Denford Software & Machines

Hello All,

Is the [BILLET X Z used for Fanuc simulation only or does it also have an effect on live turning?
When using ATC do the tool offsets only need to be entered once?
For example if I have a different length and widths of stock will the system calculate the end of stock and centre line zero or does it require to edit the tool offsets for each billet size?
The reason I ask is that I am using UG-NX to create a toolpath geometry (gcode) and am having a little dificulty in setting the tool start points etc.

Kind Regards,
SRG

Is the [BILLET X Z used for Fanuc simulation only or does it also have an effect on live turning?

In my experience of the later software, this command only effects simulation and has no effect on machining / offsets. I would expect it's the same in earlier software.

When using an ATC the tool offsets should be set once to a known position (eg the front face and centre-line of the chuck)
Then a work offset can be applied to shift all those tools to the front of the billet (ie Z+Billet Length)
Output from a lathe CAM system will vary but you should be able to configure it to so that X0,Z0 is the front, centre of the billet, X +ve values are diameter positions, Z -ve values go into the work (towards the chuck)

HTH

Thanks your reply Admin.

It makes sense ofsetting from the chuck as you sugest I will give this ago.

I followed the tool setting intructions found in the Denford documentation which states to use the end and side of the billet to set offsets. I have attached an OCR scanned pdf of the procedure in case any one is interested.

I managed to cut a ballhandle which came out ok'ish for a first effert apart from the screwcutting operation the post processor out put G33 X Z I K and the cutoff opp Picture attached.

Kind Regards,
SRG

use the end and side of the billet to set offsets.

Looking at the .pdf (thanks) it tells you to enter the measured diameter.
That's looks like the normal procedure for most lathes:
Turn something down a little bit (don't take a big cut as push-off will effect the reading),
Move away in Z only - keeping X at the diameter just turned,
Stop the spindle and measure the turned diameter accurately,
Enter this number into the current offset (whichever you are setting - work or tool)

This measured number is taken into account whenever the CNC wants to know where X0.0 is (ie, the chuck centreline)
That's because the X numbers output from CAM systems are (usually) diameters, so when you move tool 1 to X25.4 then it should be 12.7 away from centre and cut a 1" diameter