It’s not like that bloke at work who thinks he knows every fuckin thing. Sometimes he’ll listen, but most of the time he has to tell you.

No, no macro system variables follow special rules.

Anyway (The Explanation)

O9001(Tool Measurement Macro)

1.  #100=#4120 (Grab Tool Number);

2. #101=#5023 (Store Machine Z Position);

3. #102=-500.877 (Setting Block Z);

4. #150=#102-#101 (Calculate Tool Length);

5. #150=-#150 (Reverse Z Figure);

6. G90 G10 L10 P#100 R#150

7. G28 G91 Z0 (Return Z To Zero Return);
8. G90;
M99;

The first line 1. looks into system variable #4120 which contains the number of the current tool in the spindle.

You ask what this is and then put it in #100. Obviously you can’t write to this variable.

The next line 2. asks where the machine is in Z (Machine Position) #5023. Again you can’t write to this but you can store it in #101.

Line 3. stores the value that you measured early in #102. This is where your measuring block is from zero return.

In line 4. you take these values away from one another to give you the tool length

This ends up as a minus figure so we need to reverse it. We do this on line 5.

5. #150=-#150 (Reverse Z Figure);

6. G90 G10 L10 P#100 R#150

Line 6. is a standard G10 because we have L10 this means it writes to tool lengths. P is the tool number and R is the tool length.

I always stick a G90 at the front of this G10 in case some twat  leaves the machine in G91 in which case it will add to the existing tool length. (Oh dear total fuckin dog shit mayhem)

So You Want To Use Macro Like An Adult?

Lots of programmers use macro in a very complex and confusing way but I think that is the way they want it so you think “wow he must be a clever bastard.

In my opinion a good macro should have a really simple interface.

I’ll show you mine.

M200

Yep that’s all it is

M200 is aliased to my programme O9001 meaning if you run M200 it goes into my programme 9001 and returns.

Don’t forget you can run M200 in MDI too.

Read this article if you don’t know how to alias a macro to an M code or a G code.

More Macro System Variables

Now what we could also do is when we bring the spindle nose down to set the original Z figure, we could make the machine store this in #500 instead of my #102

500 series variables stay in the control even when it’s switched off. These variables are the cockroaches of macro programming (they survive anything).

In the event of a nuclear war the survivors would be as follows:

• 500 system variables
• Some cockroaches.
• Ozzy Osbourne.
• Keith Richards.
• My mother in law.

The code for this is really simple. Just one line in fact,

All you need do is bring your spindle down to the setting block. Then run M300, which I have aliased to programme 9002

Or if you like just run programme 9002

O9002 (Calibrate Table Block);
#500=#5023 (Z Machine Position);
M30;

Word Of Caution

Don’t use M99 at the end of your Macro unless you are calling it with an M Code Alias. Otherwise it will be stuck in a never ending loop.

So Now It’s Simple

Bring the spindle down to setting block and run M300.

This sets #500. If the block is in the same place then this is not needed.

Call the tool you want to measure to the spindle in MDI otherwise it won’t be registered in #4120

T20 M06;

Bring the tool down to the block and run M200.

Or simply type M200 into MDI and run it.

This will then store the tool length in the correct offset.

Please contact me if you require:

• Fanuc training.
• CNC programmer training.
• Want to Learn CNC programming.
• Fanuc programming   training.
• Any type of CNC course.

Don’t forget to watch my Tutorial Videos

Services offered at CNC Training Centre

Edgecam training.

Classroom programmer training.

Onsite CNC Machine 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.

[contact-form-7 id=”2706″ title=”Contact Form”]

Macro For Over 18 (Using Alias In a Macro)

Macro programming can use a G code to access a 9000 series program.

Read this article if you don’t know about this.

In this example macro we are going to set G181 to access program 9010.

We will create a new drilling cycle that can take into account the point of the drill in the drill depth.

The line below would call program 9010 from the G181

G181 A120. D16. R1. Z-20. F200.

It works the same as a G81 but with a drill point angle (A) and a drill diameter (D). It then goes on to use some simple trigonometry to calculate the drill point.

Believe me it has to be simple for me because as my mate used to say, “if brains were made of dynamite I would struggle to blow my your fuckin head off”

It feeds down to the Z depth then incrementally drills the extra bit for the drill point. Then it rapids back out.

G181 A120. D16. R1. Z-20. F200.

A (#1) = 120.
D (#7) = 16.
R (#18) = 1.
Z (#26) = -20.
F (#9) =200.

Remember the table below from the last article.

