Thread: Tool Length Offsets

All right, I need some info for benefits of gage line tool length offsets. I recently started a new gig and need to tighten up the milling department. Some of the guys are giving me the deer in the headlight look when I try to explain it. They are even running half of the machines with gage line offsets and the other half with what I call large negative offsets (touching off the part from reference home). They even own a Parlec presetter the use for checking run out only.

So in an effort to pre-stage jobs I want get everyone on the same page. I discussed that the tool is in relation to the machine not the part or some tool block. The ability to set tools on the presetter and keep the spindle making parts, but some are just a little harder to bring over to my way of thinking.

I was hoping that all you might have some good reasons pro or con. I like to
know both.

Thanks,

ME

Standardization is the key.
Personally, I want accurate tool offsets and work offsets for the same reasons you mention. I want tools pre-set, measured and ready to drop into the machine.
You can flub the numbers in many manners and get the machine to run. But the next guy coming in doesn't have a clue what the first guy did. There is a reason that you have a tool offset table and a wpc table in the control.
In a one-man job shop, it makes no difference how it's done as the man knows what he did. In a production situation, it's 180° different.

Good grief.

I quickly learned many yrs ago on a CNC Knee Mill that when there is more than one tool involved at all - that some sorta standardized offset needed to be used.

The presetter doesn't need to be accurate - just repeatable!



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

Think Snow Eh!
Ox

In the words of Ox, Good Grief!

The question of standardization, answer is a definiate YES. You may hafta beat half the crew senseless, but you gotta settle on one common method.

Regarding which method, as Tony said. For multiple machines running production or quick changeovers a pre-staged toolsetup is best. Gageline will allow you to set any tool for any machine. Of course the question will be how to keep the measured values with the tool and how to make sure it's entered properly (unless an automatic upload is available)
Also - tough I use the fixed reference method - if I'm looking at it correctly, one half the shop will have to be beaten to understand that length offset changes are reversed when using gage-line vs. fixed reference.
I think that will be the biggest issue.

They're just borrowed werds. I borrowed them from a good freind of mine named Charlie.

He's a good man and will likely let you use them as well.



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

Just say NO to neg offsets!
Ox

A con is pretty to come up with for that. IMO your first step is getting everyone to understand where tool length zero is and how to find it. On a CAT 50 taper a line axially up the center starts to generate a length value after the point where the taper diameter reaches 2.750”. Give each operator a blank end mill holder and even engrave the length on the side that they can use this as their “machine master gauge” and when they add this value to the machine position when touching a pc. it should start to come together for them. A Z axis movement in your program on the line containing the H for that tool ( I like 6”) to a check plane will give an opportunity to verify tool length before getting too close. Macros that calculate and input a work surface using a tool length or do the opposite can really cut down on data entry errors and save time.

The D1 values on this page are gauge line values for a variety of tools:

http://www.tools-n-gizmos.com/specs/Tapers.html

Con? None that I can think of.
Pro?
1. Gauge length offset is "logical" (a long tool has a bigger offset value)
2. Can be measured out of the machine with some sort of presetter.
3. Literally can be used unchanged for years if the tool is an indexable face mill etc.
4. How do you "touch-off" a curved surface?

Yeah, the only con was negated by the fact that they already own a presetter.

Are guage line offsets synonymous with positive tool length offsets? Much as I like the standardization concept of gauge line measurements, I don't like positive offsets. I'm not sure if that is the issue here, but it could merit further discussion.

But running two systems would have to be at least as bad as that, if not worse

You have two problems when trying to convert from negative offsets on tools to positive offests of tools from a presetter. The main problem you face does not involve the presetter or tools at all, but the fixture offsets of the part.

The machine "Z" is the length from the gauge line of the spindle to the table. For example, my Fryar MC40 has a Z of -25.620 (close, but a memory guess) from spindle gauge line to the bare table. Of course there are the little guards and the drive dogs, but the gauge line to bare table is the key, and this is Z negative.

