Hopefully this is an easy question, but I know it’ll depend on a few things also. I’m using Fusion 360 (education license) for my CAM and the FlyFischer PP. I am using 1 setup and 4 operations that are separate gcode files. This is on my MPCNC Primo with the newest jackpot board, kobalt router, 0.5mm probe plate & clip, also using FluidDial to jog, probe, and run programs.
Before I run the first OP, I have the origin X0 Y0 Z0 set to top center of the stock in fusion 360 and I move the tool to above that point. I click “zero x” and “zero y” on the fluid dial. Then I setup the probe clip and plate and then command “probe” using the fluid dial. Then I retract from the probe and disconnect them from the tool. Then I turn on my router and run the gcode file for OP1 using the fluid dial.
OP1 is a 3D Adaptive Clearing with a 1/4” flat end mill (tool 31) that leaves 2mm of stock radial and axial.
OP2 is a Parallel operation with a 1/4” ball end mill (tool 32) that leaves 1mm of stock.
In between OPs I physically changed the tool, re-probed the top of the stock (not cut on) but did not do a tool change in FluidNC. This ended up 1-2mm too high during OP2, therefore not taking any material off.
I run Marlin, not FluidNC, so there may be FluidNC things happening here I don’t know about. My first guess is that you are baking in the retraction after the probing. Are there any G92 g-code commands in the postprocessor setup? Personally, I have a rule that, for any operations involving the top of the stock, the tip of the bit is always at (0,0,0) before I run the next file. I also don’t have any G92 commands in my postprocessor settings. During your Z probing you can have the bit retract to remove the probe, wait for a couple of seconds, and then drop to Z=0. Or you can manually send a G0 command to move to Z=0 just before running the second file.
If my guess about baking in the retraction is correct, it is possible your adaptive clearing is also 1 or 2mm high as well.
My start gcode that the PP inserts is attached. I do have a G92 X0 Y0 in there, but that only happens while it is physically located at the workpiece origin (in this case top center of stock).
As far as the retracting, I wasn’t using anything but the “retract” button on the fluid dial.
It’s possible that probing with the dial is not updating G92 Z0 therefore creating many possible issues.
I’m beginning to think it might be the fluid dial probing commands, and will try to find the code within the fluid dial to confirm. I will also try to use a probe during the start gcode, instead of with the dial before I run the program, since that’s what I’m finding while reading through many of the forum posts.
I initially thought it may be a tool length offset issue, but I’m still not sure how that works with how I’m running separate programs for each tool and whether I need to do a “tool change” with fluidnc so it has the tool length offset set to the correct tool.
Given your start code, the issue is not the one I expected.
I don’t know anything about FluidNC, but, given your process, I don’t think the absence of a “tool change” is the root of your issue. Is it possible that you have not correctly accounted for the touch plate thickness?
Just before you run each of the files but after probing, send the tip of the bit to Z=0. I don’t know FluidNC g-code, but you should be able to do something like “G0 Z0”, or you might need a feedrate so “G0 Z0 F200”. After running the command, see if the tip of the bit is touching the top of the stock. If it is not touching the stock, then you have the root of your issue, though you may have to dig a bit for the solution. If it is touching the stock, then that gives you more information to track the problem down.
Note you can run this test without cutting a project.
Yesterday I did that and found that the tip was 1 mm above the stock at Z0. I have the probe thickness set to 0.5mm for the touch plate, mic thickness of the plate was 0.48mm. In a few I’ll be running the new start gcode with a probe built in to see if it’s the fluid dial that’s causing the bad offset
Although I had to do some wizardry to make it work for OP3 (since i started OP2 the second time 2mm below the origin to actually cut material), I believe I figured out the issue.
I won’t be able to probe my origin on any operations after OP1 since the stock has been cut there, so I opted to write a probe macro that uses the proper gcode before I run my OP program.
I probe the top of the stock where it hasn’t been cut yet, using the probe macro I wrote.
jog to X0 Y0 Z0 (in this case where the top center of the stock would be if previous OPs hadn’t cut yet)
Run the gcode program for the next OP
During the start gcode it calls for G92 X0 Y0 Z0 to ensure G92 is set to where the origin is in F360 matches where the tool is located at the origin.
This iteration only: I dropped Z-1 before running the program, which brought the tool to where it’ll cut the 1mm stock remaining from the previous OP2. I won’t have to do this step anymore I hope…
Since you have stock out beyond the cut, could you not just change your G92 X0 Y0 to something like G92 X0 Y-20 and move -20mm before starting the job to get you over uncut stock?
I could, but it would have to be changed depending on which stock offset I’m using in F360. This is a round part that I decided to use the top center as the origin. On other parts I may use the top of the close left corner of the stock (seems to be the most used place). It just was I chose with F360 because originally I was going to cut this out of a round log 2” tall, but got this beautiful cedar plank yesterday for free!
I originally had G92 X0 Y0 in the start gcode, but now it’s G92 X0 Y0 Z0 and I have a feeling the fluid dial wasn’t setting G92 Z0 when I probed. With the probe macro, it’s seems to be setting it correctly, or the G92 X0 Y0 Z0 is correcting it.
I’m going to start a second one of these tomorrow, to confirm if this issue is fixed. In the end I’m pretty certain fluid dial’s probe screen isn’t accounting for the probe thickness I set of 0.5mm. Also I have a suspicion that G92 isn’t getting changed. I guess I’ll see tomorrow though.
I used a 1/4” yonico carbide 1FL end mill at 2000mm/s Feedrate 20k RPM during a 3D adaptive clearing for OP1. I left 2mm of stock radially and axialy. I set it to 0.5mm step down with a 1 dia. Max step down. I reduced the program time from 2hrs to 1.5 hrs by changing from 0.5 to 1.0 mm step down.
OP2 was a parallel operation with a 1/4” yonico carbide 2FL ball end mill at 4000mm/s feedrate 20k RPM. I left 1 mm of stock radially and axialy. I used “machine steep areas” and played with the step over, and steep area stepdown but didn’t drastically change the times or stepover. It seems this operation is more based on the “cusp height” to determine step over, but I’m still learning.
OP3 was another parallel operation with similar settings, but with a 1/8” ball end mill, and 0 mm stock left.
I am making another one currently and got rid of OP2 and changed OP1 to only leave 1mm of stock.
To finish this thread, I am confirming that using a probe gcode file and the start gcode attached here (instead of using the fluid dial probe menu), I can probe the top of the workpiece and run the program for OP1, change tools, jog to anywhere there’s uncut top stock, run the probe gcode, jog back to my origin (G92 X0 Y0 Z0), then run OP2, and don’t have the issue I originally had where the tool was too high for the subsequent operation. I run each operation that has a different tool without telling fluidnc I’m changing tools/TLOs other than the G92 X0 Y0 Z0 at the beginning of each gcode file. Thank you everyone for your help and input that helped me understand what I was doing wrong.
