[Se5a]

This mill homes to the rear right of the bed, normally I would run Mdi from that point so all inputs would be negative coordinates.

This uses the absolute coordinates which I can’t change. As you can see if I enter 0.00 for each axis it moves to the near center of the bed, maybe used a fixture at one point?

From where should I measure my work offsets from?

Thanks
Craig







Sent from my iPhone using Tapatalk

[the_gentlegiant]

Hello Craig,

Is your screen messed up?

You might want to check back to our many older posts where I think I went over all of this.

From the looks of your MDI input and the position of your table , you currently have the negative version of those absolute numbers entered into G54. Normally you wouldn't have a Z value in your Work Offset unless you're using a tool setter or master tool system.

Like I said earlier, everything you enter into the machine, whether work positions or tool offsets relates to the machine's Home Position which is faithfully described under the "Machine" heading on the Position Page.

If you locate the face and left corner of the fixed jaw of your vise and while still there, enter the numbers you see in the "Machine" position into the G54 Work Offset area of the control, and then after returning Z to Home, MDI G54 G0 X0.Y0. The machine will move to that same corner of the vise. The Absolute Position Display will show X.Y0. Z should be dealt with using the tool height (H) offsets. You set those the same way as the work offsets. Touch off each tool onto the top of your stock or whatever you programmed as Z Zero in your drawing, look at the "Machine" Position Display for Z, enter that negative number into the corresponding tool height offset then MDI this in (rapids set low-watch distance to go display)

G90G54G0X0.Y0.
G43Z1.H1

The above assumes tool one. You MDI that code and your tool will end up one inch above the left corner of your vise and the Absolute position display will say X0.Y0.Z1. If the Z doesn't say one inch you might need to change a parameter. Honestly... I almost never watch or care about what the REL and ABS position displays say anyway. Seriously. Seldom look, unless I'm playing around manually on something. Distance To Go on the Check screen is the one to care about when running each tool for the first time.

When setting your tool heights try this. It works on some machines and saves typing. ( I think I explained this earlier but...)

When your tool is touching the top of the stock or wherever you want Z0. to be, and with the curser at the active tool on the Tool Height Offset page, hit EOB/Z then Input. Roll over EOB and Z like you would for Control Alt on a keyboard. On my OM machine this enters the current machine position into the Tool Height Offset. Very handy and saves errors. Maybe it will work on yours.

Hope this helps. Forgive me if you know all or most of this already.

[Se5a]

It’s starting to make sense, so what I did was move the spindle to the corner of the vise, just eyeball it to learn it.

Set those machine cord, into par 1221 aka G54 it did not move where I should have, there was a value entered in par 1220 “external workpiece zero point offset value” I zeroed these numbers and now when I Mdi x0y0z0 it moves right to the corner of my vise G54

Am I on track?

Thanks for the help!


Sent from my iPhone using Tapatalk

[the_gentlegiant]

Yes that's certainly getting there. Again you wouldn't generally enter a Z value in your G54 or par 1221. Leave the Z setting for the Tool Offset Page.

(Repeat of above) Change what you put in G54 Z to Zero. Take tool one, whatever it is, and bring it eyeball very close to the top of that same vise jaw you positioned to earlier. Take what you see in the Z part of the "Machine" coordinate and enter it into tool one's offset register. (a negative number) Then do as I said previous. Put Z back home and MDI -

G90G54G0X0.Y0.
G43Z1.H1

That will bring tool one to one inch above the corner of your vise and should make the Absolute Display say the same. You see how that works? G43 calls in the tool height offset. (G49 cancels it) Imagine that each tool in your carousel is going to be a different length. The machine needs to know those differences, and that it what the tool offset page is for. Each time you call a new tool you also call G43 with it's companion H number. H2 tool two. H7 tool seven etc. Take a look back at the programming example I think I shared awhile back. You'll see where G43 is brought in with each tool as it is approaching the work.

Again in this case G54 has Z set to Zero and this is normal. The control of Z height is taken care of by the tool offsets. I admit your machine seems to have peculiarities on how things are entered. You have G54 but have to enter it into a parameter? Seems weird but maybe that's how yours works.

