Setting G54 Z Zero and Tool offsets accordingly
thank you for your time and assistance in this matter. I Have been asked to setup and run an older VF-2. Noone in the facility can tell me to what Gage/height block the tools were previously setup to. My question is , is there a parameter that I can look at to find this information. If not, then how would you setup the tools/ work offset. thank you again for your replies.
Are you taking tool data from a printed record or from an external tool setter? Are the length offsets included in your programs (in G10 commands)? If the answer is no, then choose your own reference plane and start measuring as you like. The G54 Z0 is simply the difference between the height of your reference plane and the Z0 of the workpiece.
Tough Hu's post is correct, you must first determine how the machine is set up.
In settings, you have a field called: "Tool Offset Measur Uses Work"
If it is:
ON, then you must set your tools to the Z0 of your part, typically the top. IOW each and every tool has to be picked up to the Z0 of your fixture, AND your G54 offset must be zero ( without complicating the post ...)
OFF, then you can pick any solid and stable reference point to measure each and every tool to this point. This can be the top of your stationary jaw, the table with a 2" gageblock or anything.
After this you just measure the distance from the top of your fixed reference point to the Z0 of your part - which might be anywhere, even on the bottom or middle of it, enter that value
in the Z-field of your active workoffset and you go.
Now, if I'm guessing correctly, you're trying to find out where the tools were picked up to by the previous person.
The simplest answer would be to move the X/Y to a safe place, clear the Z-field in the G54 workoffset and type in MDI:
G00 G43 H01
Observe where the tool is and try to make sense of what they might have used, knowing that you're now 1" above what that might have been.
when setting off of a block I have my operators go to the position page, scroll to (operator) then as the last tool is still on your block have them zero out the Z axis line. After that just touch that same tool off of the top of Z of each fixture and key in the data as it is on the operators Z axis line to the apropriate g54,g55,ect (note after puting a value in use F1 not input).
I've had issues setting up my vf1.. And I prefer setting off a reference plane as well. I'm a big fan of letting the machine to the math for me.. First off i set all my tools off the top of the two inch side of a one two three block on solid end of the vise body, using the tool setting functions to set the tool height. on the last tool, i'll cursor to highlight that z-offset, push F4 "copy" then i take that tool and touch off the top of the part, and push part zero. push F3 "paste" this puts that last tool height in the register, then push write.. this subtracts the tool height from the part zero height thus letting the machine do the math for you.. "it's been awhile since i've done it so i hope i've got the f3 and f4 right as far as copy and paste goes".. this'll put your G5X Z0.0 where you touched off and may need to adjust for excess stock..
To my simple mind you need to...
Originally Posted by thesePAPERwalls
press the OFFSET key, use cursor PAGE key to change to tool offset/work position pages.
What I would do is while on the tool offset page, press ORIGIN, control will ask clear offsets yes/no, press y to clear all off sets. Now you can proceed to load tools and set offsets using whatever Gage/height block you wish, make sure the tool number is highlighted, press TOOL OFFSET MEASURE button, NEXT TOOL, repeat...
Agreed! Better to start from scratch than to guess at a bunch of unknowns.
Originally Posted by BGL