What's new
What's new

Presetter - Offset question

Sean S

Titanium
Joined
Dec 20, 2000
Location
Coos Bay, OR
Hi all,
Although I've had a toolchanging CNC (Deckel FP4NC-TC) for several years, I've never used the tool offsets in any project.

Since I'm rarely making more than one of anything (and even that's rare), and using only a few tools (mixed with "manual" actions), I am a total offset novice.

Generally I've just touched off each tool prior to running the part of the program that used it.

I do have a presetter, although I have never really used it.

So here I am. I could really use any tips on presetter use, and how it works into the process, and I do have one actual question to start with...

...Where does one determine the zero length offset to be? Or in other words, offset from what?
Should I be making some sort of standard to touch off with in the NC that also gets used to zero the presetter or??

I feel I must be missing something pretty obvious.

Many thanks for your advice
Sean
 
Hi all,
Although I've had a toolchanging CNC (Deckel FP4NC-TC) for several years, I've never used the tool offsets in any project.

Since I'm rarely making more than one of anything (and even that's rare), and using only a few tools (mixed with "manual" actions), I am a total offset novice.

Generally I've just touched off each tool prior to running the part of the program that used it.

I do have a presetter, although I have never really used it.

So here I am. I could really use any tips on presetter use, and how it works into the process, and I do have one actual question to start with...

...Where does one determine the zero length offset to be? Or in other words, offset from what?
Should I be making some sort of standard to touch off with in the NC that also gets used to zero the presetter or??

I feel I must be missing something pretty obvious.

Many thanks for your advice
Sean

It's from the gage line of the taper to the end of the tool. The gage line of the spindle is also the reference point of the machine Z.
 
It's from the gage line of the taper to the end of the tool. The gage line of the spindle is also the reference point of the machine Z.

Thats if you want a positive offset, if you want a negative offset use a master tool longer than all the other tools. All comes down to prefrence.
 
I would highly recommend a + offset for every toy - based likely on the guageline, but where you base your measurements off of is really quite irrelivent - as long as it's always the same.

By going with the longest toy - this assumes that you will be changing offsets as soon as you pull that toy out to put something else there? Makes no sence to me. ???

Then for "part zero" you should be able to call up any toy with it's offset and jog down to the surface on the part that you want to be zero and run a G code of some sort through MDI and it would shift your reference zero postition on your machine. The exact procedure is special to your machine/control tho. (As far as the G code or whatnot. I think I useta use G92 on the Cinci?)

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

Sens Lawyers, Guns, and Money!
Ox
 
Sean,
I suggest you do the problem backwards, so to speak, to understand how to use a presetter. Take a tool (best choice would be the master tool you usually touch off with when you machine without a presetter, and preferably the longest, as Ox says), put it in your mill, and zero Z with it (by your favorite method) against a smooth piece of scrap. Now remove the tool and stick it in the presetter, note the reading (assuming the presetter starts in absolute mode, with Z=0 at the gageline) and then zero the presetter. Now, take the next tool you want to use and stick it in the presetter. The presetter will tell you the offset for the new tool. Now stick this tool in the machine and move to Z=0 (being mindful of a crash if you messed up somehow). Confirm that the tool is above the piece of scrap by the amount you measured with the presetter. Now you're golden for all the other tools you need offsets for. Next time the presetter starts in absolute mode, either go to gageline zero and set Z to the negative of the value you noted above for the master tool, or move to the Z you noted and re-zero. Of course, if you use some other method to pick up part zero, the principle is the same: just get the presetter and the other method on the same page Z-wise.

If your presetter also does tool radius, just take a light test cut and measure the actual radius you got, then plug the tool into the presetter, align on the tool radius, and set the presetter value to the value you got from the test cut. Then you can measure your other tools.

RKlopp
 
Sean,

What do you use to find part zero? Use that to set the presetter zero, then all offsets require no math (and hence no errors) to calculate.

I am for from expert, therefore everything I do is designed to eliminate possible errors. I use a Haimer 3D manual probe, or a Renishaw electronic probe. I have a set of offsets in the presetter for each. Generally I use the Renishaw because it is faster and automatic, so presetter offset #1 is set so that its length measured in the presetter would read zero. For a job, measure the other tools with this offset selected, then you can just punch them directly into the machine as read, use the probe to set part zero to zero, and punch cycle start. This eliminates any math or sign errors, you are left only with actual measuring errors or keypunch errors.

