Fanuc OMC tapedrill G43 H offsets not calculated

[alexius]

Hello all, I have a Fanuc Tapedrill with OMC controll. My tool offsets are not getting activated. If I put in G43 H6 Z10 for instance, the head moves to a certain position but the offset is not calculated in. I also tried it through a program from the memory but no luck.
If I look in the PGRM screen in MDI mode the selected H number is displayed after a G43 but no compensation for the offset. The work offsets function as normal.
Anyone have an idea what is going wrong?

Similar Threads:

• Tapedrill Mate T 1008 and PS585 alarms
• Fanuc Tapedrill Model T goes through toolchange with same tool
• Pratt and Whitney Fanuc 0-MB Tapedrill Parameters
• Need Help!- (v25 Pro) Automatically calculated feeds / speeds... mostly way too high.
• Problem- Incorrect toolpath calculated

[the_gentlegiant]

I'm just going to stick to the basics because I don't know how deep your Fanuc skills are.

In your example, how and where did you measure your tool 6? Was it on the top of the part or are you using a tool setter of some kind? If so are you taking into account the tool setter height? What reference position did you use for the height of the tool and where did you enter that information? At the time of tool measurement, was the EXT (external) work offset at Z0.?

[alexius]

I'm just going to stick to the basics because I don't know how deep your Fanuc skills are.

In your example, how and where did you measure your tool 6? Was it on the top of the part or are you using a tool setter of some kind? If so are you taking into account the tool setter height? What reference position did you use for the height of the tool and where did you enter that information? At the time of tool measurement, was the EXT (external) work offset at Z0.?

Hello, thanks for your response.
I use a tool setter and take this height in account. Take the machine coordinates from home Z to the head on the work table and fill it in at G53 (work offset 00) then I fill in the height of the tool setter at G56 and activate G56. So now the absolute reads 0 from tool setter to head. Then I touch the setter with the tool and read the absolute distance. That's my tool offset and I fill it in at offset 002 or 003 etc. In the offset page. Then I select MDI and fill in G43 H3 Z0 and INPUT then OUTPUT START. The head moves and you see in the screen that H3 is selected. But the H offset does not get calculated in absolute. What do you mean with EXT?

[the_gentlegiant]

Hello, thanks for your response.
I use a tool setter and take this height in account. Take the machine coordinates from home Z to the head on the work table and fill it in at G53 (work offset 00) then I fill in the height of the tool setter at G56 and activate G56. So now the absolute reads 0 from tool setter to head. Then I touch the setter with the tool and read the absolute distance. That's my tool offset and I fill it in at offset 002 or 003 etc. In the offset page. Then I select MDI and fill in G43 H3 Z0 and INPUT then OUTPUT START. The head moves and you see in the screen that H3 is selected. But the H offset does not get calculated in absolute. What do you mean with EXT?

Hi alexius,

Is this a system you've used for years on this machine and now it stopped working? Or is this a new to you machine and control and you thought this was the way to go?

Personally I've never paid much attention to Absolute or Relative position screens. When setting offsets of any kind, the Machine Position or Machine Coordinates is the only thing a person should be paying attention to. This position is the true position of the machine including the Z head no matter what else you have entered. Even if you have something in your G53 work offset 00 (same as EXT. or the first set of coordinates on the Work Offset Page) the Machine Coordinate will always show True Position from Machine Reference Zero. (Zero Returned Zero) Whereas your Relative and Absolute positions will mix in numbers or settings you might have entered elsewhere.

Before I go any further, are you using a manual setting tool of known height that you set on top of your part Z reference surface, whereas you're measuring tools for each job? Or are you setting this manual setter on say your machine table and using it as a master, where any new tool gets measured at the same place and is used for any job now or in the future?

Or... are you using a permanently mounted electronic part setter like a Renishaw or the likes of? Of course this falls into the Master type of part setting category, where tools are always measured there and Z heights for individual jobs are adjusted in the work offset pages.


Just for fun, if you have a manual setter of known height, say 100mm, set it on top of your part. Now go to your G53 Offset 00 (EXT) area and enter Z100. (Positive number) Now touch off a tool on the setter. When the setter is at zero or wherever it normally should be with the tool touching, go to the Tool Height Offset Page and put the cursor next to the Tool Height Offset number you wish to save it to.

Now while holding down EOB, hit Z, release and hit INPUT. (Sort of a Control Alt Delete computer keyboard kind of move) This should place the correct height offset into the space next to the cursor. After holding EOB and hitting Z, you should see the number appear in the buffer area at the lower left corner of your screen. Anyway... the number entered will be the same number that you'd have if you touched the tool off on top of the part. Meaning it includes the tool setter height. But before running the job, remove the 100mm form G53 Offset 00. If you don't your tool will incorrectly stop 100mm above the part.

