Help with Fixture Offsets

My goal is to zero all my tool lengths to the table and use fixture offsets to set the height difference.

So, I went into utilities, and I set all my tools to the table. This worked fine.

Next, I went to fixture offsets and selected fixture 1, and I jogged my tool #1 to the work surface and to the corner I want to be 0,0. I selected that and stored it.

So with selecting fixture E1. G0 X0 Y0 takes me to the corner of my part, wonderful.

Since tool one is already there, I do an MDI of Z6.0 H1 E1
It wants to drive the tool way below the work surface?

I think where I'm going wrong, is when I set fixture offsets, I need to apply the H1 before doing the fixture Z offset or I would be off by that amount of tool 1?

Any help?

If you set all the tool lengths to the table then the Z value in the fixture offset needs to be the distance from the table top to the Z zero surface. We use a tool length probe on our Fadal. The tool lengths are usually large negative values and the Z value in the fixture offset is a smaller positive value.
Take note-- You may need to pick up fiture offse and tool length on the same line. G0G90X1.Y1.E1Z2.H1
If the Z value in the fixture offset is greater than 4.0 inches and you try a position in X and Y with no Z offset the machine will hit the Z plus hard stop and crash. (been there , done that!)
Hop all this helps.

set tool offset relative to the table. this will be a negative Z dimension.
G0 H1 Z2.0
this will move tool #1 2-inches above the table.

set fixture offsets relative to the table too, but this will be a positive Z above the table.
G0 H1 E1 X0.0 Y0.0 Z2.0
this will move the tool #1 to 2-inch above the fixture offset #1.

So, are we saying that I take the tool 1 length offset then touch my work and record that Z position and subtract them then that is what I enter into the fixture offset?

Example: Tool 1 Length in the table is -18.500"
My part is above the table 5.500"

So my fixture offset is 5.500 which now makes tool 1 really -13.000?

The way I do it with my Fadal in format 2 is to set all tools based off the table.

Then I’ll go to T1 my 3d indicator. Next I will head to MDI and type
g90
G00 z12.0 h1
(this will take my tool tip 12” from the table. Change z depending on what you need)

Then hit jog and it still will account for the tool offset. Then I simply touch my z point and write that number down. Usually something like 5.5”.

Next I just enter that into the fixture offset.

The x and y I find with the offset utility normally.

Quote:

---

Originally Posted by rwskinner

So, are we saying that I take the tool 1 length offset then touch my work and record that Z position and subtract them then that is what I enter into the fixture offset?

Example: Tool 1 Length in the table is -18.500"
My part is above the table 5.500"

So my fixture offset is 5.500 which now makes tool 1 really -13.000?

---

Yes.
your tool offset will have a negative Z.
your fixture will have a positive Z and is the difference between the table and the fixture height (as you noted),
but will generally also include a X and Y offset.

Quote:

---

Originally Posted by rwskinner

So, are we saying that I take the tool 1 length offset then touch my work and record that Z position and subtract them then that is what I enter into the fixture offset?

Example: Tool 1 Length in the table is -18.500"
My part is above the table 5.500"

So my fixture offset is 5.500 which now makes tool 1 really -13.000?

---

Exactly! When you combine fixture offsets and tool length offsets on the same line the machine does the math right everytime. The way I have my students do it is:
1) set tool length(s)
2) MDI G0G90 Z8.H1 (or something safe above the part)
3) press "jog" do NOT depress manual. This leaves the tool length register active.
4) jog the tool down until you touch the top of the part (the Z zero surface of your part.)
5) write down the Z value shown on the screen.
6) enter the recorded Z value into the fixture offset.

Either way works just fine. Seems like I have to do alot of explaining both ways.
Let us know if all this info works for you!
Jim

Perfect. Yes, it seemed that is where I was getting messed up is after the MDI I was pressing Manual and it was jacking up my position. I will try again ! Thanks.

That worked perfect and using MDI the G0 G90 X0 Y0 Z2. H1 E1
put my tool on the corner and 2" above the work. Great.

Now I ran some simple test code, but it ran my Z above the CS position, like it's still using G53 coordinates.

Code:

---

%    (FADAL Program from Vectric)
O1004
N20G00G17G40G80G90
N25T1M6    (Profile 1)
N30G0X0.0000Y0.0000S0E1
N35Z2.5000H1
N40G0X0.0000Y0.0000Z2.500
N45G0Z1.500
N50G1Z1.0000F10.0
N55G1Y-12.0000F25.0
N60X12.0000
N65Y0.0000
N70X0.0000
N75G0Z1.5000
N80 T2 M6
N85 G43H2
N90 S0
N95G0X0.0000Y0.0000Z2.5000
N100G0Z1.500
N105G1Z1.000F10.0
N110G1Y-12.0000F25.0
N115X12.0000
N120Y0.0000
N125X0.0000
N130G0Z1.5000
N135M5
N140G0G80G90M5M9
N145Z0 G53
N150X0.0 Y8.5 Z0 E0 H0
N155M1
N160M30
%

---

Missing G43 on H1?

Quote:

---

Originally Posted by Techman

Exactly! When you combine fixture offsets and tool length offsets on the same line the machine does the math right everytime. The way I have my students do it is:
1) set tool length(s)
2) MDI G0G90 Z8.H1 (or something safe above the part)
3) press "jog" do NOT depress manual. This leaves the tool length register active.
4) jog the tool down until you touch the top of the part (the Z zero surface of your part.)
5) write down the Z value shown on the screen.
6) enter the recorded Z value into the fixture offset.

Either way works just fine. Seems like I have to do alot of explaining both ways.
Let us know if all this info works for you!
Jim

---

okay, I guess this is a Fadal deal. Anytime you change fixture it moves Z to Zero even when you don't tell it to?

Bad code here...

N25T1M6 (Profile 1)
N30G0X0.0000Y0.0000S0E1
N35Z2.5000H1

Change it to...
N25T1M6 (Profile 1)
N30 G0 X0.0000 Y0.0000 Z2.5 H1 S0 E1

And it works. I need to go fix the post so it doesn't do that anymore!

So I edited the Post Processor so it changed the position of some of the offset commands. It seems with Fadal, If you call a E# you better tell it where you want the X,Y, & Z !

Here is with the fixed post that seemed to fix all my woes.....
Thanks for everyone's help!

[CODE]
O1004
N20G00G17G40G80G90
N25T1 M6 (Profile 1 - Tool 1)
N30G0X0.0000 Y0.0000 Z3.0000 H1 S100 M3 E1
N35G0 X-4.0000 Y-4.0000 Z3.0000
N40G0 Z2.0000
N45G1 Z0.0000 F10.0
N50G1 X4.0000 F50.0
N55 Y4.0000
N60 X-4.0000
N65 Y-4.0000
N70G0 Z3.0000
N75 T2 M6 (Profile 2 Tool 2)
N80 G43 Z3.0000 H2
N85 S100 M03
N90G0 X-4.0000 Y-4.0000 Z3.0000
N95G0 Z2.0000
N100G1 Z0.0000 F10.0
N105G1 X4.0000 F50.0
N110 Y4.0000
N115 X-4.0000
N120 Y-4.0000
N125G0 Z3.0000
N130M5
N135G0G80G90M5M9
N140Z0 G53
N145X0.0 Y8.5 Z0 E0 H0
N150M1
N155M30
%
</CODE>

I had similar issues with mine with the head going up when I have it in format 1 and g90 default. The same program will run fine in format 2 default g91. If you have hsmworks there is a good post available from Autodesk.