Problem setting tool/workoffsets with Haimer and 123 block

Hey Everyone,

To get right into it, I have a 2004 Sharp SV2412 with a Fanuc Oi-MC Controller. I am trying to set my tool offsets on a 123 block set on my table, and then measure the distance from the 123 block to the top of my part, and set that number as my Z G54 work offset.

When I did this and ran the program it crashed straight into my part and scared the s**t out of me.

Before this, I've been using the paper method off the top of my part and had no problems, but I am looking for more accuracy and repeatability.

Here is the process I am using, I hope someone can tell me where I am going wrong.

1. Set all tool offsets off 123 block (slowly raising spindle until 123 block will slide under tool)

2. Zero Haimer out on top of 123 Block, set my relative Z to zero.

3. Zero Haimer out on top of part, look at relative Z and enter this number into my Z work offset.

In my head this should work, but maybe there is something I am not getting.

Any help would be much appreciated!

Thanks!
Will

Sorry I don't have any specifics, but have you double checked your numbers??

Maybe someone with more Haimer experience will chime in...

To start, what number do you use for setting your tool offsets? Hopefully you're looking at your "Machine Position." You know... the one that doesn't change no matter what offsets you have entered elsewhere. If you're doing that, I think your method should be working. To verify what you're doing. Write down the Z axis "Machine Position" both when you measure the 1-2-3 block on the table using your Haimer and when you measure the part top with the Haimer. Take your calculator and subtract the second measurement (part) from the first (table). Set that in your G54 Z including the sign (+ or -) you end up with. If you still crash I don't know what to tell you, other then make sure you have nothing in the Z area of your G53 or "Shift" register.

Extra... absolutely make sure you have the correct tool offset called for the current tool. I mean... that's a no-brainer, but it's not like it never happens.

Dave

Minus sign mess-up? BTDT, fortunately caught it during 5% rapid used for first tool. Code asks for G55 and you put the offsets in G54. BTDT. Again caught it before disaster. Otherwise, the method you described sounds like it should work.

Boos said:

1. Set all tool offsets off 123 block (slowly raising spindle until 123 block will slide under tool)

2. Zero Haimer out on top of 123 Block, set my relative Z to zero.

3. Zero Haimer out on top of part, look at relative Z and enter this number into my Z work offset.

Click to expand...

This process works just fine, but its extremely dangerous setting your tool heights that low for this exact reason. Any mistake, or forgetting to set it will crash. Your method works exactly like you're intending though. Double check your Z origin in cam. Also make sure you don't have any additional Z- wear.

13engines said:

To start, what number do you use for setting your tool offsets? Hopefully you're looking at your "Machine Position." You know... the one that doesn't change no matter what offsets you have entered elsewhere. If you're doing that, I think your method should be working. To verify what you're doing. Write down the Z axis "Machine Position" both when you measure the 1-2-3 block on the table using your Haimer and when you measure the part top with the Haimer. Take your calculator and subtract the second measurement (part) from the first (table). Set that in your G54 Z including the sign (+ or -) you end up with. If you still crash I don't know what to tell you, other then make sure you have nothing in the Z area of your G53 or "Shift" register.

Extra... absolutely make sure you have the correct tool offset called for the current tool. I mean... that's a no-brainer, but it's not like it never happens.

Dave

Click to expand...

I think the problem must be that I put in a number wrong, probably mixed up the + or -. I really like your idea of double checking by subtracting the machine position while on top of the part from the position while on the 123 block.

rklopp said:

Minus sign mess-up? BTDT, fortunately caught it during 5% rapid used for first tool. Code asks for G55 and you put the offsets in G54. BTDT. Again caught it before disaster. Otherwise, the method you described sounds like it should work.

Click to expand...

I am almost positive after your responses that the issue was me messing up a minus sign, because I do remember some fuzzyness when I was figuring out if I was supposed to put one or not. I am going to try again and triple check before I do anything. Thank you!

couch said:

This process works just fine, but its extremely dangerous setting your tool heights that low for this exact reason. Any mistake, or forgetting to set it will crash. Your method works exactly like you're intending though. Double check your Z origin in cam. Also make sure you don't have any additional Z- wear.

Click to expand...

If I am understanding right, would it be safer if I stacked up some 123 blocks so they are above my part. This way if there is an error, it would likely just end up cutting air?

By the way, I think we might know each other. If so, I'd love to pick your brain sometime if you were willing.

Boos,

As long as you are zero'ing your Haimer to the same "level" as where you are setting your tools, you have it right. The delta from the top of the 123 to the top of your work (or wherever you put your part origin) should go in as a positive value in G54 Z value (or G55, or whatever you're using). I always do a "sanity check" on this value with a scale or tape measure. As my dad told me 50 years ago: "a 6" scale is more important than a micrometer since you are more likely to miss something by an inch than by a few thousandths". LOL

Even if you have the utmost confidence in your code and your setup process, it never hurts to 'comp up the Z maybe 2" using G52, and at least make sure that first tool comes down to the correct spot (check by sliding your 123 block under it in the 2" direction obviously).

