Fanuc tool length offset, compensating for fixture offset.

BRIAN.T · Mar 28, 2019

Im switching my shop from the old "touch off to the top of the part" to a more accurate touch off point.

Most of my machines are Mitsubishi control which will ignore any fixture offset Z value, thus giving you a consistent tool length every time. My two fanuc controls however will add (or subtract) whatever you have set for G54 Z. So if I touch off a drill to the table during setup I get say z-14.800, but as soon as I add in my fixture offset and touch off the same tool I get z-17.800, which will obviously crash.

So my question is, other than why is fanuc the absolute worst, is which parameter do I need to change in order to stop that from happening. The tool length should be the tool length regardless of anything else happening in the machine.

Fanuc iO-MC circa 2006 maybe.

Vancbiker · Mar 28, 2019

Fixture offsets do not affect or change the machine coordinate position display which is the one you should be using for tool setting. I suspect you are using the absolute position display which does change with fixture offset changes.

BRIAN.T · Mar 28, 2019

Vancbiker said:
Fixture offsets do not affect or change the machine coordinate position display which is the one you should be using for tool setting. I suspect you are using the absolute position display which does change with fixture offset changes.

Please explain! I could certainly use the machine position for setting tools, but that would force me to write everything down and type in into my offset table according. The Z measure button, which is what we use to input a value into the offset table only reads one number, which I guess is the absolute position.

13engines · Mar 28, 2019

Vancbiker said:
Fixture offsets do not affect or change the machine coordinate position display which is the one you should be using for tool setting. I suspect you are using the absolute position display which does change with fixture offset changes.

I totally agree that the machine coordinate display is the final word on no nonsense position for tool offsets and everything else, but if the OP is using the time and key punch saving EOB/Z/Input command to enter tool offsets, that function includes any setting in the both the Shift and Work Coordinate areas of the control. Great function, as long as you're on top of what's set elsewhere. More then anything, I use this Z "problem" as the Fanuc scorning OP seems to think it is, to my advantage. One very basic example... on my OMC machine I use a 4" tall part setter. Add Z4.0 to the Shift register when measuring tools and using EOB/Z/Input, and it adds the 4" to the tool length automatically. Then I'm really working off of the table height or part top or whatever the setter is on.

Not sure there is a parameter to change that. Best way to find out is get your parameter book out and start digging. Sounds like a couple good days of bathroom reading.

Dave

guest · Mar 28, 2019

The tool measure function uses the relative Z position. If the machine has absolute encoders, relative and absolute match up when the machine starts up, so absolute and relative display the same numbers.

On machines without absolute encoders, you typically origin all axes on home-out, and relative displays the machine position.

The WCS offset measure function uses the machine position. So if you have a WCS offset in Z, the tool length measure will be from there on machines with ABS encoders, because the relative display is showing the absolute position.

If you want the tool lengths to be measured from Z home position, you would origin relative Z at Z home before setting tool lengths.

BRIAN.T · Mar 28, 2019

13engines said:
I totally agree that the machine coordinate display is the final word on no nonsense position for tool offsets and everything else, but if the OP is using the time and key punch saving EOB/Z/Input command to enter tool offsets, that function includes any setting in the both the Shift and Work Coordinate areas of the control. Great function, as long as you're on top of what's set elsewhere. More then anything, I use this Z "problem" as the Fanuc scorning OP seems to think it is, to my advantage. One very basic example... on my OMC machine I use a 4" tall part setter. Add Z4.0 to the Shift register when measuring tools and using EOB/Z/Input, and it adds the 4" to the tool length automatically. Then I'm really working off of the table height or part top or whatever the setter is on.

Not sure there is a parameter to change that. Best way to find out is get your parameter book out and start digging. Sounds like a couple good days of bathroom reading.

Dave

This is exactly what I'm hoping to do, however the problem I foresee is when my guys break a tool they would have to remember to remove any z workshift in the fixture offset, then add the 4" back to the ext shift correct?