You set a vise on the bare table and set a part in the vise. You measure part top Z ZERO to the table. For example, lets say you have a Kurt holding a piece that will be drilled, and the top surface of this part is 4 inches above the bare table. Your Z fixture offset is now -21.620

This becomes your hardest part of the change over. The idea/concept of the tool presetter doing positive lengths becomes easier once this concept becomes clear. I had to learn this idea and convert many in a shop as well. Once I got the fixture offset idea down (and how this can be changed to accomodate the repeatability of the presetter), the change over from the old part touch off method to the presetter became very easy.

I have yet to understand why on earth a MTB would set up a VMC with a -Z to the table. It goes completely against the cartesian coordinate system, and against the left hand rule. Z from the table to the gage line of the spindle when the spindle is up and home should be a positive number.
The WPC Z should be a positive number and the tool offset should be a positive number. The control knows to subtract both the WPC Z and the TO Z from the actual positive reference number.
I've seen machines set this way (lathes and mills)......but IMHO, it's stupid......The good thing is it can be easily changed with a simple parameter.

My question is how would you implement positive offsets on a Haas? When you touch off a tool on a Haas, the tool offset measure button puts the machine absolute z position into the field.

On the Haas, the Z value is referenced to the tool home position. On my machine it's around 16 inches from the table, with 4 above home.

On other machines I've always used the positive offset method, using any tool to touch off part zero. With the Haas you have to touch off all tools or make certain you always have a part of the table unoccupied to measure tools from.

On my brother I tell it the stack up from the table top and it measures the tool length from the gage face. When I set part zeros I just take the machine absolute - .003 - tool length. On my centroid controlled knee mill I have all tools referenced from a spot drill. I can use the probe or touch off the spot drill to get part zero. Since the knee goes up and down, this is a prerequisite.

Originally Posted by HuFlungDung

Are guage line offsets synonymous with positive tool length offsets?

Hu...yes they would be the value from the tip of the tool to the GL making them a positive value.

Originally Posted by Tonytn36

I have yet to understand why on earth a MTB would set up a VMC with a -Z to the table. It goes completely against the cartesian coordinate system, and against the left hand rule.

Tony…I could not agree with you more. I have never understood why they setup the machines that way. I have never run that way and no one has been able to explain to me the benefit of running that way. Every time I get to a new place or setting up new equipment that is the first thing that I change.

When I put a part on the machine that is a given height 6.565 I want to enter that number and see that number in my workoffsets or fixture offsets, not some -20.3569 number. That does not tell me anything about what my part is. When I put a tool in the machine that is a given height 4.254 to GL, I want to see that number and enter that number in my offsets. This is also a much easier visual check of the tool. If there is 8.659 in the offset page you know right away that the tool is not offset.

IMO it just makes everything easier to see at a glance and with a tape measure to roughly verify rather than having to grab the calculator and start adding and subtracting.

ME,
As everyone has stated standardization is key. Some people will get it others will take time. When I am setting up a product line, part and tool offsets is where I will explain until I am blue in the face to make sure they understand how the machine is setup. I would not just give them a procedure on paper that explains step by step how to offset a tool. I will make a drawing of the machine and tool and explain what is being + and – in order to come to the value and why.

Stevo

Originally Posted by HuFlungDung

Much as I like the standardization concept of gauge line measurements, I don't like positive offsets.

We use negative tool length offsets simply because waaaayy back somebody put a G44 on the line containing the H so it was just continued as a legacy practice so as not to get spanked running an old program. The odd time a minus sign might be missed on manual entry mostly by new hires that think our way is wierd.
Why don't you like positive offsets?

I agree the length in the registry should jive to what you see in front of you from the spindle face to tool tip.

I don't like positive offsets because of a perceived danger of having more potential for crashes if a minus sign were accidentally input with the offset. The negative offset method does not have this same danger, as inputting a positive offset takes the tool up higher where no harm occurs, except an overtravel alarm.