Of course you cannot measure the probe in many (most?) presetters directly, too many parts moving at once. But you can measure some reference tool in both machine and presetter, and by comparing this to the probe measured in the machine, get your offset set correctly.

Some say you should use the longest tool for reference, so that all other offsets are negative. The reasoning is that if you forget to set an offset for a tool, it won't crash (assumes the offset defaulted to zero). For me, eliminating any source of errors is the most important goal.
 
Sean,


Some say you should use the longest tool for reference, so that all other offsets are negative. The reasoning is that if you forget to set an offset for a tool, it won't crash (assumes the offset defaulted to zero). For me, eliminating any source of errors is the most important goal.


On that note - it's never a bad idear to enter +25.0000 in eny empty pockets if going the + offset route.

I HATE NEG OFFSETS! Too cornfusing and a good way to make scrap (crash?) via a bad adjustment!

---------

1,2,3,4,5,6,7, All good children go to heaven.
Ox
 
The shop I ran with Fanuc controls using fixture offsets, the tool length was always the actual tool length. The fixture offset was always the actual distance from spindle gageline to the Z zero of the part.

If you use actual tool length, any program can call the tool. If you use tool length as discrepancy from master tool, or as the air gap between the tip of the tool and part Z zero the tool length will change from program to program.

Sure you can call different TLO numbers for the same tool, but someone will change the tool and not change all the offsets. I consider that a recipe for diaster.
 
Hmm.... ok, adding and subtracting...and subtracting and adding.... I'll get this.

So far for touching off, I've just used an edge finder for part X/Y, and used the actual tool(s) via paper or light touch for part Z.

I do have a 3D probe in my future (probably Haimer), so should I get a nice long holder for the probe (one longer than most of my tooling) and go from there?

I guess then I'd have to also have the presetter push down on the probe until it reached zero.

From there I've got to decide the control vs cam offset calculation issue.

Which Renishaw model is a simple 3D probe that would work with my 4NC (ie, no control integration)?

Thanks guys. I'm learning a lot.
Sean
 
I use a Renishaw MP11 with my FP2/3NCs. It will work great with your FP4NC (right after you do the conversion to a nice Heidenhain control with built-in probe cycles :rolleyes5:).

The Haimer though, you just stick in a collet chuck or an EM holder. Concentricity doesn't matter because you adjust that out on the Haimer. You probably don't need to look for a long holder - the probe itself is longer than most tools I use, and that is with a short stylus. I cut down a 3/8 EM holder leaving just enough length below the flange for a small set screw. Buy the Haimer, you won't regret it. Much faster, no chipped tools or scratched work.

The problem with screwing down the presetter on the Haimer to measure it is the Haimer may take more force to actuate it than the presetter probe - or less, either way you get a bad measurement. However you can do the measurement indirectly by comparing a reference tool.

If you have a manual presetter with a screw micrometer, then you can measure the the probe directly. When I was using that arrangement I wrote the probe measurement on the base of the presetter with a Sharpie. The thing you have to watch for is the math and sign errors when you subtract the probe length from the tool measurement.

You could reserve a tool table location for the probe, set its comp length to whatever the probe measures in your presetter. Then remember to probe and set zero with that tool number selected and comp'ed. If you get this to work right, you can punch in the real measured length of the tools, and the control will do the subtraction for you.

I suppose if you have a real VMC with many production jobs to run and repeating setups, then setting all the offsets relative to the gage line makes sense. But I set up for each job of one or a few parts, and rarely repeat it - so eliminating the errors is key. If you doing a run of 1000, ruining the first couple as you work out the errors may be acceptable. If you are doing a run of 2 parts, ruining the first couple looks real bad.
 
I HATE NEG OFFSETS! Too cornfusing and a good way to make scrap (crash?) via a bad adjustment!

I too hate negative offsets but I know a few guys who swear by this method.

If you use actual tool length, any program can call the tool. If you use tool length as discrepancy from master tool, or as the air gap between the tip of the tool and part Z zero the tool length will change from program to program.