EDIT IN: I can't recall off the top of my head if this matters or not. When doing the trick above, make sure there are no other active work offset Z settings in play. In this example above, if you look at the number entered into your tool offset, it should be 100mm more negative then the number that appears in the Machine Position or Machine Coordinate area. If it is more or less then 100mm, that means that another active work offset is being included. Say G54 happens to be active while measuring tools and it has Z-36.26mm entered. This might mess things up. Can't remember if this matters or not, thinking maybe not. The test is in what I just said about machine position and measured tool height being exactly 100mm different in this example.

I think this is a Fanuc thing but it might be a Machine Tool Builder thing. It works on the late 90's OMC machine. Hopefully it works on yours. You might have to be in EDIT or MDI or HANDLE. Not sure if that matters.

Regardless, get back as to what type of setter and system you're using. It may be tomorrow before I can answer again. Though others may certainly chime in.

[the_gentlegiant]

Any luck yet finding out what the problem is?

Did the EOB Z INPUT thing work on your machine?

[alexius]

See my YouTube video how i set the work offset for tool setting.
(there is a small amount Z offset due to a typing error but this video is for explanation)

After this procedure in let the tool tip touch the setter to zero. I then look at the absolute value and enter this on offset 001 for instance. Then i go to MDI then push PRGM and enter there G43 (INPUT) H1 (INPUT) Z0 (INPUT) (OUTPUT START)
Then the tool offset 001 should be loaded right? I also tried if it made a difference doing this in G00 or G01 but nothing happens. On the screen you can see that H1 is selected but the absolute value doesn't change.

[alexius]

The EOB Z input works

[the_gentlegiant]

Hi alexius,

What do I search to see your video? What's the title?

Still don't know why you're messing around with Absolute or Relative position screens when setting tool offsets, but seeing how you do things in the video will explain a lot. Maybe after that I'll have some useful or relevant help to offer.

While I'm here let me ask again.

Did this process you're using work in the past for years and then suddenly stopped working? Or is this a new-to-you machine and you're still figuring it out?

[alexius]

Hi alexius,

What do I search to see your video? What's the title?

Still don't know why you're messing around with Absolute or Relative position screens when setting tool offsets, but seeing how you do things in the video will explain a lot. Maybe after that I'll have some useful or relevant help to offer.

While I'm here let me ask again.

Did this process you're using work in the past for years and then suddenly stopped working? Or is this a new-to-you machine and you're still figuring it out?

https://youtu.be/jtrZ-rew1Ak

But bottom line is G43 isn't activated/calculated

[the_gentlegiant]

Hello alexius,

Wow... okay. How can I say this? Everything I saw in that video the machine and control did just as you asked. You didn't do anything to activate the tool offset for tool 1 or any tool. You pretty much just zeroed out a work offset Z setting. Not even sure if that's what happened.

Unless you were using the machine spindle head just as an example, there is no reason you should ever need to measure what you measured.Meaning the machine head.

At least I see you're using a manual measuring device. (How tall is the blue measuring device?)

Answer me this. Are you wanting to leave tools loaded all the time to use over and over on multiple jobs? Or do you think you'll need to reload most tools when going from one job to another? What I'm getting at is are you looking to use a master system where you always measure tools in one spot on the machine and not on top of the programmed Z zero of your part? Or do you plan to just measure on top of your work piece(s) (part) setting new offsets for each job?

Answer me that and I can set you straight.

I see your machine has Home Position in the upper left corner instead of upper right. Never saw that before. I say that because I see positive X numbers in your work coordinates. Normally everything is negative.

Anyway... what I saw in the video has nothing to do with setting tool offsets and getting the machine ready to do work. Getting the position screens to say what you want is the least of your problems. They will act accordingly when they are used properly.

I don't have time now as I'm running production work.

Try this:

Take that blue measuring thing and set it on top of your workpiece.

Zero out all your Z work offsets including the G53 00 one.

In your Work Offset Screen, enter the Z height of the measuring device in the G53 or 00 or (EXT) Machine Work offset. Set a positive number.

Bring tool 1 down on top of the measuring device.

Go to the tool offset page and put the cursor next to tool 1

Hit EOB Z IINPUT - The number that is entered there will be the Machine Position plus the Height of your tool setter.

Send your tool back to Z home.

Zero out the G53 00 offset where you had the tool setter height entered.

Make sure G54 Z is also zero.

Jog the machine in X to move the spindle away from the workpiece.

