Using a static drill on a lathe

Al_V · 2005-01-27 22:47:51

When you set up a static drill in the turret and take it to the centerline (X0), lathe spindle running, then feed Z into the part to drill a hole in the center of part, should this tool defined as a lathe tool, or a mill tool?

BillH · 2005-01-28 21:29:22

Hi Al,
Good question. There are 2 kinds of tools: Rotaionally symmetric (aka "mill tools") and insert tools (aka "turn tools"). Over time VERICUT has changed to allow inserts to be used in a mill tool (we just spin them about the tool's Z axis behind the scenes). You can also use a mill tool in a turning operation, as long as the tool aligns with the turning centerline. The "turning centerline" is the stock's Z-axis.

So this is a long-winded way to say, either will work. The behavior is slightly different when using a turn tool vs. a mill tool to do a lathe drilling operation.

For a turn tool:
The tool image will be an insert (swept 2D profile).
The tool must reside in a valid turning plane (i.e. any plane that contains the stock's Z axis).
You must be in turning mode for material to be removed.

For a mill tool:
The tool image will be a revolved tool (revolved 2D profile).
The tool Z axis must be coincident with the stock Z axis.
If in turning mode the tool will do a turning operation. An error will be reported if the tool z-axis is not coincident with the stock z-axis.
If in milling mode the tool will do a milling/drill material removal, regardless of whether it aligns with the turning axis or not.
If in milling mode and you check setup > motion > check for spindle off, and the milling spindle is off, you'll get an error for any material removal with this tool.

We're changing this logic a bit for VERICUT 6.0, and not really differentiating between milling and turning tools. VERICUT will check the status of the machine and the cut you're trying to do and report an error if it is not allowed (such as milling with the spindle off, or turning with a milling tool with the milling spindle on, etc.).

Sorry for such a long answer to a seemingly simple question.

Al_V · 2005-01-29 04:01:41

Thanks Bill,
I am using an indexable type drill to first drill, and then rough bore the part with the outer insert. So, I defined it as a lathe tool (swept), with a cylindrical holder behind it.

It works OK, but the tool looks like a spade drill in the simulation, I guess I could shorten up the Z length of the cutter.

Is there some tolerance for the tool axis to be coincident with the stock axis? On a machine with a tilted turret and gage lengths and work offsets there could be some rounding error.

I have a machine with a 15 degree tapered turret that is tilted at 15 degrees so that the turret face of the tool indexed to the spindle is perpendicular to the spindle, but all the other faces are not.

BillH · 2005-01-31 16:43:47

Hi Al,
Since you're using the tool as both a drill and a boring bar, the way you did it is the way to go.

Yes, there is a tolerance associated with the check for "on center" lathe drilling when using a rotationally symmetric tool (aka milling tool). I don't know the exact value, but typically these kind of checks are small (1.0e-5 or 6 order of magnitude).

There is a similar check to make sure the insert is in a valid turning plane (i.e. a plane that contains the Z-axis of the stock) when in turning mode.

VERICUT uses double-precision floating-point numbers in all its calculations. This gives us something like 17 significant decimal digits. In the "real world" (not the simulation world) things are rarely that precise, so VERICUT has to be tolerant of the physical data vs. calculated values.

Hope this helps,
Bill

VERICUT Users' Forum

#1 2005-01-27 22:47:51

Using a static drill on a lathe

#2 2005-01-28 21:29:22

Re: Using a static drill on a lathe

#3 2005-01-29 04:01:41

Re: Using a static drill on a lathe

#4 2005-01-31 16:43:47

Re: Using a static drill on a lathe

Board footer