Z work offset and/or tool length offset in vmc??

Nerdlinger · May 27, 2021

Hi Everybody!

I was flipping through Smid's CNC Programming Handbook because I enjoy going "back to the basics" from time to time and he really preaches the use of Z0 in work offsets and then compensating entirely via the tool length offset:

...The Z0 offset entry is very important in the machine control. Specified Z0 means that the coordinate setting for the Z amount does not change from one part to another...The only time there is a need to consider Z-axis within the work offset setting is in those cases where the height of each part in the setup is different...

I can dig it...and that is what we do on machines that don't have probes (leave Z0, touch the tools off to the top of the part, tool offset measure, Bob's your uncle! (so our tool length offsets end up being like -15.123.) But on machines with probes I enjoy setting the Z0 offset to a number that represents the distance from the gage line to the top of the work (on our Haas's) or the distance from the table top to the top of the work (on our Brother's) and then having the tool length offset represent that actual length of the tool!

I imagine this is just one of those, "more than one way to skin a cat" scenarios but I am inquisitive by nature and tend to suffer from tunnel vision so I wanted to ask if there IS a generally-accepted way of setting top of stock and tool length out there or if it is more of a, "one guy tells you thing and one guy tells you another" deal.

Thank you!

camhead420 · May 27, 2021

This is one of those what ever works best for you things.
Also could of just opened a can of worms :willy_nilly:

leeko · May 27, 2021

I'm still wrapping my head around this, and forgive me if it's a dumb question:

If you leave the WCS Z value as 0, and touch off on the part to set your tool offset instead, doesn't that mean you have to re-touch off every tool, every time you run a different part? That seems like a hassle compared to leaving the tool offsets untouched and just changing to WCS z-offset value.

I suppose it makes sense if you're setting up for a production run, but for prototyping or small numbers of parts it seems like the other way makes more sense.

There's probably something I'm missing here - it's been known to happen

Lee

Sent from my SM-N960U using Tapatalk

Booze Daily · May 27, 2021

I prefer the gage line method. It makes more sense for my use. Plus it's a quick visual check on the tool length.

Booze Daily · May 27, 2021

leeko said:
If you leave the WCS Z value as 0, and touch off on the part to set your tool offset instead, doesn't that mean you have to re-touch off every tool, every time you run a different part? That seems like a hassle compared to leaving the tool offsets untouched and just changing to WCS z-offset value.

There's probably something I'm missing here - it's been known to happen

Lee

Sent from my SM-N960U using Tapatalk

Yes you would re-touch off for each new set-up. So instead, what seems to be common is to touch off a standard place, like say a 1-2-3 block on the table. Now you measure from the 1-2-3 block to the top of the work and put that in G54 Z value. It's sort of a hybrid of the two.

GENERALDISARRAY · May 27, 2021

So whenever you setup a new part, you have to set every tool you are going to use? Even if they are always in the magazine?

Very productive.

Booze Daily · May 27, 2021

^^ Not if you use the gage line method or the hybrid method.

gregormarwick · May 27, 2021

If you're running a cnc mill and are not using at least a dial type height setter and a haimer, then you are wasting huge amounts of time.

And yes, not using the Z work offset is ridiculous.

angelw · May 27, 2021

Hello Nerdlinger,
Yes, there are many ways to set the tools and coordinate system for the part. However, where the Z Workshift is always left at Zero, requires the tool length offset to be set for all tools used in the program for each new job. Not all that inconvenient where only few tools are used, but rather time wasting where many tools are involved. Further, unless the routine is to set all tools in the magazine, whether they're used in the particular job or not, this system can result in tools in the magazine with length offsets that suits nothing and the potential for a crash should any of these tools be introduced to the program later and inadvertently not have their tool length offset set.

With systems that use the Z Workshift to set the workpiece coordinate system, the tool length offsets of all tools in the magazine should suit the current workpiece Z Zero by setting the Z Workshift with any tool in the magazine. I have my clients develop the habit of always setting the Tool Length Offset of any new tool introduced to the machine, as soon as its put into the machine.

The method of setting the Tool Length Offset of each tool and not using a Z Workshift Offset, also precludes being able to pre set the Offsets away from the machine unless an accurate dimension for where Z Zero of the workpiece involved is within the machine space.

Overall, the Zero Z Workshift methods provides a few more opportunities to stack the machine.

Regards,

Bill

mmurray70 · May 27, 2021

Nerdlinger said:
I was flipping through Smid's CNC Programming Handbook because I enjoy going "back to the basics" from time to time and he really preaches the use of Z0 in work offsets and then compensating entirely via the tool length offset

Sounds like Mr. Smid has spent more time writing books then running machines.

mhajicek · May 27, 2021

Yeah, no.

As said above, if you touch off the tool on the work you need to repeat that for every setup, even if using the same tools. If your typical job has three tools, maybe not a big deal. Mine often have over 20 per job, and I group jobs that reuse many of the same cutters to save setup time.

Also think about what happens when you break or wear out a tool. If you're touching on the top of stock, when you set your replacement tool it will be on another piece of stock, which may be a little thicker or thinner, so if you replace one tool you have to touch them all. If you're doing short runs in aluminum, again, maybe not a big deal. Longer runs in steels, Ti, etc., big headache. And how do you save the part that was running when the tool failed? You can't touch off with a part in place. Gotta pull it, put in fresh stock, touch off all your tools again, then put the part back and hope it's in the same place. If it's a $10 piece of stock, no big. Hundreds or thousands, or for some people tens of thousands of dollars per piece of stock, that's a problem.