And if I'm being honest I never realized how much I hated fanuc until I started using heidenhain. Fanuc certainly makes parts, but let's be honest it's not how you'd design a control if it were up you. I mean "switch to edit-typd program number -f set - program number - p set- execute, just to transfer a program to the CNC memory. Come on that's outrageous.

BRIAN.T · Mar 28, 2019

guest said:
If you want the tool lengths to be measured from Z home position, you would origin relative Z at Z home before setting tool lengths.

Where else would someone want their tools measured from?

guest · Mar 28, 2019

BRIAN.T said:
Where else would someone want their tools measured from?

Lots of different ways to do it. Reference tools, gage length. Check this recent thread.

Problem setting tool/workoffsets with Haimer and 123 block

13engines · Mar 28, 2019

BRIAN.T said:
This is exactly what I'm hoping to do, however the problem I foresee is when my guys break a tool they would have to remember to remove any z workshift in the fixture offset, then add the 4" back to the ext shift correct?

Brian,

If you're replacing a broken tool and you have Z offsets entered in your SHIFT register and/or in the Z of whatever Work Offset is currently active, unless you want to zero out everything and put it back when you're done, here it's best to just write down what you see in the Machine Coordinate Display and enter it manually. (In lieu of EOB/Z/Input) If you're measuring off a part setter gauge, which are typically of known height and at whole values, it's certainly simple enough for anyone to add that single digit height to what's read off the Machine Coordinate Display.

If you tend to put your Z work shifts in your Work Coordinate registers instead of the SHIFT register, one trick you can do is keep your work setter Z height entered into an unused Work Coordinate space. Say G59 or G54P48 if you have that many. Then when you go to set new tools with your setting gauge, call up the tool in MDI along with the Work Coordinate where your tool setter height is entered. In other words, make say G59 active while setting tools. Broken tool? MDI G59; green button before measuring it. Undoubtedly, or hopefully rather, your main program will call the needed active Work Offset again before work starts.

If you tend to put a global Z offset in your SHIFT register and leave G54-G59 alone, revert to the first paragraph. That or as you said. Remove it, put your Z4. gauge height in there, use EOB/Z/Input to enter the tool, then put your working Z offset back when done.

Dave

BRIAN.T · Mar 28, 2019

guest said:
Lots of different ways to do it. Reference tools, gage length. Check this recent thread.

Problem setting tool/workoffsets with Haimer and 123 block

Well in understand there are plenty of place to touch a tool off TO, the FROM is always machine zero. Unless your on a fanuc, in which case it might be machine zero, plus some random work offset value

guest · Mar 28, 2019

BRIAN.T said:
Well in understand there are plenty of place to touch a tool off TO, the FROM is always machine zero. Unless your on a fanuc, in which case it might be machine zero, plus some random work offset value

I guess I am not understanding your complaint.

The tool length is the distance from Z home to the part zero, calculated by the control as the value in the tool length offset register plus the value in the G54 Z offset register.

If you want to use the tool measure function, you want to origin relative based on how you are going to set your G54 Z- wherever that happens to be. If you want something other than zero in G54 Z, the tool length needs to be measured relative to that position, because the G54 Z value is going to be added to the tool length when you command the machine to that absolute position.

For example- Probe a 123 block. Zero relative. Touch off each tool to the 123 block, measure the tool length. The tool length measured is the difference in gage length between the tool and the probe. Now probe the top of the part. Go to the work offset page and enter Z0 <measure>. This sets the G54 Z0 to the machine position based on the length of the probe. All your tool lengths are set relative to the length of the probe, so you're good to go.

OR- Zero relative at Z home position. Touch off all you tools to the 123 block, measure the length. The tool length is the distance from home position to the 123 block. Now probe the 123 block, zero Z relative again and probe the top of the part. Input the number displayed in relative Z into G54 Z. This sets the G54 value as the distance from the 123 block to the top of the part, and the G54 Z value is NOT the machine position.

