Purpose of Work Offsets

[stylinmike]

Bit of a noob CNC question here. If you have a two sided part, like the first couple operations of an AR lower, for instance, do work offsets serve any real purpose? The way I understand it, work offsets are used when you have multiple parts in multiple fixtures on the table at the same time. But if you are running one part in a vice and you have to flip the stock and re zero anyway, what purpose does multiple offsets serve? Why not just create two programs in mastercam with two different coordinate origins and rezero before running each one.

[j_blankenship]

If you're running one piece, then using multiple work offsets doesn't serve any real purpose. However if you even want to run 2 pieces, or volume production then you can run another 1st side piece without any extra work as well as the 2nd again with any extra work.

I rarely run one of anything, but when I do mold work I won't even use tool offsets - I'll just set Z zero using each tool and keep trucking (this is on a Milltronics where you can do that). I run several different parts on my Fadal that only use one tool, so I won't use a workshift for X or Y, and also no tool length offset for those parts - I just set the floating zero where the part origin is and the Z the same.

It all depends on what you're doing and how many as to how much effort you put into the set-up on the front end to save time on the back end.

Rgds,
John B

[stylinmike]

Just as I thought. So if you wanted to do 3 AR receivers at the same time, in 3 different vices, with the same gcode (other than changing the work offset line), then that would be where it would be beneficial? So the process (in mach 3) would be to select your first work offset in the software, zero it out on your first work piece, select the second offset, zero it out, select the third zero it out, then take your gcode for one part, and duplicate it twice - changing the G54 to G55 and G56?

As for tool offsets (bear with me, im still learning), is that basically just the difference in z height between the tools? If this was a one off part, with manual tool changes, could I just manually zero out each tool after I change it?

[j_blankenship]

Right, you could use a different work offset for each vise and run a copy of the paragraph for each vise, or you could use a main program with a sub-routine that would activate the workshift in the main - the jump out to the sub to perform the cutting (be careful with this, it can be tricky). I can't say specifically for Mach3, it's been a while since I had a machine running with that and I don't really remember how it worked with workshifts and such.

Yes on the tool-length-offsets as well.

Sounds to me that you've got the concept pretty well.

Regards,
John B

[stylinmike]

Really appreciate your help! More questions to come later . Alot easier finding answers here than sifting from cnczone and its 200 sub forums

[Petri]

A lot of times I use several offsets even when running just one part just in case something gets messed up in the end. That way I don't have to retouch off the offsets again. Not neccessary but I find it helpful doing it that way since having more than one offset doesn't make any more work.

[j_blankenship]

I'm not 100% sure what you're saying, but it sounds like you will set something like G54 through G57 all at the same spot in cast G54 gets corrupted somehow. I know another guy that does that, he says he's had problem with just that happening and then he can switch to one of the others he set and keep truckin'. Whatever works for you.

I know a mold maker that sets a workshift several different places on the part, generally centered on a hole. Can't figure that purpose for it, but he uses it so he can program each area seperately...doesn't make sense to me.

[Petri]

I only do it if I have to flip the part more than once, that way when I mess up somewhere I just grab a new piece of material and keep on running. Guess it came from having to machine around parts and then flip them over to cut the back off, which would change the Z offset. Also if the origin on a print is on one side and and I have to flip it over I use the same side for touching off to keep the numbers in the program the same as on the print. Easier to follow the program when running for me but I'm sure there are just as many ways to run parts and setting offsets as there are machinists.

Only reason I see to have more than one offset on the same setup is if the print has more than one origin. Believe me I've seen it more than once. 

[lakevieweng]

There are work offsets (G54-G59 that set the x, y and z). Then there are TOOL offsets.
You can touch your tools off of the top of your workpiece and next time you will have to touch off ALL of your tools each time you change the height of your workpiece.  You WILL crash eventually with the tool you forgot to touch off.
What I do is touch off all my tools in all my machining centers 6 inches off of the table. Two 1,2,3 blocks stacked on top of each other. Bring the tool down below the top of the blocks and work your way up in the Z until the block slides under. If you come down on the hardened block you will chip your tool everytime. After you have set all your tools to the same 6 inch reference point, take an endmill and start the spindle. Come down onto the top of your workpiece until it just touches by .001". Then look at the Z dimension. Let's say it is -16.125" then look at the tool offset for your endmill. Let's say it is -16.500. You then have a part that is .375' HIGHER than your 6" reference blocks. You put that number in the Z of your G54-G59 offset, whichever one you are using. What will happen is ALL of your tools will move up the .375" and work off of the top of your part.
Then when you make a different part you only need to measure its difference in height from your 6 inch block.
Sometimes I program off the bottom of the part and sometimes I program off of the top of the part. You need to decide what you like better and make notes on your programs how you touched off that part.
This system is similar to boats in the ocean and how the tide raises and lowers ALL the boats. The taller parts are the high tides and the shorter parts are the low tides. Email me if you need help and good luck. Always watch your "distance to go" in Z when first running a new tool and a new program.