PM

First of all on start up origin the machine and set the relative values to zeroes. Do not change this ever. You have to do this whenever you start the machine. This is your home position. Set your tools off the 123 block as you did. These values are the distance from your origin "relative screen " to the 123 block. With your offset you are planning to use active G54 thru G59 by using mdi and typing G54; insert start. Now G54 is active. Jog your haimer down to the 123 block. Use Z "0" measure. Your absolute screen should read 0 in the active offset screen. Jog to the top of your parf and put the absolute Z value in the G54 offset. This is the distance from your 123 block to your part 0. Now its ready to run. Make sure their is no values in the G53 offset. This is a incremental value that affects all of your offsets.Never mess with the relative values. These are your tool lengths from origin. Let me know if this works and I'll take you to an advance level. Good luck

Sent from my SM-G960U using Tapatalk

Boos and Guys!
Someone with a Sharp SV2412 must chime in here!

Your thinking and method of setting the workoffset with the Haimer is good.
Zero the operator ( relative, temp or whatever you want to call it ) coord at the top of the 1-2-3 block, move over to the work's Z-location and reading
the display.
BUT!!!
This is where shit becomes dependent on the MTB-s implementation!!!

Normal, common sense would dictate that a negative number from top of 1-2-3 block is entered as such, similarly a positive number is positive.
However, it really depends on where you enter it!
Don't have a Fanuc controlled mill, but do have a Oi-Tc lathe where there is a "Common" workoffset, and there are individual workoffsets ( G54, 55, 56 etc )
The thing messes with my head every time!
On this machine ( Mori Duraturn), I touch the tools to the toolsetter, and it enters a negative number for the tool.
Then, I take one of the known tools, touch the face of the rough part to set the common workoffset, and Bang!, it enters a:
1: Positive number if the part is below the toolsetter
2: Enters a negative number if the part is above the toolsetter

From here if I want to take off an additional say .02 from the part, I can do one of two things:
a: Enter -.02 in the G54 Z field
b: ADD +.02 to the common Z field and leave G54 at 0!!!

Option a: makes sense, but b: is freakin' weird!
I can wrap my head around how option b: works, but cannot figure out why Fanuc made it as an option or why Mori decided to use it!

At the same time on another Mori with the Mits control, the "Common" offset is while visible and set to 0, but it is also disabled and is not accessible in any way.

Basically what I was rambling on about is that your thinking is good, but someone with the same machine, OR Bill ( Angelw) should chime in with some more info.

Boos said:

Hey Everyone,

To get right into it, I have a 2004 Sharp SV2412 with a Fanuc Oi-MC Controller. I am trying to set my tool offsets on a 123 block set on my table, and then measure the distance from the 123 block to the top of my part, and set that number as my Z G54 work offset.

When I did this and ran the program it crashed straight into my part and scared the s**t out of me.

Before this, I've been using the paper method off the top of my part and had no problems, but I am looking for more accuracy and repeatability.

Here is the process I am using, I hope someone can tell me where I am going wrong.

1. Set all tool offsets off 123 block (slowly raising spindle until 123 block will slide under tool)

2. Zero Haimer out on top of 123 Block, set my relative Z to zero.

3. Zero Haimer out on top of part, look at relative Z and enter this number into my Z work offset.

In my head this should work, but maybe there is something I am not getting.

Any help would be much appreciated!

Thanks!
Will

Click to expand...

Hello Will,
Although not completely spelt out, I suspect that all your Tool Offset values are Minus; the Tool Offset for each tool is the Air Gap between the tip of the Tool and Surface of the 123 Block, when the tool is at the Z Reference Return Position. This being the case, using the Haimer in the manner you have described above will work. If the Haimer is Zeroed on the Top of the 123 Block and the Relative Position Displayed also set to Zero at this time, then the Relative value as displayed when the Haimer is reading Zero when contacting the Zero Surface of the work-piece, is the value that will be entered in the Work-shift Offset registry.

Given that the Tool Offset and the program coordinate are correct, the only way you could have crashed the tool into work is for the Work Z Zero to have been above the level of the 123 Block and you mistakenly entered a Minus value in the Work-shift Offset, there was a Minus Value entered in the Common Work-shift Offset, or you screwed up when setting the Relative Display to Zero.

If the control doesn't have a Measure Feature (often the case), I prefer to use a simple Tool Offset and Work-shift set Macro that uses the Machine Coordinate System in the calculations. Using such a system, to a great extent, rules out operator error when setting the Relative Display to Zero (this step may have been omitted when setting the Work-shift manually as you have described), and entering the correct value in the Tool and Work-shift Offset registry. All of the calculations and entering of the Offsets is done by the control, not the operator.

