U100L lathe zero measuring the material

Since I have my lathe with a U100L, I always set the Z zero with a master tool (z offset = 0), press CAL on the zero offset line, and that is it. Easy.
All all my other tools have their offset in relation to that tool/the face produced with that tool.

Now, I will probably sell this lathe, and the client told me that they work measuring the length of the material from the chuck up to the material end. Client does not want to change the way they work, so I am trying to reach a practical solution for this.

I have try to make some changes on the "zero menu" but none seams to work out correctly. In fact I was quite close setting a zero point that was indeed on the start of my chuck, then the measured entered in the "zero shift". This seamed to work out, but as soon I was in "MEM mode" to run the program, the value inputted on the zero shift went back to zero.

Thank you

makes point. because any negative coordinate means the work inside the chuck.
the zero shift is actual until reset or similar action - that it's intention is. If you want to keep your zero offset, use zero offset then.

place zeroshift in program VZSHZ=30 shifts your Z-zeropoint by 30mm (or inch)

Why not do it the same way you are doing it now, but instead of calculating 0 on zero offset page, calculate material length. Standard programming from Japan always shows from the chuck out, not face of the part. In fact when using IGF you had to add the PZ shift of the part length to get zero at the face.

Underthetire is correct. If you have a part 3 inches long from the chucking face then just CAL 3 on your zero set page with your zero tool in position at the front of the part. Avoid using zero shift since it is temporary and will disappear if switching to manual or pressing reset.

Best regards,

Quote:

---

Originally Posted by OkumaWiz

Underthetire is correct. If you have a part 3 inches long from the chucking face then just CAL 3 on your zero set page with your zero tool in position at the front of the part. Avoid using zero shift since it is temporary and will disappear if switching to manual or pressing reset.

Best regards,

---

Using this method I am saying that the part is 3 inches up to where my tool is (in Z); this is it depends on the actual tool position, and therefor not suitable.
Or am I missing something obvious?

Quote:

---

it depends on the actual tool position

---

Yes, the CALculate function uses "Zerro tool" or actual tool position for calculating the coordinate of the work point

Quote:

---

and therefor not suitable

---

Why?

Because my client is used to measure from the chuck to the end of the part.
He places a tape measure from the chuck into the end of the material.

Using the Calc button, the method would be measuring from the end of the material up to the tool.

Please understand that I am only trying to see if it is possible that my client continue to use the same measuring method as in another machine that he is more used to, and therefor does not need to learn another way of doing the same thing.

Quote:

---

Using the Calc button, the method would be measuring from the end of the material up to the tool

---

No. Calculation method is not related to "the end of the material" or something else. You place Your "Zero tool" at any desired point and do Calculate any coordinate according drawing or other requirements. You can use a real tool (MID manual mode only) as well if You need high accuracy of work setting.

You are not understanding the function of CAL.
Just to make a simpler explanation, the CAL function tells the machine where the zero position is in relation to where the turret sits now at the current time. It does not have to be 0 but it must be a known position.
Where ever you put the tool and do a CAL 0 is where the ZERO is set. It can be the face of the part, the face of the jaws or any other position. If you put the tool on the moon and CAL 0 WRITE it will think the moon is zero. But you are not limited to CAL 0. You can do a CAL 123.456 WRITE or CAL -999.999 WRITE.
But in all cases you must position the setting tool at a known position so the calculation is correct.

The easiest way to set a zero at the back of the jaws is to measure the depth of the step you have bored in the chuck jaws and use the face of the jaws as the touch point.
So if your chuck jaws have a 1" step you touch the jaw face with your setting tool and do a CAL 1.0 WRITE and it will then know your zero position is at the back of the step on the jaws.

In my opinion setting at the back is not accurate because the part may not actually touch the back face of the jaws if the operator does not hammer it back or mis-locates it. The better way is to take a small skim off the face and set the zero on that face and have all Z positions negative. That is the industry standard way of programming, regardless of what the Japanese or any other person does. Your client needs to get with it and do things the right way. But whatever.

Thank you,

I believe that I understood from the start what the CALC does. It does the calculation in relation to the turret/tool.
However the desired method is to measure the material that is placed on the chuck and enter that value (where, I do not know, not even sure if possible), independently of the turret position.
It would be informing the machine that: You now have a piece of 3" length that is available for machining. If the turret is near the top of the material or the turret is on its more positive position it does not matter.
In other machines is like changing the current work coordinate (for example G54 in Z value).

Please take in mind that I always worked as described:

Quote:

---

Originally Posted by fordav11

In my opinion setting at the back is not accurate because the part may not actually touch the back face of the jaws if the operator does not hammer it back or mis-locates it. The better way is to take a small skim off the face and set the zero on that face and have all Z positions negative.

---

But my client is used to work as I described before, and I was trying to reach some similar way for him to work.
I hope that I was clear enough.

Quote:

---

Originally Posted by fomaz

It would be informing the machine that: You now have a piece of 3" length that is available for machining..

---

I think the only way is to place "VZSHZ=3" in one of the first lines of the program OR place "VZSHZ=V1" in one of the first lines of every program and input the zero shift amount from the chuck to the face in "user variable" or "common Variable" (dont know the preciese name of the page) nr 1 (if nr 1 is used for something else use another nr).
If your client gets used to programming the VZSHZ=V1 in every program the only thing to input is variable one, only problem is then that this zero shift amount isn't automaticly entered in MDI mode.You would have to (I think) manualy typt VZSHZ=V1 before any other MDI command

Sounds like your client doesnt want an okuma. Thats how the OSP control works, trying to go about it any other way is just overcomplicating what your machine does. Just offer to go in and teach all the ops how to use CALCULATE.

Already did and he did not liked it...
For me it is just perfect. Place a zero then calc. Simple, done, no mistakes.
He prefers a tape measure. Well not possible then. At least I asked.
Thank you all.

Quote:

---

not possible then

---

it is possible. it's described already. take the measurements, a big calculator, write down your results and put it in the variable VZOFZ for Z offset for instalce. Put the line "VZOFZ =987,654" in the part program and that's all.

Ok, Thank you, not possible without editing the program/ not suitable/ not easy for the client.
It is much better that he learn to place the "master tool" near the material and then calc 0.