Fanuc "Not 0" Control on VMC's?

[Ox]

IDK what to make of this, but you are right!
It was 3.69, but ...

Good eye!

And I am sure that I had to of done it myself, not realizing that I was in WEAR at the time.
I mean - what's the odds that someone else had a tool with almost the same offset in just that pocket before we got the machine?

I know that I have dealt with this a few times now on set-ups, and I wouldn't have thought that I would have always been setting it up with T24, but I am now second guessing...
Typically I would touch off with a drill or C-drill, or something like that.

There were a few .005 - .015 values in WEAR as well, but not in pockets that I have used yet.
This mill has twin 20 tool changers, and I haven't used it much yet, so lots of open pockets in there yet!

Well, I am sure that this will clear up one issue...

Now I need to git a thumb drive reader hooked up to it...

(none of my 0 controls have a wear page for offsets, only length; we use offsets 61+ for cutter comp offsets)

Yeah, this thing has offsets to 400!


-------------------------

Think Snow Eh!
Ox

 

[Ox]

Historically I have hardly ever used the WEAR pages, but maybe I can blame this on the Swiss lathes that I have been running as of late. While at least those have 18 controls, they doo NOT use the Geometry pages, and all tool offsets are in the WEAR pages. OK, well maybe not "all" offsets, but the ones that we use most of the time anyhow.

So, maybe I can blame that oops on that?


----------------------

Think Snow Eh!
Ox

 

[dandrummerman21]

Another parameter you might want to change is parameter 18 bit 5 to a 1. This will make the control consider the tool length on the absolute coordinate display.

That way, if you're at z-.080" in your program, it should show up as z-.080 (instead of z3.123), and you wouldn't need to zero the relative display to achieve it.

There are similar parameters for what is displayed when using cutter comp g41/42. It can either display the actual location with cutter comp, or lie to you and display what's programmed.

 

[Ox]

That is already a 1.
It displays propper when in cycle (as in the pic)

It's that I would expect it to always display with the tool length in mind, as long as there is a tool in there.
My point is that when touching off during set-up, the CRT does not consider what tool you are touching off with.

Now, at least this is not a crash scenario! If you forget to go look up the TL when setting Z0, then it will just be cutting air in cycle, so there is at least that ....


-------------------

Think Snow Eh!
Ox

 

[dandrummerman21]

I thought that in the sideways pic (pic 5) on the previous forum page, the absolute coordinates display as z7.whatever instead of z-.080


I never trust relative displays. Things may get screwy with relative display when you're changing between work offsets and tools.


Parameter 394 bit 6 controls whether or not the machine resets back to g54 when you hit reset. If you're using g57 and hit reset, you can make it still keep g57 active.




I should make a list of parameters that I need to change when we get a new (used) machine. A new (2003!) robodrill with apc just hit my floor on the weekend, and I've yet to go through it to get it to behave like the rest of the machines.

 

[Ox]

You know, that came up earlier... (last Fix Offset)

In this case, I'm on the fence over worrying about it keeping G57 in this case.
The job I had in it a cpl months ago - I was using 4 Fix Offsets, so it keeping the last one - doesn't mean much.


BUT! I just had a thought...

The control defaults to G54, but if I change this param, and I finish my program [like normal] as:

G53 X15. Y0

I wonder if it would hold the G53 (base) coordinates?
THAT's what I was wanting in the first place!

I will go try that!


------------------

Think Snow Eh!
Ox

 

[Ox]

I thought that in the sideways pic (pic 5) on the previous forum page, the absolute coordinates display as z7.whatever instead of z-.080


I never trust relative displays. Things may get screwy with relative display when you're changing between work offsets and tools.


Parameter 394 bit 6 controls whether or not the machine resets back to g54 when you hit reset. If you're using g57 and hit reset, you can make it still keep g57 active.




I should make a list of parameters that I need to change when we get a new (used) machine. A new (2003!) robodrill with apc just hit my floor on the weekend, and I've yet to go through it to get it to behave like the rest of the machines.

That didn't seem to change anything.

"B6" = second from left - correct? Same page?


----------------

Think Snow Eh!
Ox

 

[dandrummerman21]

That didn't seem to change anything.

"B6" = second from left - correct? Same page?


