touch off vs tool touch off ?

gizmo6023 wrote: Since my machine uses an R8 collet I will need to do both touch offs for Z on each tool change?

If you are using an R8 collet then I would suggest post-processing each tool operation separately into different G-code files.
Load the tool, touch-off the tool-length, load the relevant file and run it. The change tools and run the next file.
You will find that this is more flexible (especially if things go wrong). You may find that in batch-production is it better to run the first op on each part, then the second op on each part, and so on. This does depend on accurate work-fixturing.

I see no information for X & Y touch off and what I am getting is not making much sense. I was expecting to set the part X0 Y0 but was getting something quite different, well over 1 inch different than expected.

Check your tool table, it is possible that you have accidentally put X and Y offsets in the tool table.

I will have to adjust where my part zeros are in Fusion as LCNC is placing the part 13 inches above the table and hanging over the left front corner by half the part dimension.

This isn't necessarily wrong...
In the CAM part of Fusion you need to set the machining origin in the "setup" section. You can choose the XYZ orientation and pick a part feature or the stock box as origins. By default it picks the part orgin, but that is very unlikely to be the machining origin.

It is very hard to change to part-origin in the part model inside Fusion. Don't bother trying. (It will be the origin point in the first sketch, so you need to redefine the starting sketch)

You then need to jog the CNC machine to the corresponding point on the work / stock and touch of that as the origin.

andypugh wrote:
If you are using an R8 collet then I would suggest post-processing each tool operation separately into different G-code files.
Load the tool, touch-off the tool-length, load the relevant file and run it. The change tools and run the next file.
You will find that this is more flexible (especially if things go wrong). You may find that in batch-production is it better to run the first op on each part, then the second op on each part, and so on. This does depend on accurate work-fixturing.

Makes perfect sense.

Check your tool table, it is possible that you have accidentally put X and Y offsets in the tool table.

I will have to adjust where my part zeros are in Fusion as LCNC is placing the part 13 inches above the table and hanging over the left front corner by half the part dimension.

Tool table was fine but my part origin was in the wrong place.

This isn't necessarily wrong...
In the CAM part of Fusion you need to set the machining origin in the "setup" section. You can choose the XYZ orientation and pick a part feature or the stock box as origins. By default it picks the part orgin, but that is very unlikely to be the machining origin.

It is very hard to change to part-origin in the part model inside Fusion. Don't bother trying. (It will be the origin point in the first sketch, so you need to redefine the starting sketch)

You then need to jog the CNC machine to the corresponding point on the work / stock and touch of that as the origin.

There may be a misunderstanding on my part on the value to assign to part origin ( assuming it is in the proper place on the part)
is this supposed to be the value displayed on the DRO for the axis being touched off or zero?

gizmo6023 wrote: There may be a misunderstanding on my part on the value to assign to part origin ( assuming it is in the proper place on the part)
is this supposed to be the value displayed on the DRO for the axis being touched off or zero?

No.

Imagine that the G-code origin in Fusion is set to the left front top corner of the stock.

You can jog your tool down to touch the top of the stock, then touch of the Z to zero.
Then do the same with X and Y to the left and front sides.

Now, when the middle of the end of the tool is at the G-code origin defined in Fusion the DRO will read 0,0,0

In practice you would not normally do it this way. You would use a wiggler or a probe.
If your probe has a 5mm ball on the end you would probe the left side of the stock and touch-off the X-axis to -2.5mm

To set Z height it can be convenient to use a dowel. I use a broken carbide end-mill but I can see a strong argument for using something like brass that can't damage the cutter. Don't jog down to the dowel, jog slowly up until the dowel just slips under the tool.
Then touch-off the coordinate system to the dowel diamter (8mm in my case).

What you are trying to achieve is a DRO reading of 0,0,0 when the tool tip in in the same place as the origin triad in Fusion.

Touch-off is about telling the system where the tool tip _actually_is_ in the CAM coordinate system at the time that you do it.

Thank you.
I guess part of what is making this difficult to visualize is only my tool path is displayed in AXIS.
Is there a way to display the part as in the Fusion Cam simulation?

gizmo6023 wrote: Is there a way to display the part as in the Fusion Cam simulation?

No. Partly because LinuxCNC only knows what is in the G-code, and that doesn't contain enough information.