Z axis issue with Fusion360 WCS

Hello, first offthis is my first request for help on this site. So I will start here notknowing if this is a lack of my understanding of LinuxCNC or the samething with Fusion360 CAM. So I will start here to make sure thelatter is good to go.

Made some things tocut on my little MDF machine in my garage and for simplicity lets sayit’s a square. Ran it through the CAM on Fusion360 setting the WCSorigin to be at front of the part, left hand side and top of the workpiece and no extra stock added during the CAM setup and do the 2DProfile, simple. Great piece of software for weekend hobbyist BTW.

Load up LinuxCNC andthen home the machine. Clamp in my work piece, in this case half inchplywood on a spoil board. Install my cutting tool. Move the machinedown and over to touch off both X and Y at where I want them to startin relation to the WCS I set in CAM. I believe I’m correct in thisunderstanding, right? Next I bring down the Z axis and touch it offto the top of the part with a sheet of paper. Once again I believeI’m correct in this understanding, right? Side note, the Z axistool touch off button is grayed out and cannot select it. So I’mjust picking the touch off button, since it is the only one I canchoose. Which shouldn’t make a difference, since all code startsfrom triple zero, right? Move the Z up a little, turn on the routerand press play to run the code.

The Z goes up tohome and prompts for a tool change. Click OK since the correct bit isalready install. It continues over to X0 Y0 and down to what I’mguessing should be Z0, right? But it starts cutting air. One time it drovethe bit in hard, but I think that was a my bad. The other three timesI have used it to cut parts it has been in the air. So continuing on,I stop the code and turn off the router. Move the Z down and do thesheet of paper again. But this time the tool touch off button is notgrayed out and can be selected so I use it now to redo the Z axiszero. Restart the OP and it cuts the part perfectly like I wouldexpect it to.

Whats going on? What am I messing?

Here is the first 30 lines of code from Fusion360

%
(JOERGBIG_OP1)
(T1 D=0.125 CR=0. -ZMIN=-0.465 - FLAT END MILL)
N10 G90 G94 G17G91.1
N15 G20
N20 G53 G0 Z0.
(18 INCH BLIND HOLES2)
N25 M9
N30 T1 M6
N35 S35089 M3
N40 G54
N45 M9
N55 G0 X1.625Y0.9375
N60 G43 Z0.6 H1
N70 G0 Z0.2
N75 Z0.08
N80 G1 Z-0.0312F165.776
N85 G0 Z-0.0272
N90 G1 Z-0.0625F165.776
N95 G0 Z-0.0585
N100 G1 Z-0.0937F165.776
N105 G0 Z-0.0897
N110 G1 Z-0.125F165.776
N115 G0 Z-0.121
N120 G1 Z-0.1562F165.776
N125 G0 Z-0.1522
N130 G1 Z-0.1875F165.776
N135 G0 Z-0.1835
N140 G1 Z-0.2187F165.776
N145 G0 Z-0.2147

It appears that in your G-Code your Z axis values are negative. This means that the top of the workpiece should probably be Z=0.0 as you have attempted to set. You need to make sure the origin point in the cam system is the same point you are selecting as your touch-off point.

Since you have had one issue where the tool gouged into the material and other issues where the tool is cutting air I am expecting your issue is tool length offsets in your tool table. When you touch off you are using a different tool number than the one used in your program. You touch off and get a Z=0 with the tool that it loaded for the touch off or with no tool loaded. Then the G-Code calls to load Tool 1 with the T1 M6 line. This loads the tool and applies the tool length offset in the tool table for T1.

My suggestion would be to set the tool length offset for T1 in your tool table to 0.0 if this is a manual tool change machine where you touch off the tool to the work-piece for each tool used.

Thanks for the reply nitro. I did some checking into the tool table on linuxCNC and there was values shown on the Z axis for the first three tools, so I changed them to zero and saved. See below for the file as it is now.

T1 P1 D0.125 ;1/8 end mill
T2 P2 D0.25 ;1/4 end mill
T3 P3 D0.201 ;#7 tap drill
T99999 P99999 Z0.1 ;big tool number

As you pointed out the gouging happened when I was playing around with some engrave CAM in fusion. For some reason it selected tool 64 or close to it and linuxCNC was putting up an error of no tool or some such. So was trying to edit the code to change it from T64 to T1 and H64 to H1 and that is when it hit the part. So as I said before totally my fault.

Also does this line on the code, override any values you have entered into the tool table? Or just add to them?

(T1 D=0.125 CR=0. - ZMIN=-0.465 - FLAT END MILL)

Once again thanks for the advice, I’ll have to brush up on the manual, WIKI and any other source I can find to read about the tool table.

ROFL, just noticed my avatar. How did the birthday balloons on the kitchen table end up as my avatar? Well guess since I’m using the laptop. I bet there was a curious two year old when I stepped away. Oh well was good for a laugh will have to change it. Thanks again.

The line you ask about is a comment as it is wrapped in parentheses. Any line or part of a line that is wrapped in parentheses is treated as a comment by the LinuxCNC g-code interpreter. The post processor for linuxCNC from Fusion360 has an option to print out all tools that are used in the file so that you can have them setup by reading the beginning of the file. This is an option in the post processor and can be disabled in the post processor dialog.

Another option you have to keep from having tool length offset issues is to use G49 to cancel using tool length offset compensation. If you put this at the beginning of your g-code file and don't ever use a G43 command anywhere else then tool length compensation will not be used.

Looks like you need to do some reading about the linuxCNC g-codes. Here is the link to the webpage with the g-code summary and details of each code.

http://linuxcnc.org/docs/2.7/html/gcode/overview.html

http://linuxcnc.org/docs/2.7/html/gcode/g-code.html

http://linuxcnc.org/docs/2.7/html/gcode/m-code.html

Deleting post as previous posters have already answered your question.