I'm "storing" a CNC lathe for a friend for a few months, and just to make sure that it stays in top shape, I'm going to make sure that it still works from time to time .
Anyway, the work that I'll be doing with it will be essentially prototyping. I rarely need more than 10 of any given part.
The lathe has an 8 position turret and the possibility of some gang tooling, but it still seems to me that I'll be changing out tools fairly often. I've been trying to decide the best way to set up the tool and work offsets.
In the mill I have a "master tool" (a 3D indicator) and all of the lengths are relative to that tool. That seems to work best for me there. I just zero with the indicator and all of the other tools in the changer are ready to go.
The lathe seems like a different situation. Having a master tool doesn't seem like as good an idea here. It seems like I should make all of the tool lenght offsets relative to the chuck? I could always program relative to the chuck as well. My G54 offset would almost always be zero for Z with that method, I suppose.
For the X axis offsets, should I always determine an offset for the tool relative to the centerline of the chuck? This seems time consuming, but maybe I could get to be fast at it. I've also thought about using G54 to get me to the centerline of the chuck. That way straight tools in the turret could be setup with a zero X offset.
Other than acquiring a tool probe for the lathe, what can I do to make changing tools and setting offsets go as quickly and acurately as possible?
If you are new to CNC turning, I'd recommend getting your feet wet with the turret instead of the gang tooling. Gang can be faster for big runs of small parts, but it presents some extra complexity when programming.
Without knowing the make of control, etc, I can only generalize a bit.
The controller knows a few things and does all of the math behind the scenes. It knows the amount of travel, the turret home locations.
You tell it your stock location, and tools relative to that piece of stock.
Put a 1" diam x 6" long rod in the chuck and let some of it hang out.
Make a facing cut with tool T1.
Tell the controller that the part face is located at Z0 (note that the stock face can be anywhere within usable travel of the machine)
Now tell the controller that T1 is at Z0. This zeros the Z position of the tool.
[Note that if you move & rezero the stock, the tool zero will be equal to the zero of the stock]
Take a light OD skim cut with T1 and mike it, 0.934 for example.
Go back and set the X offset for T1. Your controller may do this a couple of ways, but it may be as easy as entering in the current position (your just measured diameter). *note you may need to enter this value as a radius depending on the control. I prefer diam programming, but to each their own.
Bring the turret clear of the work and call T2.
Touch T2 to the end face of the stock and set it's Z offset to 0 at that position.
Bring it around and touch the OD, skim cut if necessary, and enter the X offset.
Repeat as necessary.
Take the 1"diam setup bar out of the lathe and put in one of your part blanks.
Call up a tool and touch the blank's face. Now tell the control that you are using T1 and have located it to the part's Z0 (or whatever Z you want). Note that this is a PART ZERO not a tool zero.
Now, all of your tools will have their X0Z0 at the end face & center of the stock blank.
Only need to set the tools once- then when you have a workpiece change, reset the Z zero.
One word of caution though. On some controls there are multiple screens of offsets. Typically one page will be for primary offsets, measured in multiple inches. The other page will be wear offsets in thousanths. The idea is when you set a tool and are running parts, as the cutting edge wears, you can bump up the wear offsets to dial in dimensions. BE SURE THAT the wear offsets are set to zero when touching off tools (otherwise you'll go nuts chasing that .005" error!!!)
For a 2 axis lathe, always set your X=0 to equal the centerline. It's troublesome and dangerous to program any other way.
Hope this helped some. it's not bad at all once you get going. Just measure all the tools to the same reference point (setup bar) and you can't go wrong.
I concur with Damon's suggestions above. If you'd like to try, a slightly different (yet similar) method can be used where the face of the turret is imagined to be doing the cutting. The tool offsets are the distances away from the turret face in the X and Z directions, in other words, something like would be done for a machining center. Remember that if a tool were to stick out 1.25" from the turret in the X direction, the X offset would be 2.5" if you are programming using diameter. The Z value is read directly. Using either this setup or Damon's, you can re-use your offsets for multiple jobs, effectively changing only the Z axis PART zero location. X zero should always be on the spindle centerline as he has mentioned.
