No Tool Touch Off button
Load a tool. (M6 Tnn G43 in the MDI window)
“The equivalent functionality is there by picking "tool table" in the drop-down in the dialog box.”
Any chance you could expand on that. I know how to get to the Tool Table but once there I am not sure how to touch each tool off.
Press "Touch off"
In the dialog box that appears, click the drop-down and select "tool table"
Put a number in the box that describes the current tool tip position. (for example, the diameter measured with a test cut)
There are a number of ways to do organise tool lengths. Some like to have a "master tool" which always has zero offsets in the tool table. (I do it this way, and use tool 1, a WNMG turning and facing tool, as the master tool). Then all other tool offsets are relative to Tool 1.
Alternatively you can decide to have zero in the working coordinate system offsets. Then the tool lengths are relative to the axis absolute zero position. This ought to work well and I am considering changing to doing it that way. Then You would use the G54 (etc) working offsets purely to set the Z=0 position along the bed (Z changes a lot, X almost never)
In either case, you can really mess things up if you accidentally touch-off the X into the Z box or pick the coordinate system rather than the tool in the drop-down.
Once set up I would suggest making a copy of the tool table, and noting down somewhere the G54 X offset.
After using Andy's method above to use the MDI to touch off each tool in the Tool Table, I then had to go back into my NGC program and replace all the M6 Tn tool changes with Hn G43.
Once I did that, it worked as I had expected. I still have a few things to refine, such as the best way to touch off a drill bit (on a lathe with gang tool post) and how to get Fusion to export the tool paths correctly for an inverted cutoff tool on the gang tool post.
Thank you though to all that commented and helped me work my way thru this. I will admit, this has been a much steeper learning curve than expected. However, as I am hopefully starting to get some of the basics, I can see how nearly anything will be possible with this general workflow of Fusion for the CAD/CAM and LinuxCNC to control my lathe now. But how from here that same workflow will work for a mill, rotary table, router, 3d Printer, etc.
RETAIN_G43 means that you only have to do it once. (which is just helpful enough to be a bit annoying)
You can remap "T" to do the whole thing as most lathes do, including tool wear offsets. I do rather think you shouldn't have to, but at least in 2.8 that is the way. Look at the sim/axis/remap/lathe_fanucy sample config.
So, where a commercial lathe might use
T0103 (Change to tool 1, use tool offset 1 and wear offset 3)
M6 T1 G43 (change to tool 1, use the tool 1 offsets)
I am used to using the LinuxCNC way so haven't changed my confog.
I have 3 tools setup on a gang tool post:
- T01 = 55 Deg LH insert tool
- T02 = Drill bit
- T10 = Upside down cutoff tool (to cut from X+ side not X- side
The steps I used to setup everything was:
- Edit Gcode to be able to handle gang tool post
- Replaced all M6 Tn w/ G43 Hn
- Home machine
- Set T01 (Master Tool)
- MDI > M6 T01
- Touch off Z > Select G54
- Touch off X > Select G54 > enter radius
- Edit Tool Table > Enter 0 for Z, 0 for X > save file
- Set T02
- MDI > M6 T02
- Touch off Z > Select Tool Table
- Use Coaxial Indicator to center bit
- Remove material from collet
- Center bit with indicator
- Put material back into collet
- Touch off X > Select Tool Table
- Set T10
- MDI > M6 T10
- Touch off Z > Select Tool Table
- Touch off X > Select Tool Table > Enter radius
- This worked but I am curious about a few things:
- Is this the proper way to do the "master tool" method?
- Did I actually need to change all the M6 Tn to G43 Hn for the gang post to work?
- If I turn my machine & control box off, other than re-homing, do I need to just touch off T01 again, or repeat the whole process?
[*]Edit Gcode to be able to handle gang tool post
[*]Replaced all M6 Tn w/ G43 Hn
You need "M6 Tn G43" for each tool change. G43 will assume the H to match the current tool.
ie, M6 _and_ G43.
[*]If I turn my machine & control box off, other than re-homing, do I need to just touch off T01 again, or repeat the whole process?
When you restart you should be exactly where you left off (assuming repeatable home switches), but will probably need to re-touch-off Z into G54 to suit the new stock.
If you load a tool (including G43) then you can touch-off G54 with any tool, and all the other tools will follow.