SeymourDumore · May 27, 2021

Nerdlinger said:
(leave Z0, touch the tools off to the top of the part, tool offset measure, Bob's your uncle! (so our tool length offsets end up being like -15.123.) But on machines with probes I enjoy setting the Z0 offset to a number that represents the distance from the gage line to the top of the work (on our Haas's) or the distance from the table top to the top of the work (on our Brother's) and then having the tool length offset represent that actual length of the tool!

Not sure how Haas is working nowadays, but 10 years ago there was a definite different procedure in picking up tools between a lathe with toolsettter and without.
(If I had my guess, their mills were the same.)
All of that is a bunch of bullsihite because the Haas programmers couldn't figure out how to apply a different logic!

There SHOULD BE NO DIFFERENCE in work and tool pickup procedure between probe or no-probe!
In fact, that is the PRIMARY reason I don't have a probe on my Haas VMC-s!

MORI figured it out on the lathes, so should the idiot "programmers" at Haas.

But to answer your question, your Work Z offset ( Z-workshift) should NEVER be 0! ( If it is, you're either doing it wrong or should run and get a lotto ticket)

Nerdlinger · May 27, 2021

Thanks, everyone! It sounds like we are all on the same page...I just got spooked a bit when I read what I read in that book :skep:

. Yes - on the two machines we have that do not have probes we touch off every tool to the top of the work on every set up. It's not that big of deal because most jobs run for at least a week, but I understand that loss of efficiency compared to what I consider to be the "proper" gage line method we use on all the other machines. Thanks, again! :cheers:

gregormarwick · May 27, 2021

Nerdlinger said:
I just got spooked a bit when I read what I read in that book

I wouldn't pay much attention to that book. Years ago I bought a copy, because the word was that it was the book to read if you wanted to get good. I probably opened my copy three or four times. I haven't seen it for years, and I don't really care where it went. I have a similar opinion of that book to the machinery's handbook. A huge expensive tome, filled with not very useful information.

My indifference to the CNC Programming Handbook is the reason I bought Sinha's book instead of Smid's when I wanted to learn more about macro programming. In retrospect I think that was a very good choice.

Fancuku · May 27, 2021

Smid sounds like one of those guys who learned programming but never actually touched a machine.
Setting the work offset to zero and touching off tools on every new job even if you never moved them is insanity.

706jim · May 28, 2021

Fancuku said:
Smid sounds like one of those guys who learned programming but never actually touched a machine.
Setting the work offset to zero and touching off tools on every new job even if you never moved them is insanity.

Absolutely.

Set tool length offsets as a positive distance from spindle gauge line to tool tip and the offsets will remain usable for any number of programs.

There are several methods of accomplishing this (including mine)so I'm not going to wade through them again.

Scruffy887 · May 28, 2021

And if you use Mazatrol you measure a tool and done. Break it and measure the replacement. Go back to work on any part.
I know, sorry, I'll let myself out...........

DouglasJRizzo · May 30, 2021

Nerdlinger said:
I imagine this is just one of those, "more than one way to skin a cat" scenarios but I am inquisitive by nature and tend to suffer from tunnel vision so I wanted to ask if there IS a generally-accepted way of setting top of stock and tool length out there or if it is more of a, "one guy tells you thing and one guy tells you another" deal.

Thank you!

Smid isn't wrong, and in fact, it's how I set up mills for years. However I learned a pretty good trick when I worked for a MTB. On mills that didn't have probes, you would set all the tools off a 1-2-3 block on the table. Then, measure from the top of the workpiece to the block and input that into the work coordinate "Z". Now, when you have a different job and say, the tools were the same, you just measure the height to the block and the machine is set rather than touching off tools individually again. Kinda like a lathe setup in a mill. Seems to work OK.

Spindle and tool probes however, are largely making this obsolete, excepting on older machines.

gregormarwick · May 30, 2021

DouglasJRizzo said:
Smid isn't wrong, and in fact, it's how I set up mills for years. However I learned a pretty good trick when I worked for a MTB. On mills that didn't have probes, you would set all the tools off a 1-2-3 block on the table. Then, measure from the top of the workpiece to the block and input that into the work coordinate "Z". Now, when you have a different job and say, the tools were the same, you just measure the height to the block and the machine is set rather than touching off tools individually again. Kinda like a lathe setup in a mill. Seems to work OK.

Spindle and tool probes however, are largely making this obsolete, excepting on older machines.

This is effectively what you're doing when you use a height setter and a haimer, except the height setter + haimer is easier, quicker, and more accurate.

Vancbiker · May 30, 2021

In the very early 80s when I first stood in front of a VMC, the guy doing the training taught the “touch each tool to the part” method and always leave the fixture offset for Z at 0. Not knowing any better at the time I blindly followed what was taught. This was on a machine with an indexer so I was setting different tool offsets for each face! Thankfully it only held 20 tools and there were 99 offsets.

After a while I got to thinking it was a waste of time so started trying different things. First thing I did was touch just one tool to the new workpiece and note the difference and then just incrementally adjust the offsets for the remaining tools. Was noticeably faster than touching all the tools.

Then I started wondering why the control had a Z fixture offset when I was told to always leave it 0. Started playing around with small numbers in there to see what happened and man did the lights come on. Started setting tools to a set block and setting the fixture offset as the difference between the set block and the 0 face of the part.

Thought I was a genius and had sussed out a great secret in how to improve CNC operations. Then a few years later, discovered that other shops were doing the same thing. My balloon was quickly popped.

Z work offset and/or tool length offset in vmc??

Stainless

Cast Iron

Stainless

Titanium

Titanium

Hot Rolled

Titanium

Diamond

Diamond

Stainless

Diamond

Diamond

Stainless

Diamond

Cast Iron

Titanium

Titanium

Titanium

Diamond

Diamond

Similar threads