[hiatec]

Hello everybody,
I just started working with an OKUMA Crown Lathe with a OSP700L control. I am working in establishing the tool offsets following the instructions found in this site: http://www.countyhistory.com/rbcreations/ron/ref.html. Everything works fine for the roughing and finishing tools; but when I try to set up the drills I always end with an offset of about 2 inches from X-axis. Can anybody describe for me a different procedure to set-up the tools?

Thank you very much for your cooperation.

[phx]

Hello everybody,
I just started working with an OKUMA Crown Lathe with a OSP700L control. I am working in establishing the tool offsets following the instructions found in this site: http://www.countyhistory.com/rbcreations/ron/ref.html. Everything works fine for the roughing and finishing tools; but when I try to set up the drills I always end with an offset of about 2 inches from X-axis. Can anybody describe for me a different procedure to set-up the tools?

Thank you very much for your cooperation.

hi
drills(not driven) have the offset in X=0

[broby]

Make sure your "Machine" Zero for X axis is set to centreline of your toolholder first!
Then all drills have an X axis offset of "0"
All other tools are "offset" from the centreline of the tool holder.
I teach the following method of tool qualification and find that it works a treat!
1. With the tool clamped in the turret, move the tool to take a cut.
2. BEFORE you cut the job, bring up your tool data page, select the X axis offset for the current tool and press the "Calculate" button, followed by the "Write" button. Ignore the offset that is calculated at this stage!
This will calculate the tool offset as though it is at X0 where ever the tool is located.
3. Turn a diameter long enough for you to measure.
4. You can move the tool on X away from the job at the end of the cut now.
5. Stop the spindle and measure the diameter.
6. Go to your tool data page and with the tool selected ADD the negative amount of the diameter you just measured to the X axis offset. The resulting "Offset" is the number you need!

E.G. if you are turning the OD of a part and the tool is positioned at the start of cut and the "Calculated" X offset is 115.32mm, turn the OD of your job and it is measured at 89.65mm, the tool offset will come up as 25.67mm! (115.32-89.65=25.67)
Now I may have some of the numbers wrong in my example as I am at home and obviously not in front of a machine to get real values... but try it, it is an easy method!
When qualifying boring bars and you want to make sure the boring bar does not "rub" on the ID, you cna manually wind in along Z in the -ve direction and then, while still winding the handwheel in the -ve direction flip the axis control to X axis and the tool will move away from the job easily. Measure the bore and subtract the size from your "0" offset and bingo the tool is set!

Measuring Z axis is very easy if you use a dial gauge with a flat end mounted.
Bring your Zero set tool upto the dial gauge, calculate Z0 for the position and then touch each tool upto the same "Zero" point on the dial gauge, calcuating each tool as Z0 as you go!
Using the dial gauge rather than "touching" the face of the job allows for any over-runs of the operator, resulting in gouges in the face!

Hope these suggestions help.
Regards
Brian.

[throttle_jockey]

Uh, that takes way too much time. Set an RPM that is safe in MDI. Go back to manual, turn on the spindle, take a cut on the diameter, weather it's OD or ID doesn't matter. After taking a skim cut on material, do not move turret in X direction. Measure the part, go to tool offset page, cursor down to appropriate tool, on appropriate axis, hit extend and hit calculate and type in the diameter and hit the write key. I.E. with an OD tool, say tool #1, I skim the part, stop the spindle and it measures 2.433. Go to tool offset page and put cursor on X axis of tool 1, hit extend, hit calculate, and type in the 2.433 value.
FOR DRILLS,
Jog the tool down to x zero, with no tool offsets called up. Put an indicator on the chuck or collet and sweep in the tool. If the tool is out in the "Y" direction, a direction you cannot compensate for, there are cams on the back of the ID tool holder that will give you about .015 of stroke to get the tool to come in. If you cannot get the drills to dial in your turret may be out of alignment.

[broby]

Too slow you reckon?
Well at least using the method I laid out, I do not have to leave the tool in contact with the job after cutting the part!
You advocate taking a cut and then stopping the spindle to measure the part before going to the tool data page, great way of stuffing your insert if you are unlucky! Especially if you are using a Cermet or Ceramic type of insert.
I have used this method (and trained quite a lot of others to use it) for years now, Much easier and quicker everyone agrees!

[throttle_jockey]

I apologize for the brevity of my last post, I made assumptions. CLEARLY you never stop the spindle with the tool in contact with the work piece.

[broby]

Well I would believe that stopping the spindle would be somewhat a pre-requisite before being able to measure the job! Either that or you are VERY quick at taking a measurement!
What I am referring to in my ealier post is the process where by you can turn a diameter and move the tool away from the surface of the part before stopping the spindle, thus not leaving the tool in contact with the part.
What is the slow point in my method that you do not like?