If you use negative offsets you can also use the tool length from program to program. The way to use it is call T0, then place a master tool in the spindle (ie 8” long) touch off the surface of the part and call the surface zero or set fixture offset so top surface is zero. Now set all tools off the same surface, if tool is shorter then master the value will be negative. Make part…When setting up for the next part place any previously set tool into spindle and touch off on the new part surface just like if you use positive offsets! It’s all preference.

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

As for using the Presetter, Your presetter should have come with a master calibrated tool with known length and radius. If you don’t have it shrink a gage pin into a tool holder and have another shop measure length and radius for you. Next place the master tool into the presetter and find the corner of the master tool then set the readout to the values scribed on the master tool for length and radius (if you want to use negative offsets just zero out the display). Now set all your tools and all the tools for your friends.

Don’t use a presetter to set your probe, do it on the machine. Take a Z cut on a part with an endmill and before you move z up set the surface to Z zero then set the probe offset to that surface, if you use the Haimer then when the indicator is at zero on the top of the part zero surface set the tool offset.
 
OK - Since I really hate the direction of this thread - I am gunna post one more time with more info...

For my Cat 40 machines - I have one of these:

http://www.kennametal.com/e-catalog...romloc=srch&parentId=1013636&sid=11AB19DEE08C

I doo not use it for tightening - as it is sold for. I have it setting on a plate with a height guage also setting on it. Slap the toy in the fixture and race the height guage crost it and you are in business.

If a digi height guage - it would be best to zero off the top of the fixture. Otherwise I subtract the known "constant" from the value on the guage.

In a more perfect werld tho - back when I did have a Quick Switch 30 CNC knee mill - and no idea how the rest of the werld did things.... I took a plate and slapped it into the 4jaw on the lathe and bored a hole in it on prox taper of the holders and with a major D of prox the guage line of the #30 holders. Slipped a cpl riser blocks under it so's the shank of the toyholder didn't bottom out on the table and then my hight guage was rat on the money!

It doesn't matter in eny way as to whether or not your guage line is a perfect match to the spindle or not. All that matters is that every toy that goes in that machine goes through that guage fixture - so that they are all relivent to one another.

This is not rocket science by eny stretch!

If you doo it this way - every toy is set for the next part - nomatter what it is. I kannot imagine setting toys up for every last diff part! :eek: What the heck are you guys - a glutten fer punishment? :skep:

[With hep from some on this board] I just recently "setup" an old retrofit that the original retrofitter aparently didn't want to bother finishing as it was set that the "home" position was zero-zero on a lathe. This made for every offset to be neg. Trying to make proper adjustments to a neg number may not hafta make junk by default - but it is much easier for it to be "my fault"! It's bass akwards to every other properly done machine in the shop - and while you still make the value less if you wunna take off more - in the case of neg values - less is more - literally. :willy_nilly:

Dooing it right doesn't hafta involve some stupid $2500 contraption with a brand name and a cert of some [feel good] sort! :rolleyes5: And I highly recommend not setting part lengths via touch-offs as a regularity. You will git "stack-up Tol" variances fer sure! (And it will take longer than slippin it through the fixture quick anyhow.)

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

Like Desperados Waitin' fer a Train!
Ox
 
Last edited:
OK, my head is spinning.

Let me add...

I do have a digital height gauge (Trimos vertical), and my presetter is also digital although manual (Trimos TPR).

I'm going to ask in the Deckel forum what the repeatability of the home position on the FP4NC is (ie cold start).
Makes me wonder if the tools could be referenced to the machine home and then just use a height gauge on the table to get Z offset (probe for X/Y)?

This is just about as confusing as I thought it would be.

Sean
 
I'm not a CNC instructor, I haven't written books on the subject either, I didn't even stay at a Holiday Inn Express recently, but I'm fascinated to see so many ways of doing what I took to be a cut and dried procedure. I'm with OX on this one, KISS for safety and productivity.