Regards,

Bill

Boos said:

If I am understanding right, would it be safer if I stacked up some 123 blocks so they are above my part. This way if there is an error, it would likely just end up cutting air?

By the way, I think we might know each other. If so, I'd love to pick your brain sometime if you were willing.

Click to expand...

Yeah, it is definitely safer to set your tools higher than your part so you're never zero below the work, but this can give over travel in Z in some cases depending on what machine/control you have. For pretty much all my first op hogout work I set my origin to the bottom of the stock if its in Talon jaws, so the top of the jaws. There are infinite ways of setting up just be consistent with it. Your method mentioned earlier is solid, just need to be very careful of your values. That Z in your work offset needs to be a positive number or you're guaranteed to crash.

I'll shoot you a text.

I use my haimer this way for z offset. I have a dial indicator z offset tool, set to exactly 4" tall at "0" reading. I reserve a tool pocket for the haimer only. I load the haimer into spindle, touch off to "0" on a fixed block on the table that is exactly 4" tall, then set the tool length for that pocket to zero if you have measure function. (All my machines have that function so what you need to reference to may vary).

This sets the haimer as the reference tool. You only do this one time.

I then touch all my tools off using the 4" tall dial indicator on the table to "0".

I then reload the haimer and touch the top of part and set the part z to zero.

couch said:

Yeah, it is definitely safer to set your tools higher than your part so you're never zero below the work, but this can give over travel in Z in some cases depending on what machine/control you have. For pretty much all my first op hogout work I set my origin to the bottom of the stock if its in Talon jaws, so the top of the jaws. There are infinite ways of setting up just be consistent with it. Your method mentioned earlier is solid, just need to be very careful of your values. That Z in your work offset needs to be a positive number or you're guaranteed to crash.

I'll shoot you a text.

Click to expand...

Hello couch,
Is this where you always set the Z Zero, or only for first op hogout? Hardy being consistent if you vary it. I've always considered Z Zero at the base of the Work-piece counter intuitive, particularly when drilling holes, cutting a pocket to a depth etc.

Using the Air Gap between the Tool Tip and Setting Device is always going to result in negative Z move unless a positive Work-shift greater than the Tool Offset is used (the negative sign in the Work-shift Offset being omitted for example). If a short Master Tool, where all other tools are compared to it, is used, then the Tool Offsets will be positive and result in a positive Z move from Reference Return, if the Minus sign of in the Work-shift is omitted. Using the Spindle Nose (the gauge line of the Tool Holder Taper) is tantamount to using the shortest possible Master Tool and one whose length is not going to change.

markp said:

if you have measure function. (All my machines have that function so what you need to reference to may vary).

Click to expand...

Definitely not the case.

Regards,

Bill

So is this controll different than 99% of fanuc based controls? Your tool offset is the distance from your home position to your "123 block" relative offset screen after the machine has been referenced and zeroed. And the z offset G54-59 is the distance from your "123 block" to your part Z0.

Sent from my SM-G960U using Tapatalk

White Lightning said:

So is this controll different than 99% of fanuc based controls? Your tool offset is the distance from your home position to your "123 block" relative offset screen after the machine has been referenced and zeroed. And the z offset G54-59 is the distance from your "123 block" to your part Z0.

Click to expand...

99% (OK really 100%) of Fanuc mill controls can set tool and fixture offsets in a few different ways. The method you use is one of them, but not the only way.

If a company is using a tool presetter, most of the time their offsets will be gage line of the tool to the tool tip and a positive value.

Vancbiker said:

99% (OK really 100%) of Fanuc mill controls can set tool and fixture offsets in a few different ways. The method you use is one of them, but not the only way.

If a company is using a tool presetter, most of the time their offsets will be gage line of the tool to the tool tip and a positive value.

Click to expand...

Is the OP asking about how to use preset tools? He just crashed. I'm guessing his machine position "relative position screen has not been referenced and zeroed thus giving a bad tool length offset. Just my opinion. Trying to simplify it.

Sent from my SM-G960U using Tapatalk

I know the OP was not asking about preset tools. I was pointing out that stating 99% of Fanuc controls use tool lengths set in one particular method is incorrect.

Vancbiker said:

I know the OP was not asking about preset tools. I was pointing out that stating 99% of Fanuc controls use tool lengths set in one particular method is incorrect.

Click to expand...

Please enlighten us on your technique in this situation using tool offsets to a set plane and work offsets to compensate from set plane to the part Z0 datum of the part. I am more than willing to learn. Maybe I'll even change the way I have been doing it. Thanks

Sent from my SM-G960U using Tapatalk