Problem- Macro Executor

[eswar.enp]

hi,
I want make a macro screen in which the user should able to change the G54 values(work offset).

kindly help me in this regard.

thanking you,
Eswar.

[James L]

Are you looking for a screen that prompts users to enter values? How will the positions be recorded initially by the operator? Could use a little clarification on this.

[eswar.enp]

No, I am developing the program.
My requirement is through that screen i should be able to change work offset values.
I have compiled the a sampl macro program and loaded , it is working fine. But i am not having any idea how to input value through macro screen.

thnks
Eswar

[stevo1]

Eswar,
First off what model Fanuc control are you using? If you just want them to change the G54 you can go to the offset page that displays the G54-G59 settings and you can have them change them there. That is the only screen that I know of that you can change the values of G54.

If you wanted a program to change them say a main start program then you could have them programmed as follows.

O0001(main start program)
#5221=10(G54 X VALUE)
#5222=15(G54 Y VALUE)
#5223=7(G54 Z VALUE)
…
…
M98 or G65 Pxxxx

On a side note to G54 this is usually the machines default work coordinate so any values in here will be taken into account for any moves after the machine program has ended or reset has been pressed. IOW when all tool offsets and modal codes have been canceled your G54 is still active with the current values your operators had set. I usually have the guys use G55-G59.

Stevo

[James L]

I can't think of any ways of getting a macro to prompt for input right off. If, however you wanted an operator to be able to load a piece of work and read the edges with and edge finder you could use a macro call similar to what steveo listed at the start of a main program. I'm still not 100% on the application of this.

[stevo1]

The best way to have a program prompt the operator for input would be to have a M0(program stop) or a operator message using #3006 variable. Once the program is stopped you could have a note to have them set X,Y,Z location to variables and then have the variables read to G54. Ex below.

O9000(macro xxx)
…
…
M0
(set #100=G54 X position)
(set #101=G54 Y position)
(set #102=G54 Z position)
…
#5221=#100
#5222=#101
#5223=#102
…

Inplace of the M0 if using the #3006 to display a message would be as follows. #3006=1(set #100,#101,#102=X,Y,Z). Whatever is written in between the () would be displayed as the message. The limit to this is a message can only usually display a max of 26 characters.

Stevo

[James L]

I can see using a message to operator. I was unsure if, after doing this, input could be read by the program without having to restart the macro with different variables. If it is possible to add this level of interaction with the macro then I can think of a whole range of possibilities with this. All programs I run are on Haas machines.

[stevo1]

James,
I am unsure of the exact capabilities of a Haas. I mainly use Fanuc and I know that Fanuc and Haas run pretty close to the same. I have been slowly picking up on the Haas functions through various threads and I have been seeing a lot of very useful functions that I wish Fanuc had.

Operator messages function like the M0 or M1 function except the #3006 displays the message. The program will stop on that line of code. Once the cycle start button is pushed it will continue with the next block. Now with the Fanucs you will be on the operator message screen and you will have to navigate back to the program screen. You can try this quite easily by programming the #3006=1(message) and once the message is displayed go back to your program screen and the #3006 block should be highlighted and paused as if it were a M0. Now just push cycle start.

I use both ways but if you have to display a larger man readable then the M0 is the only option because of the limited charters with the #3006.

Originally Posted by James L If it is possible to add this level of interaction with the macro then I can think of a whole range of possibilities with this.

When it comes to macros and things like this the limitations are almost endless. I am still trying to figure out some of the functions from my predecessors. He had about 40 different macro programs working together using about 20 different tools and the parts had a combination of about 60 different processes. To top it all off there were about 500 different part configurations. All you had to do was look at the matrix sheet and pick were you wanted to start anywere in the 60 different processes and type the code of 13596746. Each group of 2 numbers would dictate were the program should lead. Then again if I had written my college thesis on machine tool programming like he did then I would probably understand.

Stevo

[James L]

I'll have to play around with that a bit. As far as differences between Haas and Fanuc machines running macro, there are pros and cons both ways. Fanuc has a number of options available in its macros that is not supported by the Haas machines I am using.. specifically the modal macro calls.

[stevo1]

So Haas doesn’t support the macro modal call like the Fanucs G66? I don’t usually use the modal call because most of the holes are that we drill are equally spaced or can be calculated in the macro. However there are a few times that we get holes at all various locations throughout a part and the modal call is the cats a$$ when it comes to that.

Stevo

[John_B]

Stevo,
It must vary by MTB which coordinate a machine defaults to at the end of a cycle. Both my machines with 0m-C controls default to "G53". My machine with a 10m control I think stays at G54 as you mentioned.

It sound like Eswar is looking for a macro similar to those I use. I have a series of 8000 programs I leave in the control that start at 8054, 8055, and so on that reads the current position register and changes the appropriate G54, G55, and so on to that position. This way I just do my edge-finding, use the relative position field and zero the first axis I do, then find the second axis - and when I've found both I return both to the zero position in the relative field and run the macro for the workshift I'm going to use in the program.

I also have one stored as 8000 that I use to record the tool length offset when I touch off, it reads the current Z position, the current tool #, then enters the position in the appropriate tool offset register.

These have saved me a good bit of time over the last few years. I'm not where I can get to these macro programs just now, but I can post them later if needed. They're not too sophisticated though, this is pretty basic programming.

Best regards,
John B

[dcoupar]

I believe Eswar is looking to build a "custom screen" such as several manufacturers have done (YCI and Doosan I know of have them). Hence "Macro Executor" in the subject line. I've seen reference to "Embedded Macros", but I don't even know where to point him for how to get started. It seems to me that there's quite a bit of $ required for software, compilers, etc.