Enter this small program into the machine

%
O100 (TEST)

G17G21G40G49G54G80G90G98

G0G43Z10.H1

M00
%

The tool should stop 10mm above the part. Check it by jogging the tool over the part. I bet your absolute screen says Z10. too. If it doesn't there may be a parameter needing changing. Can't recall.

That's all I have time for now.

Try it and let me know what you got. Good luck.

BTW - The production runs are about a half hour each. So have time between runs to check in.

[the_gentlegiant]

Hi alexius

Looking at some parameters. Copy and pasted. Change at your own risk.

0001 #I PROD In the relative coordinate display, tool length compensation is included/is not included. (my machine is 0 )

0002 #1 PPD Coordinate system setting does not cause relative coordinates to be pre-set/causes. (my machine is 1 )

0010 #7 APRS At a manual reference position return, automatic coordinate system setting is not executed/is executed. (my machine is 1 )

0024 #6 CLCL At a manual reference position return, the local coordinate system is not canceled/is canceled. (my machine is 0 )

I included my machine settings but that doesn't mean yours have to match.

Honestly in 20 years I almost never have watched the position screens. I think my OMC machine Absolute doesn't include the tool offset but it never bothered me as I never look anyway. What you measure at the part is what's important.

Still thinking you're not setting the tool offsets correctly.

[alexius]

Ok i did exactly as you asked. (see YouTube link: )
The tool stops 10mm above the setter and not above the part. Yes i put in 50mm (toolsetter height) at G53 z.
After the EOB tool offset input in set g53 at zero again. But no change and the absolute value isn't changing as can be seen.

[alexius]

Ok i did exactly as you asked. (see YouTube link: )
The tool stops 10mm above the setter and not above the part. Yes i put in 50mm (toolsetter height) at G53 z.
After the EOB tool offset input in set g53 at zero again. But no change and the absolute value isn't changing as can be seen.

A small update; it seems that the tool offsets are taken in account but the absolute values do not include the tool offsets. I'm almost certain that this is a parameter setting. I've changed parameter 0048 #1 and 0018 #5 (see attachments) but to no effect.

[the_gentlegiant]

According to my book, parameter 48 is for twin turret lathes only.

Parameter 18.5 should do what you're after. On my machine (parameter 0018.5) is 0 and mine never displays correctly either. That's one reason I never bother looking at it. This machine has made thousands of parts over many years without it. Last time I'll bother saying it, you don't need it for programmed work. If you plan on lots of manual stuff then maybe, but I don't use mine manually as it sort of defeats the purpose.

Update: Well thanks to you I changed 0018.5 to 1 on my machine and it makes the Absolute Display display the programmed position just like it should. G0G43Z0.1 displays Z0.1000 when it should. G1Z0. displays Z0.0000 All good. I'll still never bother looking at it, but thanks anyway. It might be nice to have there to watch when I'm bored waiting for the machine to finish a run.

Anyway... I think I've exhausted about all I can think of. Besides you don't bother answering any of my questions and the videos don't show anything a person can see. Keep scanning the books. You might find something else.

0018.5 at 1 should do it. Not sure why it's not on yours. Just to be sure - Bit 5 is third from left. 00100000

[alexius]

First of all let me make one thing very clear;
I'm very grateful that you put so much effort in helping me!
unfortunately i didn't had much time the last days. I had limited time
to try the things you told me to check. Also i wanted to keep the thread as
light as possible, so i only responded to the things that were relevant (in my opinion)
But the main thing is: YOU SOLVED THE PROBLEMS!!
The thing was that i got confused because of the fact that the Absolute values didn't
represent the actual Absolute positions (since it didn’t take the tool offsets in account)
I'm going to try the 0018 position 00100000 tonight, i i did 00001000 as 5th position.

[alexius]

First of all let me make one thing very clear;
I'm very grateful that you put so much effort in helping me!
unfortunately i didn't had much time the last days. I had limited time
to try the things you told me to check. Also i wanted to keep the thread as
light as possible, so i only responded to the things that were relevant (in my opinion)
But the main thing is: YOU SOLVED THE PROBLEMS!!
The thing was that i got confused because of the fact that the Absolute values didn't
represent the actual Absolute positions (since it didn’t take the tool offsets in account)
I'm going to try the 0018 position 00100000 tonight, i i did 00001000 as 5th position.

UPDATE:
setting parameter 0018 The correct way does the trick!
Now my absolute values are true. (yes I want to do some occasional manual milling)

Now only one thing that I want to get right. On the Fanuc OMC you must do a G49 priora tool change. But then I always get a movement to the position minus the tool offset. Is there any way around this?