What's new
What's new

1989 LeBlond Makino RMC55 - Fanuc 0M - Display question

Chevy427z

Stainless
Joined
Oct 12, 2004
Location
Clinton, North Carolina
Morning Folks.

Ever since I have owned this machine (about 12 years) the Z axis has never displayed "absolutely". It's nothing critical to my operation, so I never pursued it. It'd be nice to see as X and Y are fine.

Is there a secret or magic setting or parameter somewhere?

Many thanks.

Mark
 

Attachments

  • 20210912_151605.jpg
    20210912_151605.jpg
    90.8 KB · Views: 58
Parameter 18 bit 5.

In the absolute coordinate display, tool length compensation is included/is not included.

Obviously will only show when g43 is active.
 
Thank you!

Have I been setting my tools incorrectly all this time? I set my tool where I want it, then input the relative value that I see into the tool register.

I assumed that G43 would always be be active (with or without calling it up in a program), apparently an incorrect assumption. I will take a closer look and play around with my numbers.

Thanks again!

Mark
 
I knew this would be difficult to explain. I know the A is for the 4th axis. That's not an issue.

X and Y indicate where my tool is in relation to the part zero (in absolute). Z should indicate where the tool is in relation to the part, also (in absolute). Positive above it and negative below (or into) it. Z has always indicated where the tool is incrementally where it is in relation to the machine, not the part. Say my tool is 2" above the part, the display would should it's position relative to the machine, like -7.something (for example).

Dan (above) has me thinking that I have been setting my tools wrong. I touch off my tool and input into the tool register what I see on my "REL"ative screen. Say I read Z=-7.312, that's exactly what I would put into my tool register. If anyone needs more pictures of the various steps I take to set my tools, I'm only too happy to oblige.

Mark

edited: I haven't had a chance, yet, to look at the parameters that Dan talked about.
 
There's a whole bunch of ways to set your tools. Depends on what you have available to you.

For example, we have an offline tool presetter. There is a standard tool which measures 4" to gage line that we calibrate the presetter to. All tools are set on this machine. All tool lengths are positive. All work offsets for z are the distance from the 0" gage line (basically the face of the spindle)

So if I took a probe or some other tool, and the probe/tool was 13.123" long, you'd touch it to the top of the part and add 13.123" to the absolute z coordinate. Probes make this simple but you accomplish the same thing whether it's an endmill touching the surface of your part.


Other people will leave G54 Z set to 0 and all tool lengths are negative. In that case, you'd look at the machine coordinates and simply type them as you see them. This doesn't work as well if you have multiple parts at different heights on the table with different coordinates, although you can work around that by having an incremental distance measuring the distance between the top of g54 and g55, for example.

There's others who have tool presetters on the table, or set all the tools off a gage block or similar.

There's probably some nuanced methods i haven't thought of.


Have you been making good parts with relative ease of tool setting? then I'd suggest you maybe stick with what you do. It isn't "wrong" if it works. But there might be simpler (to you) methods.


If you are running a milling program and you know the tool is at Z-.250 but you look at the screen and in absolute it says Z-7.632, that's annoying as hell and the parameter I posted should fix that. It is very likely that hitting reset on your control will reset g43, so after hitting reset, the coordinate should go back to how it looks now.

If in the middle of the program with g43 active, you single block it and go into MPG, the absolute coordinate should still show as absolute with cutter comp on. So if you simply wanted to do some "manual milling", you could literally have a bit of code like this:

T1M6
G90G80G40G17
G0G54X0Y0S1000M3
G43H1Z5.
M0(PUT IN MPG AND DO YOUR MANUAL MILLING HERE)
M0
M0
G28G91G0Z0M19
G90


... and the coordinates you see on the screen should all be absolute with G43 cutter comp enabled. so if you went 1" deep it would show that.
 
Thank you for the detailed explanation! I know that took some time, and I appreciate it!

I'll check that parameter and possibly figure another way around this.

To answer your question, I've had no problems setting my tools like this and running programs consistently, for years, in fact. It's just annoying to look at the screen and not know for sure if it's where it should be, like when proving out a program step by step and watching the "distance to go". I'm just extra careful.

Your post jogged my memory to when I ran a bunch of Fadals in another shop. We'd use a 2-4-6 block standing on end to touch our tools off. We'd use an indicator attached to the spindle to determine the difference between that point and the top of the part to set G54 Z.

I'll mess around with it and see what I come up with. Thanks again for your time. Truly appreciated.

Mark
 








 
Back
Top