Fadal Tool Offset - external Tool setter

[MatGermany]

Hello,

I have a question about Tool Offsets in my new to me fadal vmc15xt

Im using a Tool length measuring jig to measure the length of my Tools Outside of the maschine.

Do i have to Put the values positive or negative into the Tool Offset Table?

I tried both but it doesnt really Work. If i Put it negative then the Tools are much to far in -z after Tool Change. If i Put them positive then the Tools are to much in +z.

 

[RC Mech]

More information about the exact process you're using would be helpful. List the steps in your procedure and I'm sure someone familiar w/Fadals will be able to spot the error.

 

[angelw]

Hello,

I have a question about Tool Offsets in my new to me fadal vmc15xt

Im using a Tool length measuring jig to measure the length of my Tools Outside of the maschine.

Do i have to Put the values positive or negative into the Tool Offset Table?

I tried both but it doesnt really Work. If i Put it negative then the Tools are much to far in -z after Tool Change. If i Put them positive then the Tools are to much in +z.

It depends on the reference plane being used. Although any method can be used when using an external device (with some math applied), the easiest method is to use the gauge line of the Tool Holder Taper as the reference. On the machine, the Gauge Line will be the face of the Spindle Nose and on the External Device, the face of the Inverted copy of the Spindle Nose, into which you locate the tool being measured (presuming this is the type of External Device set up you have).

In this case, all Tool Length Offsets will be entered as positive values. However, for each job you set up on the machine, a Work-shift Offset has to be set in "Z" and obviously X and Y, but in Z to accommodate the Tool Length Offsets registered.

The Z Work-shift Offset will be the distance, in a negative direction, from the Face of the Spindle Nose, to the Z Zero of the new Work-piece. This can be obtained by touching the tip of any tool that has its Tool Length Offset registered, on the Z Zero surface of the Work-piece, then adding the registered Tool Length Offset for that tool to the distance value the Z Axis is down from the Reference Return Position (Machine Coordinate Zero). The Z Machine Position Displayed will be a negative value and the registered Tool Length Offset a positive value. Use the Absolute Value (positive value) of the Z Machine Coordinate, add the positive value of the registered Tool Length and then register the result as a Negative Value for the Z Work-shift.

When touching the tip of the tool on the Work-piece Z Zero, if there is a machining allowance between the surface the tool is touched off on and the Work-piece Z Zero, then this value has to be added to the Work-shift value being obtained.

Regards,

Bill

 

[Bobw]

WHY ARE YOU MAKING SOMETHING SO SIMPLE MORE DIFFICULT THAN IT HAS TO BE??

Seriously. There is an awesome little utility in the control, and you aren't typing
in a ton of numbers...

Offsets can be difficult to wrap your head around. The hardest thing being positives
and negatives.. Once you understand the directions and what each offset actually
means, it gets a lot easier.

So, you are just typing in a length in your offsets.. Is that all you are doing?
How are you telling the machine where the part is? Are you doing that in your
fixture offset?

First off, the machine doesn't care how long the tool is.. I mean it does, but telling
the machine the length of the tool doesn't help it. Your total Z offset should add up
to the distance from the tip of the tool to the Z zero of your part( total will be negative,
since its DOWN). You could measure this with a tape measure as a way to visualize
it easily.

You have a tool length offset, and you can run with just that and
a zero in your fixture offset. You can also set to a known Z point,
the table, top of the vise, whatever you want, and then put the distance from
that set point to your parts Z zero.. Those 2 numbers will add up to the
distance from the tool tip at the machine zero to the parts Z zero..

Now please tell me that you aren't using SETZ ever, at all.. Please tell
me you typed SETZ ONCE, when you first cold started the machine,
and then you've never typed it again.. Because now we are adding in a
3rd # which throws everything off, and usually results in crashes...

If you really want to find #'s offline. Lets use the gage line.. Length of tool
from the gage line, goes into the tool offset as positive, since it is from the
tool tip, heading UP (when the tool is in the machine).. Then you need to
get the length from the gage line to the Z zero you want on your part or
fixture(and put that in your fixture offset).. And that is negative because it is down..
Now those 2 #'s should add (one positive, one negative) to the total length from your
tool tip to the Z zero on your part..

Now of course, finding the length from the gage line to your Z zero is not an easy
task since its based on a taper.. So now, we need to use a reference tool that sits in
that taper.. So now we are playing with ANOTHER #, and we need to add that
number into our Z fixture offset..

.. Or.... we use that same reference tool as our Zero on our presetter.. But now
we have another complication, now our tool lengths can potentially be both positive
and negative based on the length of the reference.. One more thing to keep track
of.