The only time(s) you would have Z set in a Work Coordinate is if you were always leaving the same tools in the carousel or leaving many of the same ones in there. Then using a Master type tool system. I think it best that you measure the tools for each job until you get used to how the machine works. Meaning leave G54 Z at zero. That par 1220 External Workpiece Zero Point sounds like the master work offset register. Not sure you have Work Offsets G54 thru G59. If you did and you had them all set to say six different vises mounted on your table, and then realized all your programming was off by 0.025" in X. You could set X0.025 in that par 1220 and it would shift all the six work offsets over twenty five thou. A master offset as it were. You're good in setting it all to zero. That is definitely its usual setting.

I apologize for not knowing what peculiarities exist in your 20M control. It is an odd bird. Fanucs are pretty much the same across the board but yours might be one of the odd ones as I think some of the very early ones like 3 and 6 are. And some of the conversational stuff.

[Se5a]

It worked awesome! Here is my offset page where I input, there is an offset key on the panel.




When I use my cad program it inputs all the G code for you correct?


Sent from my iPhone using Tapatalk

[the_gentlegiant]

Well great. Glad it worked. I hope it helps your understanding of how the machine keeps track of where it is and where the tools are.

Push that soft key under WORK, it should bring up your work offset pages. Does it? Or does it have those parameters you mentioned listed? If you hit the SETTING page, that will take you to your parameters. The OPRT or OPERATION button will take you other places as will the right and left soft arrows if you have them.

If you have a great post processor in your CAM it will fill in most of the G codes. I would warn strongly against blindly following what your post spits out. Study up on the Smid book I mentioned. You really should have a medium working knowledge of what all the G and M codes mean. Not kidding. Even if you're always referring to a cheat sheet.

I see you have a thread going about MM to inch. As was said there, after you get your machine acting properly in inch, use G20 and G21 to switch between, but never within the same program.

If you have tool offsets set in one measurement system, they may or may not automatically revert to the new system. Be careful with that until you know how your machine handles the shift from inch to metric. Incorrectly set or converted tool heights are a road to disaster. Work Offsets too.

BTW - if you do find a Work Coordinate page with G54 and all its friends there. You will likely also find one labeled maybe EXT. Probably the first one on the page. This is that global offset I spoke of last time that effects all of them.

[Se5a]

It’s does bring up the work offset pages




Changing from mm to in did convert the offsets automatically




Sent from my iPhone using Tapatalk

[machinehop5]

...just to make things more complex for you, there is a G10/G11 code (I think) you can use also.
https://www.cnczone.com/forums/fanuc...metry-g10.html

[the_gentlegiant]

Well Craig, things are looking up. Looks like no more entering work coordinates into parameters. Your machine is looking more and more regular all the time. Go ahead and zero out G55 thru G59 if you're not using them. And yes I see there is that EXT offset which affects all the others globally. Just FYI. If you hit the Page Down key from either the Tool or the Work Coordinates screens, you will find a second screen containing more of them. You probably have 32 tool offsets and 6 Work Offsets. Someday when you start using Cutter Radius Compensation, you will use those spare tool offsets to set your tool radii compensation numbers in.

When you're in the Tool Offset page setting tool heights, don't forget to try that EOB/Z/INPUT thing I mentioned for setting tool heights. If it works you'll be eternally grateful for knowing about it.

I don't doubt the machine changed your settings when going from metric to inch. Just make sure it does the math correctly.

Here are a couple tricks you can use that EXT work coordinate for.

1) Say you have work coordinates for three vises (G54-G56) on your table and are testing out a new program. You can enter a positive Z value in the EXT register and it will cause your program to run above the parts in a safe area. Say the tool you want to check out has a maximum Z coordinate of Z-1.25. You could put Z1.5 in the EXT register and it would run your part safely over all the vises. Once you see that everything is good, just set it back to zero to run the part for real.

2) You might want to get a tool height setting device. Usually they're designed at some whole number like 3 or 4" tall exactly. You place that device on top of your stock when setting your tool heights. Say your tool setter is 4" tall. Before starting your measurements you would enter Z4.0 in the EXT register. This will automatically add the 4" that represents the height setter. Once you're done with measuring tools, set that back to Zero and you will be good to go. The machine will think you set your tools all the way down at the surface of your stock. Again your G54 Z value will remain Zero.

In lieu of a part setter, I've always used 0.001" shim stock between the tool and the work piece. Under that scenario you would not set anything in EXT, but simply enter what is seen on the Machine Coordinate screen as we've discussed.

Anyway... time to start programming!