----------------

Think Snow Eh!
Ox

You mean you made it a zero? 1 makes it reset. Yes, 2nd bit from left (x0xxxxxx)

Here's the manuals for it (assume you've got them in pdf but maybe not?) http://cncmanual.com/fanuc/fanuc-0-md/

 

[Ox]

It was a 0 and I made it a 1.


-----------------

Think Snow Eh!
Ox

 

[Ox]

OK, I switched it back, and it's the same, but I'm not ending the program in G57 as I used G53 to position my slides to the door, and if holding G53 is not an option, then it must go to G54 anyhow.

If I ended in G57, then maybe it would hold that value?
IDK / IDC about that.
If it would hold G53, and not default to G54, then that I care about.


I wonder what it would take to put a real keyboard on it? (not qwerty)
One that has brackets and doesn't need INSERT keyed after every entry?
Or doesn't that change that?


-------------------

Think Snow Eh!
Ox

 

[dandrummerman21]

So what do you use G53 for? I understand its use, but I don't understand why people use it?

We just set a location for G30 and set an m-code to take us there. In this shop, m27 on all of the vertical mills will take the table to the door in xy and home in z.

:9024(M27)
 
G90G94G80G40G17G0
G91G28Z0.M19
G91G30X0.Y0.
G90
M99

On a zero, parameters 735-738 are for setting G30 (it's called 2nd reference position in the parameter manual)






Is this more complicated than g53? I guess so.

 

[Vancbiker]

So what do you use G53 for? I understand its use, but I don't understand why people use it?

We just set a location for G30 and set an m-code to take us there. In this shop, m27 on all of the vertical mills will take the table to the door in xy and home in z.

:9024(M27)
 
G90G94G80G40G17G0
G91G28Z0.M19
G91G30X0.Y0.
G90
M99

On a zero, parameters 735-738 are for setting G30 (it's called 2nd reference position in the parameter manual)






Is this more complicated than g53? I guess so.

If you only have one load/unload position the G30 is just as good as G53. If different jobs have different load/unload positions then IMO, G53 is easier as you go not have to change parameters.

 

[Ox]

G53 = "Base" in the offset page - right?
Which would be MACHINE co-ordinates + any shifts that you enter?
So if you default to your "base" offset, and it is set to zero, then when you touch off, you have the value to enter in your Fix Offset page looking at you on the CRT.

No?

As mine is now, I have G54 set to zero, and the machine defaults to G54.
So when I touch off, the values that I need are on the CRT, and I can then enter them into G55 - G59.
I lose G54 for no good reason.

If I have a real FIX offset set up in G54, then things get muddy, and I need to go to my ALL CRT page and find the MACHINE Coordinants I guess and figger from there. (again - adding in my tool value yet....)

I guess I could muddy the water some more and call an H24 in MDI every time that I touch off in Z.
I guess that's not really much different than calling up an offset on the lathe when touching off...
And I git the fact that on this control (unlike the Siemens) when I call up T24, I am not stuck with offset 24.
Seldom have I ever had application for a second offset for the same tool in a mill, but I know that it can happen in odd cases.... Mostly on CDC I'm sure.


I'm just trying to get this machine set the way that I expect it to be as best that I can.
Figger out how to work around those issues that I cannot edit - as best that I can.
And then decide how bad I hate it...


One of the best things about Fanuc (other than parts and support availability - AND unit reliability in the first place!) is that I know my way around the 16/18 controls fairly well, and I feel confident in my ability to edit params w/o screwing up the whole world, and making it as I think that it should be. I may need help locating the required param from time to time, but ....



-------------------

Think Snow Eh!
Ox

 

[MotoX]

I should make a list of parameters that I need to change when we get a new (used) machine.

I will pay you for a list of parameters that will change how fanuc machines behave.

Ive got a samsung SL25 (copy of a mori), that has some weird mannerisms that i would love to solve.

 

[Ox]

He linked one above, but I try my darndest to find a better site for downloading.
Too easy to get tangled up in blue on sites like that....

If I don';t have it, I can just ask Hardinge.
They will send me the file.


----------------

Think Snow Eh!
Ox

 

[Ox]

Yet again, on the 16/18, you can scroll through the params and have a clue what they are for as you go.
Many times you can get by without the book.
Or by looking through the list, you at least can zero in on the area that you need to be.
You may need some daffynation to get honed in specifically....

On this 0, not hardly.