Both methods get to the same place.

BRIAN.T · Mar 28, 2019

guest said:
I guess I am not understanding your complaint.

The tool length is the distance from Z home to the part zero, calculated by the control as the value in the tool length offset register plus the value in the G54 Z offset register.

If you want to use the tool measure function, you want to origin relative based on how you are going to set your G54 Z- wherever that happens to be. If you want something other than zero in G54 Z, the tool length needs to be measured relative to that position, because the G54 Z value is going to be added to the tool length when you command the machine to that absolute position.

For example- Probe a 123 block. Zero relative. Touch off each tool to the 123 block, measure the tool length. The tool length measured is the difference in gage length between the tool and the probe. Now probe the top of the part. Go to the work offset page and enter Z0 <measure>. This sets the G54 Z0 to the machine position based on the length of the probe. All your tool lengths are set relative to the length of the probe, so you're good to go.

OR- Zero relative at Z home position. Touch off all you tools to the 123 block, measure the length. The tool length is the distance from home position to the 123 block. Now probe the 123 block, zero Z relative again and probe the top of the part. Input the number displayed in relative Z into G54 Z. This sets the G54 value as the distance from the 123 block to the top of the part, and the G54 Z value is NOT the machine position.

Both methods get to the same place.

Yes you are correct, all of those things are true, and straight forward, however the problem comes into play when you need to switch or change a broken tool. After you have put any value into your G54 z fixture offset you can no longer touch off to the same position, without either clearing out your fixture offset or MDI yourself into a fixture offset you're not using.

Say you set up a job, tools to a 123 block, and you probe the distance from said 123 to your work coordinate. If 100 parts later you need to touch off a new tool, what do you do? Simply touch off to the same 123 block as you would during setup, nope. If you do what happens? Your tool rapids down whatever that additional Z offset distance may be.

So, I'm back to either touching off additional tools to a work offset I'm not using (seems odd) or I write down my machine position... On paper.... To input simple information into a computer... Seems easy enough but come on really??

I'm making my hatred for fanuc sound worse then it really is, they are ok, they make parts.

SeymourDumore · Mar 28, 2019

guest said:
The tool length is the distance from Z home to the part zero, calculated by the control as the value in the tool length offset register plus the value in the G54 Z offset register.

Well, it might be so on your machine, but it really shouldn't be that way, and is likely settable in parameters.

The tool length should be a distance traveled from machine home to a fixed reference.
Then, the Work G54 offset should be the distance from Fixed reference to Part Z0.

That is how in-machine toolsetters work.

BRIAN.T · Mar 28, 2019

SeymourDumore said:
Well, it might be so on your machine, but it really shouldn't be that way, and is likely settable in parameters.

The tool length should be a distance traveled from machine home to a fixed reference.
Then, the Work G54 offset should be the distance from Fixed reference to Part Z0.

That is how in-machine toolsetters work.

You know what I'm talking about! It definitely shouldn't be that way. It's crazy dangerous. I'll keep digging through my parameter book.

sinha · Mar 29, 2019

BRIAN.T said:
Im switching my shop from the old "touch off to the top of the part" to a more accurate touch off point.

Most of my machines are Mitsubishi control which will ignore any fixture offset Z value, thus giving you a consistent tool length every time. My two fanuc controls however will add (or subtract) whatever you have set for G54 Z. So if I touch off a drill to the table during setup I get say z-14.800, but as soon as I add in my fixture offset and touch off the same tool I get z-17.800, which will obviously crash.

So my question is, other than why is fanuc the absolute worst, is which parameter do I need to change in order to stop that from happening. The tool length should be the tool length regardless of anything else happening in the machine.

Fanuc iO-MC circa 2006 maybe.

Fanuc does not use the term "fixture offset." It is perhaps "Ext offset" you are talking about. It is generally kept zero.

Tool length offset would be equal to tool length when the spindle gauge line is used for setting WCS such as G54.

