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”]