In theory, a presetter measures the length from the gage line on the taper to the end of the tool. The gage line is a theoretical point just outside the spindle taper face and just behind the tool taper v-flange. Where that line is, and where exactly you are measuring from isn't critical as long as it's somewhere near there and you measure from the same point on every tool. 1.-Every tool gets measured and the length recorded. 2.- All those lengths get input into the control in the right place for each tool. 3.- one of those tools is put into the spindle and you make sure the right tool length for that tool is activated in the control (Some controls need to be told that the tool is now in the spindle. Manually inserting the tool isn't enough). 4.- That tool is now brought down toward the table until it is exactly the correct height above the table to be where you want the program Z 0.0000 to be. 5.- The control is now told that this is Z 0.0000 (can be something like G92 Z00000 enter cyclestart). All those tools can now be used in any program and part that is programed the same way provided the Z0 is set correctly for that part, and if a tool needs to be removed and later replaced, or moved to a different pocket in the ATC, etc, all you need to do is reenter the corresponding premeasured length into the control. 4. and 5. can be done other ways, for example I use a tool height gizmo that is exactly 2.0000" tall, I place that on top of the part, bring the tool down to touch it, and set G92 to be 2.0000", because I program off the top of the part or material blank. The Haimer tool just makes it quick, and eliminates the need for the tool height gizmo. I've heard of shops that program off the top of the table and allow for fixture height, so that Z does not need to be set. I've known people to program from the fixture/bottom of the part. In those cases the tool length is set the same, but machine Z is set differently.

Before I had my presetters(with 2 you gotta make them EXACTLY the same) I set tool length in the machine, I left Z 0 alone, just put the tool in the spindle, touched it to the gizmo and pushed the set tool button. The set tool button compensates for the machine Z and the tool length at the same time. The presetter is faster and safer, and if a tool needs to be replaced in cycle, just measure it and enter the length in the control, no dicking about with simulating the top of the part to locate the gizmo.
 
Knights (Kings?)
In
Satens
Service

???


---------

Gunna make somethin of your life boy - give me one more vein!
Ox
 
Some additional notes that relate to Sean's machine and using the pre-setter. First off it should be noted here that the Dialog 3 and Dialog4 controls found on Deckels use the tool offsets localy only. That is to say each program has its own offsets that are not shared with any other program. They are contained within the program itself and not in a common register like a Fanuc.... Also on the Dialog controls you can't access any tool offset unless you are running under automatic operation. That means that the machine has no offsets applied until the program is running.

So in Sean's case i would suggest the following technique: Start with the master tool in your pre-setter. I usually use the first tool in the program, but it makes no difference as long as you keep it straight as to which one is the standard. If there is one tool that stays in the tool magazine most all the time then use that one.
Reference your tool setter to that tool length, and set your length to zero at teh master length. This is the tool zero so to speak. Now check each tool in the program or magazine for that matter. Record the relative values for each tool and keep track of the tool numbers. This will be a plus or minus value to the master depending on weather the tool is longer or shorter than the master. If you are worried about having mixed signs in your compensation values then use the shortest tool as the master...
Once you have all the values, enter them directly into mode 10..the tool comp register. Set the master tool's comp at "0" . On the Dialog the tools are listed in numerical order so the master tool is easy to remember if your use T1, that way it will be at the top of your listing.
Now load the master tool into the spindle of your machine and touch off on the surface of your stock. Set to mode "2" and set your "Z" to zero "0" and you are good to go. If you use a height block like the Lyndex setting gauge then set the height of the block in mode"2" instead of "zero" .

You will not need to reset the values of the tools in the magazine for additional programs, but your will need to copy the measured values for each tool to any additional programs. If you need to replace a tool you will need to again measure relative to the master tool to set the new tool to the correct height.
So you set all the tools to a master tool, and set the part relative to that master using an offset of "0" for the master tool.....

Cheers Ross
 
Keep It Simple Stupid(not meaning you)I thought everyone knew that


Welllllll .... if'n I didn't know it ................ :o




Per Alfa:

The only thing that I see aboot your post that would make things diff would be the fact of a non common file. (Which I [can] have on a PC based control that I have - and HATE the concept!)

I see nothing in your post indicating any reason to measure them in eny special way... ???


----------

And when I die there'll be one child borned in this werld to carry on...
Ox
 
OX:
Don't think i called out any "unusual" setting technique...just wanted to clarify that one of the tools "Must" be used as the "Zero" since for ease the referencing to the control one tool or holder must be set without any offset.
Cheers Ross
 








 
Back
Top