It can get stupidly complicated, and there are about 50,000 ways to do it, and
none of them are wrong.

I'm a big fan of the KISS principal myself..

Boiled down.. Your Z#s just need to add up to the distance from your tool tip,
DOWN... NEGATIVE to the Zzero on your part.. When the Z is at the machine Zzero.

There are a lot of different ways to get there.

 

[TheOldCar]

WHY ARE YOU MAKING SOMETHING SO SIMPLE MORE DIFFICULT THAN IT HAS TO BE??

Seriously. There is an awesome little utility in the control, and you aren't typing
in a ton of numbers...

Offsets can be difficult to wrap your head around. The hardest thing being positives
and negatives.. Once you understand the directions and what each offset actually
means, it gets a lot easier.

So, you are just typing in a length in your offsets.. Is that all you are doing?
How are you telling the machine where the part is? Are you doing that in your
fixture offset?

First off, the machine doesn't care how long the tool is.. I mean it does, but telling
the machine the length of the tool doesn't help it. Your total Z offset should add up
to the distance from the tip of the tool to the Z zero of your part( total will be negative,
since its DOWN). You could measure this with a tape measure as a way to visualize
it easily.

You have a tool length offset, and you can run with just that and
a zero in your fixture offset. You can also set to a known Z point,
the table, top of the vise, whatever you want, and then put the distance from
that set point to your parts Z zero.. Those 2 numbers will add up to the
distance from the tool tip at the machine zero to the parts Z zero..

Now please tell me that you aren't using SETZ ever, at all.. Please tell
me you typed SETZ ONCE, when you first cold started the machine,
and then you've never typed it again.. Because now we are adding in a
3rd # which throws everything off, and usually results in crashes...

If you really want to find #'s offline. Lets use the gage line.. Length of tool
from the gage line, goes into the tool offset as positive, since it is from the
tool tip, heading UP (when the tool is in the machine).. Then you need to
get the length from the gage line to the Z zero you want on your part or
fixture(and put that in your fixture offset).. And that is negative because it is down..
Now those 2 #'s should add (one positive, one negative) to the total length from your
tool tip to the Z zero on your part..

Now of course, finding the length from the gage line to your Z zero is not an easy
task since its based on a taper.. So now, we need to use a reference tool that sits in
that taper.. So now we are playing with ANOTHER #, and we need to add that
number into our Z fixture offset..

.. Or.... we use that same reference tool as our Zero on our presetter.. But now
we have another complication, now our tool lengths can potentially be both positive
and negative based on the length of the reference.. One more thing to keep track
of.

It can get stupidly complicated, and there are about 50,000 ways to do it, and
none of them are wrong.

I'm a big fan of the KISS principal myself..

Boiled down.. Your Z#s just need to add up to the distance from your tool tip,
DOWN... NEGATIVE to the Zzero on your part.. When the Z is at the machine Zzero.

There are a lot of different ways to get there.

In case the OP or anyone asking these questions feels even .000001% embarrassed, don't be. This explanation made all the difference for me. Thanks Bobw.

 

[MatGermany]

It depends on the reference plane being used. Although any method can be used when using an external device (with some math applied), the easiest method is to use the gauge line of the Tool Holder Taper as the reference. On the machine, the Gauge Line will be the face of the Spindle Nose and on the External Device, the face of the Inverted copy of the Spindle Nose, into which you locate the tool being measured (presuming this is the type of External Device set up you have).

In this case, all Tool Length Offsets will be entered as positive values. However, for each job you set up on the machine, a Work-shift Offset has to be set in "Z" and obviously X and Y, but in Z to accommodate the Tool Length Offsets registered.

The Z Work-shift Offset will be the distance, in a negative direction, from the Face of the Spindle Nose, to the Z Zero of the new Work-piece. This can be obtained by touching the tip of any tool that has its Tool Length Offset registered, on the Z Zero surface of the Work-piece, then adding the registered Tool Length Offset for that tool to the distance value the Z Axis is down from the Reference Return Position (Machine Coordinate Zero). The Z Machine Position Displayed will be a negative value and the registered Tool Length Offset a positive value. Use the Absolute Value (positive value) of the Z Machine Coordinate, add the positive value of the registered Tool Length and then register the result as a Negative Value for the Z Work-shift.

When touching the tip of the tool on the Work-piece Z Zero, if there is a machining allowance between the surface the tool is touched off on and the Work-piece Z Zero, then this value has to be added to the Work-shift value being obtained.

Regards,

Bill

Thanks a Lot. This Works perfekt.

 

[Cole2534]

I just wish my post processor would kick out the fixture offset on the same line as the H callout.