O09010 (Drill Point Macro)

G103 P1           (No Look Ahead)

(Letter A #1 = Drill Point Angle)
(Letter D #7 = Drill Diameter)
(Letter R #18 = Rapid Point)
(Letter Z #26 = Depth)
(Letter F #9 = Feedrate)

G00 Z#18           (Rapid To R Point)

G01 Z#26 F#9       (Feed to Z depth)

#100= #1 / 2                  (1/2 Drill Angle)
#100= TAN[ #100 ]     (Tan Of Half Drill Angle)

#101= #7 / 2                   (1/2 Drill Diameter)
#102= #101 / #100      (Calculate Extra Depth)

G91 Z – #102            (Extra Bit)
G90
G00 Z#18          (Rapid Back To R Point)

G103 P0           (Look Ahead On)
M99

Let me explain this macro line by line

O09010 (Drill Point Macro)

G103 P1 (No Look Ahead)

The G103 is so that the macro does not read in front and get confused, it will now only read block by block. A bit like knowing the end of a book, you wouldn’t be arsed to read the rest of it.

The control normally reads in front so it has some idea what is going to happen next.

Always include an explanation with your macro in case you forget how it works. You wrote this thing so you can’t blame the bloke on nights.

(A #1 = Drill Point Angle)
(D #7 = Drill Diameter)
(R #18 = Rapid Point)
(Z #26 = Depth)
(F #9 = Feedrate)

G00 Z#18 (Rapid To R Point)

G01 Z#26 F#9 (Feed to depth at 200mm per minute)

The calculation below halves the drill angle. You will note that the drill angle is letter A which corresponds to #1

#100= #1 / 2     (1/2 Drill Angle)

Below will get  the tangent of the angle and this ends up back in #100 
#100= TAN[ #100 ]       (Tan Of Half Drill Angle)

Calculation below halves the drill diameter and puts it in #101

#101= #7 / 2       (1/2 Drill Diameter)

Macro, The Trigonometry

This is simple trigonometry and the answer is the depth of the drill point (Y).

In the diagram above
X is #101    (Radius of drill)
A is #100    (1/2 drill point angle)
Y is #102    (the bit we need to know)

#102= #101 / #100        (Calculate Extra Depth)

G91 Z – #102        (Feed down the extra amount calculated above incrementally)
G90                      (Back to absolute)
G00 Z#18           (Rapid Back To R Point)

G103 P0         (Look Ahead Back On)
M99

Carry on If You Are Over 18

Earlier in the post I mention the “Grown Up World Of Macro”. That is because I often meet programmers who learn macro and use it just because they can. Oh and to confuse the shit out of the machine operators and other programmers.

You learnt a bit of macro.

So fuckin what no one is impressed.

You can actually do more harm than good. As I have said in these posts before no one gives a flying fuck if you mess up the machine. Well apart from your boss (you know that bloke with the fat arse, little cock, and a Porch 911).

Seriously (and I rarely am) if you want to write macros here’s what you need to do.

1. Do you really need one or is it just your huge ego and you need to get a life?
2. Maybe you need to get out more?
3. Will it confuse the operator?
4. Can anyone use it?
5. Is it simple for the user?
6. Is it fool proof?

Let’s Look At My G181

Do you really need one or is it just your huge ego?
I think it could be quite useful to be able to allow for the drill point.

Maybe you need to get out more?
Definitely.

Will it confuse the operator?
No it’s very similar to a G81

Can anyone use it?
Yes

Is it simple for the user?
Yes my mum loves it and she’s 96.

Is it fool proof?
No definitely not we need to talk about this

Fool Proof

What if you missed out the Z value?

What if you had a minus value in R and a plus value in Z?

Would it still try and work if you input ridiculous figures?

Any of the above would completely screw it up. You could say “I’ll tell the operator to make sure he follows my rules”.

OK so if you just bought a new television and you accidentally pressed 12356 as a channel number.

What if the television just went off, or the screen locked up or it exploded and burnt down your house.

You would complain wouldn’t you. Us Brits can ignore this because we never complain. We’d probably ring up and thank them for the opportunity to build a new house.

Anyway we all know that the telly wouldn’t do that. It would either ignore you and treat you like the dipstick that you are. Or it would just go to channel 999 which is it’s highest channel.

Now this is not because Mr Sony is inside your telly thinking what to do if you make a mistake like shoving the remote control up your arse.

Your television has logic. This means in every scenario it knows what to do. It’s like the Bear Grylls of televisions.

So Let’s Look At Improving This

In a macro you can use a conditional statement. It’s like my wife said to me you either change your underpants every week or you piss off back to your mothers.

It gives choices.

Let’s Add This Line

IF [ #18 LT 0.0 ] GOTO999

What this means is that if #18, which is the R value, is less than 0 the control will jump to N999.

This means if you put a minus figure in R it would be less than zero and trigger the jump to N999.

