Republic lagun vmc4824 Tool offsets and part zero procedures.

I have a new (to me) machine with a delta 50 controller. I have basic navagation of the machine screens down and have successfully loaded a program that I made with a cam software and posted,but, thats about it.

Does anyone have a source for basic instruction on:

1)How to set part zero.
2)How to use the manual "spindle on" to edge find a part.
3)How to set tool length/height offsets.

I have the manuals but cannot for the life of me find the info im needing. (Im honestly wondering if they were removed.)

Can anyone help me with these basic program steps or have a source for them? Youtube is empty and finding threads with this basic info has been unsuccsessful.

Even simple keystroke order to get me pounted in the right direction would be helpful. Im a pretty quick study but this controller is far different than i have ever used.

I would be ever so grateful!!!
Thank you for any help!!!

Hi WTFab,

I don't have a tool changer on my machine but suspect this should get you going (assumes machine referenced to home, no probing package and use of a master tool).

Part zero: Mode select, select jog (0) on the main menu, select speed for axis switches or increment for MPG, bring master tool into contact with part on the axis being zeroed, mode select, select tool tables (6), (E), then select which offset you want to use, the axis and set your zero. If your tool is offset from the actual zero location, reselect the axis and enter the incremental difference (incr key) and either positive or negative offset. Repeat for all remaining axes.

Spindle on: not sure for your machine, probably use MDI and enter spindle speed Sxxx and M03 (M05 to stop) but that is just a guess.

Tool length: Jog mode, bring master tool into contact with your reference height, set zero (9) + z axis switch, home z, change tool, bring into contact with reference height, mode select, select tool tables (6), H, select tool number and zero tool. Repeat for other tools, when finished reference Z to home again to cancel temporary zero set.

This is from memory so I may have missed a step but this should get you started (I don't even think about it anymore, it's all muscle memory now).

RT

RT has it right, except going from memory I believe E is for fixture offsets and T is for tool offsets. I approach mine a bit differently. I use a tool length indicator. Starting with my longest tool I set Z to at least -.100 to allow for clearance plane. Then I bring the indicator into contact and set it to 0. Lets assume this is tool #1. Then I go to mode select 6 (offsets), T (tool), make sure I have tool #1 selected and push the calibrate button and it sets the z length offset. Then I enter the diameter info as required. For the remaining tools I will jog the tool tip until the indicator reads zero, return to offset page and push the calibrate button.

Now when I run a job, I program a z0 move on any tool (using the correct offset), then bring the work Z0 up to touch the tool. Now all my tools are set to the work surface Z0.

For setting part zero, I make my set up, use edge finders or whatever to locate the spindle centerline to my desired X0Y0, then I go to mode 6 offsets, E (fixtures) and enter the XY data in the desired offset. Be sure to call the correct offset in the program!

Another common question with the Delta control is MDI mode. There isn't one that's labeled. MDI is performed in mode 3. Option 1: in any part program, type "N." enter (that's "N" then "."). This opens a "temporary program line. Type whatever commend you wish like Mode 9, M3, S2500, then push cycle start. repeat continuously typing whatever you need. Drawback - if you are using an active program and forget to type N. then you just changed the program!

Option 2, Create an MDI program in the catalog, then select this program when you want to MDI. Follow the steps above (although it will work with any N number) and press cycle start after each command. This way you are not changing a part program by accident.