Mike1974 · Mar 29, 2019

BRIAN.T said:
This is exactly what I'm hoping to do, however the problem I foresee is when my guys break a tool they would have to remember to remove any z workshift in the fixture offset, then add the 4" back to the ext shift correct?

And if I'm being honest I never realized how much I hated fanuc until I started using heidenhain. Fanuc certainly makes parts, but let's be honest it's not how you'd design a control if it were up you. I mean "switch to edit-typd program number -f set - program number - p set- execute, just to transfer a program to the CNC memory. Come on that's outrageous.

I don't know that is fanuc or the mtb? I ran a robodrill that was a pita to load programs, but the Haas (which is fanuc based, right(?)) is easy, list program, select program, F2 and copy location, but I digress.

I don't remember the details, but our robodrill had a goofy thing about setting tools. It would add/subtract the relative value when you set the tool!!! You had to go home in z and zero the relative beforre touching tools. We even had methods out to try and fix that for us and they couldn't :skep:

I suspect your control is doing the same type of thing, and probably no way around it unless you can get to the ladder and know how to make changes. Maybe it is "just" a bit change, but it wasn't on ours (from what I was told).

BRIAN.T · Mar 29, 2019

sinha said:
Fanuc does not use the term "fixture offset." It is perhaps "Ext offset" you are talking about. It is generally kept zero.

Tool length offset would be equal to tool length when the spindle gauge line is used for setting WCS such as G54.

While that maybe true, the world uses the term fixture offsets. So I have have chosen that as well. Semantics aside, I only use Ext shift for dry runs and such, it's is kept at zero the rest of the time. My work coordinate is the issue we're talking about here, so G54, G55, G56 ect Z value.

Mike1974 · Mar 29, 2019

SeymourDumore said:
Well, it might be so on your machine, but it really shouldn't be that way, and is likely settable in parameters.

The tool length should be a distance traveled from machine home to a fixed reference.
Then, the Work G54 offset should be the distance from Fixed reference to Part Z0.

That is how in-machine toolsetters work.

I *think* that is only true if you are using negative tool length offsets. If they are positive, it is the distance from tool tip to gage line, which lets you set tools offline.

BRIAN.T · Mar 29, 2019

Mike1974 said:
I don't know that is fanuc or the mtb? I ran a robodrill that was a pita to load programs, but the Haas (which is fanuc based, right(?)) is easy, list program, select program, F2 and copy location, but I digress.

I don't remember the details, but our robodrill had a goofy thing about setting tools. It would add/subtract the relative value when you set the tool!!! You had to go home in z and zero the relative beforre touching tools. We even had methods out to try and fix that for us and they couldn't I suspect your control is doing the same type of thing, and probably no way around it unless you can get to the ladder and know how to make changes. Maybe it is "just" a bit change, but it wasn't on ours (from what I was told).

Yeah, not all of my fanuc controls (I have 3) require that nonsensical command to transfer a program, just the one that is brand new

the control from 2001 is actually pretty straight forward. Not to say it isn't without it's own issues.

And yeah that's exactly whats happening, it's adding to my length for reasons we may never understand. Who could have possibly thought that was a good idea. I'm going to check my old fanuc from 2001 today to see if it does the same thing. Different control different MTB, different everything. Maybe it's just this brand.

BRIAN.T · Mar 29, 2019

Mike1974 said:
I *think* that is only true if you are using negative tool length offsets. If they are positive, it is the distance from tool tip to gage line, which lets you set tools offline.

I am not familiar with this methodology. Please explain!

Fanuc tool length offset, compensating for fixture offset.

Cast Iron

Diamond

Cast Iron

Stainless

guest

Guest

Cast Iron

Cast Iron

guest

Guest

Stainless

Cast Iron

guest

Guest

Cast Iron

Diamond

Cast Iron

Titanium

Diamond

Cast Iron

Diamond

Cast Iron

Cast Iron

Similar threads