Thanks for the input guys!
So Damon's response is what I would call a "master tool" method. You are setting your work offset based on the facing cut of a chosen tool. All the other Z tool offsets are then relative to that master tool. The only drawback that I can see with this strategy is that if I need to replace the master tool in the turret then all of the other tool offsets are invalid.
If I make a good choice for the "master tool" in this case, then perhaps I'll rarely need to take that tool out. I can easily see this being the fastest and most accurate method of setting the Z offset, but I'm still open to any other suggestions.
I also like Jim's method of setting the tool offsets relative to the turret face. How do you acurately measure these offstets? Obviously you could very quickly setup a drill where the depth of the hole was non critical.
Certainly X=0 needs to be the centerline of the part, but I guess that my question is about how to get it there. One way is to make the part offset (G54, etc) have X=0 on the centerline for some part of the machine, like Jim's edge of the turret above. The other way is to just set all of the tool offsets relative to the home position to put them on the center, leaving the part(work,G54, etc) offset = 0.
This is a Mitsubishi control, if it makes any difference.
Instead of my method as master tool, think of it as "master workpiece".
But then you can just change your workpiece settings (Z-end face, basically) and all the tools will follow it. You can use any stock for it, no problem. The key here is that all tools are set to the same point.
For the X=0 thingie, G54X should always be 0. Have your X set properly in the tool offset. I think it would be really frustrating (and potentailly scrap-laden!) to require a G54 shift every time you called up a different tool!
damonfg said the governing word. "master workpiece". Once you've set your tools to the "master workpiece", ALL!!! your tools are now master tools!!! IOW if you don't change any of them, then you can use any of them to pick up our next job and it's Z0.
So let's say you got your tools picked up and ran the first set of parts. Your G54 Z is probably 0 at this point. Now that you're done and ready to machine your next part. It however needs a 1/2" drill instead of the 3/8 from the previous part.
So, you put the new drill into the turret and the new part into the chuck.
You take ANY!!! of your unchanged tools, jog to the part and make a facing cut. You now tell the controller that this point with this tool is the new Z0. Remember that the controller knows what this tool and it's offsets are, so it will change the G54 Z0 to some number. This number is actually now representing the distance from the previous parts Z0 and the new one.
You now take the newly installed 1/2" drill, jog to the face you've just cut and zeroed, touch the tip and tell the control that this tool is now at the current, new Z face. The control now records the distance from machine home to this point, deducts the Z value in the G54 offset and enters it into the tools Z geometry offset page.
Done. You now actually set this tool to be another "master tool".
These examples assume no toolsetter!!!
How is this differenmt than the VMC. Well somewhat similar with the small addition of "floating" fixed point. Sounds stupid but that's actually quite accurate. On the mill the height probe is fixed point, always in the same Z position.
On the lathe you first create this fixed point when the ALL THE TOOLS are first picked up, and then you float (move) the fixed Z position of the "probe point" by first re-cutting it with a known tool, and then tell the control that this is now the new "fixed probe point"
I perty much only read the original post - so excuse any repetition...
I use the chuck (collet?) face as zero with your G54 also set as 0. (G54 on my machines is G10 - but I think we're all on the same page here...)
This way you just set your G54 line to how far from chuck face you want "zero".
Think Snow Eh!
Some machines also have a "geometry" offset for the gross amount to calibrate the tool then they have a "wear" section where you make small adjustments...this is very handy.
Almost every turning job will use an 80 degree diamond or trigon turning tool first....not EVERY job, but a whole lot of them . I think you will find yourself leaving most of your OD tools in the turret most of the time...80 degree turning, pointier turning, threading, and cutoff tools about cover the deal 90% of the time.