Defining part origins on a 2216?

[slick_ride]

I have read a dozen different threads and am still having problems setting the z-axis part home position that corresponds to my CAD coordinates. I have been using the fixture offsets under the utility menu and have no problem setting up the x and y axis' using an edge finder. I am not sure how to define the z-zero point (usually the top of my stock). I typically load my first tool, touch the top of the stock and call that my z-axis fixture offset. It doesn't work. I can get it to work by defining the H value in the code as zero but only for the current tool. Any tool loaded after will crash. What is the proper way to tell the machine that the top of the stock clamped in the vise is located at z0? Do I need to pull the tool out of the spindle or register the top of the table? I use one vise and set the tool offsets to the top of the vise. Thanks, Dan

[Techman]

Maybe the best thing for you to do is leave the fixture offset set to Z 0 and then set each individual tool length on top of your part so that the tool length takes care of the Z value. If you leave the same tools in your machine from job to job and the Z height varies from job to job then you may want to consider always picking your tool length up on a gage block set on the table. If you set your tool lengths this way then you would need to establish the distance from the top of the gage block to the Z zero surface of your part and put that number in your fixture offset. Our machine has a tool length probe and thats basically how we handle it. It works out nice because I wrote a macro to automatically set the tool length. One last precaution- if you use a gage block to set tool lengths, and the Z zero surface of your part is 4.00 in or more above the top of your gage surface, you will have to pick up tool length and fixture offset at the same time.
G0G90 X0 Y0E1Z1.H1*THIS WILL WORK
G0G90 X0 Y0E1*THIS WILL CAUSE THE Z AXIS TO LIMIT OUT
Hope this long-winded answere helps!
Techman

[Techman]

Dan,
Whoops! I just re-read your post. Sound to me like you just need to put the distance from the top of you vise where you set your tool lengths to the Z zero surface of your part in your fixture offset table.
Techman

[fizzissist]

You need to think about it differently.

The computer needs to know how far each tool is from the part's Z0. That's not a fixture (E or G54) function, but the tool length (H) function.

Bring each tool down to touch off of your Z0, and the distance from the machine's Z0 home position is input into the tool length offset table in the control. You've got a dia and a length for each tool in that table..with the ability to use multiple values for each tool.

THEN, you have to initiate the H value before the tool starts cutting.

N10 T3 M6 ( SPOT DRILL
N20 M3 S1000
N30 G0 G90 X0 Y0 E1 (this is your fixture offset,,primarily for X,Y location
N40 G0 H3 D3 Z1. M8 (moves tool 3 down, and in doing so initiates H value for that tool
G0 X0 Y0 Z1. E1
G0 Z0.5
G83 G98 R0+.1 Q.05 P0.005 Z-.2 F3.
X1. Y1.
G80
G0 Z1. M9
G0 Z0 H0 M5

Any Z value in your E table is going to apply globally to ALL tools, and is used because one fixture amongst many gives you a different Z0 for that part.

Does this make sense?

[slick_ride]

Definitely makes sense but I need a little more clarification. I rarely make two of one part, primarily one-off stuff for fun. So if I have two completely different parts (cutting one part at a time) with different z0 locations, I need to define tool offsets for all of the used tools for each part? Meaning, I need to bring down and touch off each tool at my z0 for every part. I should use the tool offsets to define the part's z0, not the fixture offset? So every time I clamp up a piece of stock I need to reset the tool offsets. Sorry for the ignorance, it's just different than my other mill. Thanks again, Dan

[Techman]

Either you pick up all the tools on your part top for each different part that has a different height and use tool length offsets alone (H values), OR pick up all your tools on your vise top or something that never changes and use height offsets (H values) AND a Z value in your fixture offset. To use the latter you will need to establish only the difference in height between the top of your part and the top of your vise and put that number in your Z value in your fixture offset. Hope this helps!
Jim

[fizzissist]

Originally Posted by slick_ride Definitely makes sense but I need a little more clarification. I rarely make two of one part, primarily one-off stuff for fun. So if I have two completely different parts (cutting one part at a time) with different z0 locations, I need to define tool offsets for all of the used tools for each part? Meaning, I need to bring down and touch off each tool at my z0 for every part. I should use the tool offsets to define the part's z0, not the fixture offset? So every time I clamp up a piece of stock I need to reset the tool offsets. Sorry for the ignorance, it's just different than my other mill. Thanks again, Dan

2 Different parts on the table at the same time with entirely different fixture offset X,Y AND Z values ?

You've got enough offset pairs available to touch the tools off of both parts.

So, for example...

Part one uses Tool 1, diameter offset 1, height offset 1. T1, D1, H1, E1.

Part #2 uses Tool 1, but diameter offset 31, height offset 31, and E2.

....Part #1 then would have T1, D1, H1, E1...while Part #2 uses T1, D31, H31, E2

The logical progression being that Tool #2 would be for Part #1 T2, D2, H2, while for Part #2 it would be T2, D32, H32, and so forth.

Make sense?

This is just one way of doing it....

[fizzissist]

As to setting your tool length offsets....what control do you have, are you using Format 1 or 2?

Setting tool length offsets is terrible simple (even if it's a PIA). Is that the real confusion?? Is it that you really don't understand how to set the TLO? If so, we can walk you through that, but it would help to know which control and format. It's really easy, even without pictures.

[slick_ride]

Okay, I got it now. I setup the tool offsets off of my vise and didn't define the fixture offset (z) properly as the difference between the tool offset location and the top of my part (Thanks Jim). Thanks again for all the help. Dan

[carbidecraters]

Life would be great if every vertical mill had a tool eye and a diameter setting so you would only ever have to set one tool...but alas this isnt a mazatrol lathe

[DareBee]

Nah
Set all your tools to zero on the machine table.
This way you won't have to over change a tool setting unless you change-out that tool.
Measure the height from the table (tool Zero) to the zero surface of the part being machined.
Enter this in your fixture offset table under z. Being that you are above the tool setting plane the value will be positive.
Remember to call the H(tool #) in your program with the first Z move after every tool change.
You can cut 5 different parts with different part Zeros as long as you use (and call) the correct off-sets.

[Delw]

heres the simplist way if your locating off a vice.

have all your fixture offsets at zero

then touch every tool you have at the cut jaw face, Ie locating surface.

then lets say you put a part in the vice that is 1.0 tall.
you set your fixture offset for that "E" number at 1.0.

all your tools will follow suit
now lets say you break a tool and need to reset it, and you have the fixture offset still in, no biggy just set the tool at the same spot( vice locating surface)

that way your cad file will always show "0" for the top of the part and NO matter how tall the part is you put that number into the "fixture offset for that corresponding "E" number.

you dont necc. have to use the locating surface of your vice jaws you can use anything that is fixed and doesnt move, Ie Table, back of vice, top of stationary Jaw ,even a small chunk of metal used for a reference "Z" point that never moves. then you measure from that point to the top of your part or any zero on your part( were your cad calls "0" and put that into the fixture offset on the "Z"

Hope that all made sence.
Delw