N999 #3000= 1 (R LESS THAN ZERO PRICK!!)

#3000 puts the machine into an alarm state. The comment in brackets will be the alarm message and it looks like this.

This is how the programme looks now.

%
O09010 (Drill Point Macro)

G103 P1 (No Look Ahead)

IF [ #18 LT 0.0 ] GOTO999

(Letter A #1 = Drill Point Angle)
(Letter D #7 = Drill Diameter)
(Letter R #18 = Rapid Point)
(Letter Z #26 = Depth)
(Letter F #9 = Feedrate)

G00 Z#18 (Rapid To R Point)

G01 Z#26 F#9

#100= #1 / 2 (1/2 Drill Angle)
#100= TAN[ #100 ] (Tan Of Half Drill Angle)

#101= #7 / 2 (1/2 Drill Diameter)
#102= #101 / #100 (Calculate Extra Depth)

G91 Z – #102 (Extra Bit)
G90
G00 Z#18 (Rapid Back To R Point)

N999 #3000= 1 (R LESS THAN ZERO PRICK!!)

G103 P0 (Look Ahead On)
M99
%

Now it doesn’t take much imagination to see that you could completely fool proof this macro.

Oh and you can have loads of fun with the childish comments and sexual innuendo.

Variable Zero

#0 is a unique variable because it means no value.

IF [ #18 EQ #0 ] GOTO998

If you put a statement like the one above it means if #18 is vacant (meaning it has no value).

Then the programme will jump to N998.

N998 #3000= 2 (SORRY MY FRIEND, R HAS NO VALUE)

This is a much politer alarm and it saves a kick in the bollocks from the machine programmer when he gets offended by your childish alarm comments.

Don’t confuse zero with no value. Zero is a value. Ask your clever mate.

Default Values In Your Macro

So now for the “no value” scenario. You could make your  programme jump to a line that gives a default value.

IF [ #18 EQ #0 ] GOTO123
GOTO124
N123 #18=1.
N124 

Take a moment to study the above code.

Come on get a grip do you understand it?

Now I’m from the old school of education. When I was a boy if you didn’t know the answer to the teacher’s question it was simple.

They beat the fuckin shit out of you.

And if you discount completely fucking up the planet and starting a lot of pointless wars, my generation have done a pretty good job thus far.

Anyway today I’m going to be patient.

Let me explain…..

If you  are offended by any of the above please go to this website(this bloke writes much better stuff than me)

IF [ #18 EQ #0 ] GOTO123
GOTO124
N123 #18=1.
N124 

It’s very easy really, the first line will jump to N123 and set #18 to 1 if #18 has no value.

If however, there is a value in #18, then the control ignores the GOTO123 and reads the next line which jumps to N124 and carries on as if nothing ever happened.

Belt and Braces Things You Can Do

Check all of the following, what happens if…………

• Values to high
• Values to low.
• No value entered
• Letter missed out

You can set alarms or default values if your conditions are not met.

It’s a bit like blackmail except for the bit where they have to leave a shit load of money in a phone box for you to pick up.

Things to Think About

Think of every dumb ass thing that your user could do with your macro.

Then make your macro respond in a adult way. So if he inputs daft information the macro sorts it out. It can use defaults or go into an alarm state with a message.

Keep the macro front end really simple, this is the bit the user sees and uses. For example my macro needs the radius of the drill for it’s calculation. You will note I ask the user to input the diameter.

Why?

Because it’s simple and easy for him and that’s what he will know. I can do all the work behind the scenes hidden away in my 9000 series programme.

The front end.

G181 A120. D16. R1. Z-20. F200.

This bit is all he needs to worry about I take care of everything else. It’s like an all inclusive holiday. All you needs to do is eat sleep and constantly get pissed on cheap booze.

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 programme CNC Milling Machines

Look no further Contact CNC Training Centre

G Code Alias M Code Alias (How to use them)

G Code Alias. What is an alias Wikipedia?

Alias, it’s not just about James Bond

Alias, in the case of CNC Programming means you are using a G code or an M code to call a program.

For example you could set up G181 to call program O9010

G181 would be an alias for program O9010

These are special 9000 series programs and you set them in your parameters.

M Code Alias Fanuc Parameter 6080

G Code Alias Fanuc Parameter 6050

If you have a Haas machine it’s parameter 81 to 90 for M code alias.

It’s parameter 91 to 100 for G code alias.

So if you look above at parameter 91.

Then enter 181.

When you write G181 in a program or in MDI.

The control would go into program O9010

Therefore you can use a G code to access O9010 through to O9019. You can’t use any G code it has to be one that is not used.

It’s important to check that these 9000 programs are not used by things such as probing cycles. So be sure to check before altering.