-------------------

Think Snow Eh!~
Ox

 

[dandrummerman21]

If you only have one load/unload position the G30 is just as good as G53. If different jobs have different load/unload positions then IMO, G53 is easier as you go not have to change parameters

Fair enough. In cases like that, I add G91G0X___ after M27. If I was feeling bold (I'm not) I could make m27 a macro program and type M27X5 which would take me 5 inches to the right of M30.

But now my M27 IS more complicated than g53. To be honest I just like the m-code because it also makes sure some g-codes are cancelled. On some machines, it makes sure g5.1 is off, thru coolant, etc.

G53 = "Base" in the offset page - right?
Which would be MACHINE co-ordinates + any shifts that you enter?
So if you default to your "base" offset, and it is set to zero, then when you touch off, you have the value to enter in your Fix Offset page looking at you on the CRT.

No?

As mine is now, I have G54 set to zero, and the machine defaults to G54.
So when I touch off, the values that I need are on the CRT, and I can then enter them into G55 - G59.
I lose G54 for no good reason.

If I have a real FIX offset set up in G54, then things get muddy, and I need to go to my ALL CRT page and find the MACHINE Coordinants I guess and figger from there. (again - adding in my tool value yet....)

I guess I could muddy the water some more and call an H24 in MDI every time that I touch off in Z.
I guess that's not really much different than calling up an offset on the lathe when touching off...
And I git the fact that on this control (unlike the Siemens) when I call up T24, I am not stuck with offset 24.
Seldom have I ever had application for a second offset for the same tool in a mill, but I know that it can happen in odd cases.... Mostly on CDC I'm sure.


I'm just trying to get this machine set the way that I expect it to be as best that I can.
Figger out how to work around those issues that I cannot edit - as best that I can.
And then decide how bad I hate it...


One of the best things about Fanuc (other than parts and support availability - AND unit reliability in the first place!) is that I know my way around the 16/18 controls fairly well, and I feel confident in my ability to edit params w/o screwing up the whole world, and making it as I think that it should be. I may need help locating the required param from time to time, but ....



-------------------

Think Snow Eh!
Ox

So the point of what I was explaining before, I look at the machine coordinates shown on that sideways picture you posted before.

HOWEVER, if you like to activate the tool length, and have it show up in the absolute position page, and handwheel the machine down to the top of the part, and be able to look at that number and key it in, then no, my method doesn't work. I always added the number manually via calculator. (Does your 0md have the input+ button on the screen when adjusting offsets? 0mc and previous 0 controls do NOT have that button like 16/18/21 machines do.)

It's totally a different strokes for different folks situation. As long as you know what the hell you're doing, it will obviously work. But it would drive me mad to look at the absolute display while a program is running, and knowing that an endmill is 1" deep in a part, but the display shows 5" in z (while x and y are proper).

I will pay you for a list of parameters that will change how fanuc machines behave.

Ive got a samsung SL25 (copy of a mori), that has some weird mannerisms that i would love to solve.

Well, what's it doing?

Yet again, on the 16/18, you can scroll through the params and have a clue what they are for as you go.
Many times you can get by without the book.
Or by looking through the list, you at least can zero in on the area that you need to be.
You may need some daffynation to get honed in specifically....

On this 0, not hardly.


-------------------

Think Snow Eh!~
Ox

Yup, there's far fewer parameters. But they are kinda scattered all over the place, little organization.

 

[Ox]

I have my CRT set to show actual program locations.
You can see that in my pic.

IDK what you are talking about ???


-----------------

Think Snow Eh!
Ox

 

[Ox]

Doo all mills with 0 controls default to G54 when not actively elsewhere?
Or is it just this model?

Does an 18 act the same way?
If I had an 18, would I be pissed about this anyway?

The thought that it would default to a fixture offset that may or may not even be used on a job is just bazaar!


---------------

Think Snow Eh!
Ox

 

[dandrummerman21]

Maybe I am wrong in my assumption on this screen, but you appear to be in auto. And it might be at z-.080 based on what the relative readout says.



So I assumed your tool was -.080 and your absolute coordinate display was at z+7.32 (it would have been about half that if you didn't have that wear offset)

If I'm wrong and it shows up right when in program, disregard.

Edit: another one of your screenshots show you having the full screen up with coordinates, but if you look at the top, it's relative, not absolute. That might not be a problem to you, but relative coordinates can be cleared or changed on the fly, at will. That was the point of my ... point.


As for defaulting to g54, the 16i machines we've obtained over the years usually default to g54 as well unless I change parameter (which I do).