I suppose in real life working with positive offsets exclusively, that one just would never ever have the habit of typing a minus sign, so maybe it is not a real concern once one's mind has been thoroughly trained in that method.

I did read about an unfortunate crash that occurred when someone using the positive offset method accidentally zeroed one of the offsets by an inattentive finger stroke during a jog move. Of course that sort of dangerous happenstance looms large in my mind

I do admit that looking at the list of negative length offsets is pretty abstract. Sure, one sees a general trend that longer tools are less negative than short tools, but the exact lengths are certainly not there to easily check with a tape or a rule.

I dunno, maybe I'll change one day

One thing about standardization is what the standardization can do for you beyond one spindle (along what Seymore stated). For a single machine, the 'standard' is very arguable unless you have many jobs that require a lot of tool changing.

With positive offsetting (or gage line setting), every tool can not only be pre-set, but it will also retain that measurement regardless of which machine or job set up. Say you have to move a job from one machine to another. With preset tools, you can simply move all of them and you only need to use one tool for the work offset. All of the rest will follow. Or, you get done with a job, you can label the tool with it's offset and stick it on a rack. When a job comes up to have to use that tool, simply put it in place with it's tool offset. This also allows you to use machines that are considerably different without changing the tool offset. For example: I can use a tool in a 20 x 40 VMC for a part, then move that tool to a 1000mm HMC and the tool offset doesn't change. Or take a 40 taper tool from my Robodrill and stick in my Mazak 5-axis and still use the same tool offset.

No more touching off of parts/set up for tool length. This is also nice for setting up multiple operations or parts on one machine. Yes, you could use the coordinate Z offsetting to adjust for the "other" part with negative offsetting. However, if one of them changes or the set up is removed (while the "other" continues to run), you've lost the measured point. I can set up a new job using tools from a previous job without picking up new tool offsets. You can schedule "like jobs" back to back that may use similar tools. But if the fixture changes, you don't have to remeasure tool offsets.

... and yes, with a tape measure or scale, you can easily at a glance see if the tool offset is "correct".

My question is how would you implement positive offsets on a Haas? When you touch off a tool on a Haas, the tool offset measure button puts the machine absolute z position into the field.

There's a parameter for this.... although you already might be set. Most machines can do this. Right now, it doesn't have a known point to calculate from. The number is probably zero right now so it only 'sees' the machine position. I don't recall the Haas parameter or variable for this but someone else might know.

Originally Posted by HuFlungDung

I don't like positive offsets because of a perceived danger of having more potential for crashes if a minus sign were accidentally input with the offset. The negative offset method does not have this same danger, as inputting a positive offset takes the tool up higher where no harm occurs, except an overtravel alarm.

If you're really worried about this you can put a saftey sub-pgm that checks that tool length is longer than a certian minimum.

For instance; read active tool length-> if less than 2.0" goto error

Psycho and all.

For the record, using negative toolengths does not in any way mean you have to re-pick tools for different jobs or fixture.
Yes, I know most places out there do that, but that's not a correct assumption by any means.
And yes, Haas can be set up to use positive ( gageline) offsets. That is one way the Renishaw or Marposs toolsetter works on a Haas, but it also works with negative offsets as well.
I use and prefer negative offsets exclusively so I'd hafta look at the parameters to find out how to change them, but can be done.

Originally Posted by SeymourDumore

I use and prefer negative offsets exclusively so I'd hafta look at the parameters to find out how to change them, but can be done.

I don't get where parameters come into play???

G43 - tool length compensation (plus)
G44 - tool length compensation (minus)

Originally Posted by Curt B

I don't get where parameters come into play???

G43 - tool length compensation (plus)
G44 - tool length compensation (minus)

I guess that answered that then.....

With that note however, having different systems in one shop makes even less sense!
Imagine a tool with positive offset running with a G43 call.