[Ed from NY]

HI,

The manual says "In Format 2 the H word will only pick up the tool length offset. It is also used for Tool timers selection" and the gcode looks like this:

T1 M6
G90 S7500 M3
G54 X-2.305 Y-1.095
H1 Z1.06 D1
M8

T5 M6
G90 S3124 M3
G54 X4.27 Y.5599
H5 Z1.06 D5
M8

Aren't the tool offsets set with the UT command? Why do I need an H word then? What do the "Z1.06" and "D(tool number)" do?

Thanks!!

[vertcnc]

H1 pulls the length offset data from the tool table for T1
D1 pulls the diameter offset data from the tool table for T1 If you have your cam software calculate for tool diameter then D1 is not needed unless you use it for tool wear.

[Ed from NY]

Cool thanks. That is a weird way of doing it, that it does not pick up the offsets automatically, but at least I know what is going on.

I suppose the "Z1.06" is just a rapid that happens to be in the same line.

Thanks again!

[vertcnc]

That's pretty standard for all controls, and is a Gcode standard. It is kind of handy on a Fadal were you could actually use the H word for the tool used and The T word for the slot that it is located in the changer. You will notice that the tool table can hold at least 99 entries, but the changer has only 20 slots.
So you could call T1 H65. were it would be the tool in the #1 slot and the offset for what is #65 in the tool table.

[Ed from NY]

Ha! That is helpful Thanks!

[megacanam]

So I am having issues with tool offsets.... what am I doing wrong?

First, I went through the mass tool setup to define the lengths and diameters using a 123block set on the table. T1 = Haimer 3D, T2=5/16 EM, T3=1/8 drill.

I am picking up my work piece XYZ using the Haimer and storing it to the G54 work offset.

when I input:

T2 M6
S1200 M3
G1 F20.
G54 X0Y0 H2 D2

It wants to plow into the wooden block that I am practicing on, and not even close to the X0Y0.

Thanks guys.

[WILDMAN2]

So I am having issues with tool offsets.... what am I doing wrong?

First, I went through the mass tool setup to define the lengths and diameters using a 123block set on the table. T1 = Haimer 3D, T2=5/16 EM, T3=1/8 drill.

I am picking up my work piece XYZ using the Haimer and storing it to the G54 work offset.

when I input:

T2 M6
S1200 M3
G1 F20.
G54 X0Y0 H2 D2

It wants to plow into the wooden block that I am practicing on, and not even close to the X0Y0.

Thanks guys.

After you set your tools to that 123 block . did you set z0 at the top of your wood block? might want the H2D2on the next line

[rodney247]

In your Fixture offset page you probably stored a Z value in the G54. And you probably only wanted an X and Y. And I am assuming that when you set your tool lengths using the UT command your Zaxis was probably at the C.S.(tool change) position

[megacanam]

Yes that's right... But if I delete the z value from the work offset, how will the machine know where to go?

I've got a lot more reading to do... Thought I had it figured out, but now I'm just confused.

Thanks guys

[rodney247]

For example if you have a length offset for tool 1 of -15.000 and you store a z value in the fixture offset 1 of -15.000. and in your program you go to G54 that applies the -15. for the fixt and then the H1 applies another -15.00 from that point for the tool . Total z move will be -30. Crash. You really dont need a Z in the Fixture offset when you are using just one Fixture. The Z value is really used to make up the differences between Multiple Fixtures say you have 2 vices, and you set your tools to the first part in vice 1. when you go to vice 2 there may be a small difference in the Z say .02. so in fixture 2 there would be a value of .02 to make up the difference in the part location.

[megacanam]

For example if you have a length offset for tool 1 of -15.000 and you store a z value in the fixture offset 1 of -15.000. and in your program you go to G54 that applies the -15. for the fixt and then the H1 applies another -15.00 from that point for the tool . Total z move will be -30. Crash. You really dont need a Z in the Fixture offset when you are using just one Fixture. The Z value is really used to make up the differences between Multiple Fixtures say you have 2 vices, and you set your tools to the first part in vice 1. when you go to vice 2 there may be a small difference in the Z say .02. so in fixture 2 there would be a value of .02 to make up the difference in the part location.

Thanks for the clarification Rodney, I really appreciate Your help.

[rodney247]

no problem. If you need pretty much any Fadal manual you can download them here Fadal Manuals | ItsCnc.com

[KEVINSTJ]

I always do it like this.

M06 T1
M03 S1000
G0 G90 G54 X0.00 Y0.0
G43 H1 D1 Z.100

The G43 calls the height offset and H1 call the tool offset and the D calls the diameter offset. You don't have to put the D in. I only use the D when I am using cutter comp.

[megacanam]

Thanks kevin....

Rodney, I took the z out of the work offsets and it functioned exactly as needed. thanks again.