First and foremost is setting the Turret change position. The 2100 uses M6.1 for tool change at set change position. DO NOT use M6! M6 is change in place.
Setting change position
- Rotate turret using the membrane keypad to the longest tool.
- Jog the Z axis to a minimum safe change distance.
- jog up in X then rotate to the longest protrusion in X
- Jox longest X tool to minimum change distance (Z should still be at same location you picked clearance).
- ON the Membrane pad scroll to "Set Tool Change Position"
- Press "Set"
Done, Now all you need is an M6.1 and the turret will always move to the set position. There is a lot more customisable tool changing for faster cycles but leave that alone till you get used to the 2100.
Setting tools, Generally is the same as most other machines except the graphics page. It's a good idea to get into the habit of labeling and using the tool type since the control takes into account this stuff even when you don't want it to. Hole making in general. Set your drill point angle to 180 degrees. The 2100 takes the hole making cycle to an all new level. say you set the point for 120 degrees and use a G83 and tell the Z depth to be 2.000. The control thinks you want the usable hole to be 2.0 so it will factor in the tip angle and go deeper than the programmed value. This is the same for OD/ID work tools. Make sure you define the tool direction and the tip radius. R.A.P. generated programs all use this info.
Setting the tools.
- Start the spindle just the same as Fanuc.
- Rotate to the tool you want to set.
- On the touch screen press tool offsets (It should automatically go to the tool that's current in position.
- make a facing cut and press "Set Z" (If this is all new tools then the Z must stay common for all tools)
- make you X cut and set the same way.
- Repeat for all tools
Setting work offset Z
- rotate manually or call in MDI and the control activates the tool offset
- Touch off in Z
- Go to the work offset page
- press "Set Z".
- Done
2100 lathe programs generally don't use work offset calls or tool offset calls unless your getting complicated and adding more than 12 tools. If you see an "H" code in the program make sure it is "H1". The 2100 does not use G54. It has 999 work offset, 999 fixture offset, and 999 pallet offsets. so it uses H1-H999.
For me that is still the finest control ever made. It will piss you off in the beginning but once you come full circle with it and see all the features you will love it.
Tapping is where it shines. In a G84 cycle all your Pots still work as well as feed hold. And the tapping code rather than figuring the feed you just set as 1/pitch
Say you are tapping 1/4-20, simply F1/20 for the code.