The same thing applies with M codes (Programs 9000 to 9009).

You may be asking why you would want to do this. Well it means that you can fully automate your Macro.

You first of all place your macro code in one of these program numbers then when you want to use it you just use the G or M code you allocated to the program.

G Code Alias, M Code Alias, It Gets Way Better

Imagine you set 100 in parameter 81, when you issue an M100 the control will jump into program O9000

This is very simple but you can see how exciting it can get. I didn’t sleep for a week when I first discovered this. Just make up your own M code to do any old shit you want.

In your parameters you can alter a setting so that 9000 programs can’t be viewed or edited. So no one gets to tinker with your precious code. Below is Haas but you can do it on any control.

Welcome to the grown up world of macro because now you can make an M code that an operator can freely use but never access or alter. So to him it’s just a regular M code.

Oh don’t forget to tell him what it does otherwise he’ll never be arsed to use it.

You may well ask why can you do this with M codes and G codes. Well with M codes that’s really all you can do.

Let me explain….

With a G Code Alias………

You can add parameters. You know like when you use a G81 drilling cycle.

G81 calls a program that drills holes. You control the depth and feed etc with parameters.

Once you call a G81 it knows all about drilling holes. Like when it gets to the bottom it has to get the hell out of there.

G81 Z-20. R1. F100

• G81 calls the cycle
• Z-20. is the depth
• R1. is the point to rapid to
• F100. is the feedrate

The Z the R and the F are the parameters that pass into the program.

With an M Code Alias………

None of the above. It’s just an M code. Very useful I must say but you can’t pass parameters to it.

Toolchange (Fanuc Controls)

Ever worked on a machine where you have to write extra code to stop the spindle and take the tool up to zero before you can tool change?

Well that’s what M6 does, just tool change.

What most machines do is use an alias for M6.

So it’s not really M6?

Nope…..

M6 uses an alias. So in your parameters you make M6 access a 9000 program. That way you can put any old bollocks in the 9000 program.

When you subsequently use M6 it goes into this program which contains everything you could ever want for a tool-change.

• Stop spindle
• Turn off coolant
• Return Z to zero
• Feed the dog
• Change the tool

And all with just an M6.

If you have one of these old machines you could make your own alias.

G Code Alias Passing Parameters?

This is where it gets clever and it gets complicated.

But……

You have me to hold your hand.

OK so you set G181 to access program O9010.

G181 A50. C20. Z-10.

This G181 would pass the values of A, C and Z through to program 9010

9010 would then use the values to do it’s business.

Mmmmm how does that work?

These guys below are know as the macro variable gnomes and each one has his own letter and his own macro variable.

If you think I’m joking then go into your programming department and ask them. Say you want to learn about the macro variable gnomes.

It took me ages to do those stupid fuckin gnomes. Then I realized it wasn’t even funny but I couldn’t bear to get rid of them.

Below is a table that shows the corresponding variable for each letter. Forget the fuckin gnomes, it’s just a failed experiment. Let it go.

What this means is that if you put a value in A it will register in #1 and if you put a value in Z it will register in #26.

Then in your 9000 series programme it can use those values. It’s like a secret way to get information into your macro programme.

First of all put 181 in parameter 91.

This means that G181 would call programme O9010.

Lets create a drilling programme the same s G81  we will call it G181.

It’s no different to G81 but it will demonstrate the use of Alias.

In other words it’s completely fuckin useless but at least I’ll get my point across. Oh yes, and stop picking fault with every bloody thing I do

G181 Z-20. R1. F200.

The G181 above will call O9010 and pass the values for Z, R and F into it.

#26 (Z)
#18 (R)
#9  (F)

Remember The List

This is how O9010 Looks

O9010 (My Drilling Cycle)
G0 Z#18 
G1 Z#26 F#9
G0 Z#18
M99

Explanation

G181 Z-20. R1. F200.

O9010 (My Drilling Cycle Linked to G181)
G0 Z#18
#18 is the value passed from the letter R
R had a value of 1 so #18 is assigned the value 1
The machine will rapid to Z1.

G1 Z#26 F#9
#26 is the value passed from Z
Z had a value of -20. therefore #26 is assigned the value -20
Machine will feed to Z-20.
#9 is the value passed from the letter F
F had a value of 200 so #9 is assigned the value of 200
Machine will use a feed-rate of 200 mm per minute.

G0 Z#18 
#18 is the value passed from the letter R.
R had a value of 1 so #18 is assigned the value 1
Machine will rapid back to Z1.

M99

Don’t you just love all this shit?

This is Only the Tip of The Iceberg

See this post for grown up Macro programming

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 programme CNC Milling Machines

Look no further Contact CNC Training Centre