[sn8kboy]

Hello Everyone

I am a newbie. I just got my CNC mil all working and I have tuned all of the axis using the tool built into Mach3. I zeroed all of the axis and created an offset at G55. I started the G-code to run which is just milling two slots in a piece of 1/8" aluminum. My machine is a Little Machine Shop High Torque mini mill converted to CNC. I created the milling project in Fusion 360. What happens when when I run the G-code program it moves the flat endmill to above the part and starts moving back and forth milling air above the work piece. It eventually starts to cut into the part and mills the two slots perfectly about 1/16 deep into the material. The program was supposed to mill the slots all the way through the part. I double checked the X, Y, and Z offsets and verified that they were correct. I even ran the motor tuning wizard again to confirm that the Z axis was moving the correct amount. I can see on the DRO that it is in fact starting above the part and when the zero axis moves down to where the Z axis is 0 it engages the part and starts cutting the material. I am suspecting that the problem is with the G-code generated by Fusion 360 but I am not experienced enough with G-code to see what is going wrong. When I post the G-code from Fusion 360 I do get an error that states "The operations ether contain errors or are out of date". So maybe this is my problem? Here is a copy of the G-code I am running. When reviewing the G-code below I do see that it looks like it is starting .0844 above the part and starts moving down from there. That appears to be my problem but why is Fusion 360 doing that? Should I be brave and try to remove the lines that are above Z0 and run it from there? If I do that will the G-code allow it to go all the way through the part? I think not and I would need to add more lines of code to get it to go further into the material to go all the way through the part.

Here is a boring link to a Youtube video I made of the first attempt.

https://youtu.be/3j5eFsXiOjM?si=ij4ylQhpdjb8N63G


(1001)
(T1 D=0.3125 CR=0. - ZMIN=-0.227 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G20
(WHEN USING FUSION FOR PERSONAL USE, THE FEEDRATE OF RAPID)
(MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING MOVES,)
(WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED RAPID MOVES)
(ARE AVAILABLE WITH A FUSION SUBSCRIPTION.)
G28 G91 Z0.
G90

(SLOT6)
T1 M6
S5000 M3
G17 G90 G94
G54
G0 X0.54 Y1.71
G43 Z0.6 H1
G1 Z0.2 F39.4
Z0.1 F13.1
X3.45 Z0.0844
X0.54 Z0.0689
X3.45 Z0.0533
X0.54 Z0.0377
X3.45 Z0.0221
X0.54 Z0.0066
X3.45 Z-0.009
X0.54 Z-0.0246
X3.45 Z-0.0401
X0.54 Z-0.0557
X3.45 Z-0.0713
X0.54 Z-0.0869
X3.45 Z-0.1024
X0.54 Z-0.118
X3.45 Z-0.1336
X0.54 Z-0.1491
X3.45 Z-0.1647
X0.54 Z-0.1803
X3.45 Z-0.1959
X0.54 Z-0.2114
X3.45 Z-0.227
X0.54 F39.4
Z0.2
Y1.04
Z0.1 F13.1
X3.45 Z0.0844
X0.54 Z0.0689
X3.45 Z0.0533
X0.54 Z0.0377
X3.45 Z0.0221
X0.54 Z0.0066
X3.45 Z-0.009
X0.54 Z-0.0246
X3.45 Z-0.0401
X0.54 Z-0.0557
X3.45 Z-0.0713
X0.54 Z-0.0869
X3.45 Z-0.1024
X0.54 Z-0.118
X3.45 Z-0.1336
X0.54 Z-0.1491
X3.45 Z-0.1647
X0.54 Z-0.1803
X3.45 Z-0.1959
X0.54 Z-0.2114
X3.45 Z-0.227
X0.54 F39.4
Z0.6

M5
G28 G91 Z0.
G90
G28 G91 X0. Y0.
G90
M30

[Superman]

#1... Your program is stating G54 in the program as the co-ord system for the work origin. The position of the XYZ "work origin" should be the same as what you have in Fusion.

You setting G55 has NO effect whatsoever where the program is placed. You have to use what is in the program

[joeavaerage]

Hi,
Fusion starts a cutting toolpath above the material surface and works down ito the material. Sounds like its ramping in.

Try experimenting with Fusion Heights tab. As You can see there is a height called Feed Height....and that determines when Fusion goes into cutting mode, and note also that it defaults to 5mm.
You can set it to whatever you want....although you'll crash if you set it negative!. There is another height called the Top Height. It is usually the surface of the material at that particular time.
In the screen shot it is at the top of the stock, but in later operations much of that stock will have been machined away so you can start it a some other height. Note also that there is an offset.

Using the Heights Tab is fundamental to Fusion Manufacture.

Craig

[sn8kboy]

#1... Your program is stating G54 in the program as the co-ord system for the work origin. The position of the XYZ "work origin" should be the same as what you have in Fusion.

You setting G55 has NO effect whatsoever where the program is placed. You have to use what is in the program

Very good catch! How do I get it to use G55 as my offset? I do not want to start machining at my machine coordinates offset at G54. I wondered why is was doing strange stuff.

[joeavaerage]

Hi,
you can cause or force Fusion to post Gcode to your liking. For instance by putting a G55 at the top of your code.

This is done with the Manual NC option of the Setup tab (pictured).

By choosing Manual NC you get a dialogue box that includes all the different options that you might like, including one called 'Pass Through'. This will cause a line of Gcode of your liking being posted
in the eventual Gcode file produced by Fusion. Note that if you want it at the start of the Gcode file you'll have to drag the Manual NC entry to the top of the operation tree.

Craig

[Superman]

Very good catch! How do I get it to use G55 as my offset? I do not want to start machining at my machine coordinates offset at G54. I wondered why is was doing strange stuff.

You need to understand the process/steps from design, to creating toolpaths, to post-processing, to tool setting, to running the machine.
Each have the possibility of creating errors, how big the error gives a proportionally sounding crunch.
It happens to us all.

If you are unsure of how to set the work co-ord system in Fusion. You can edit the NC code file that you have in #1 post from G54 to be G55.
Remember, that repost-processing the code will change it back to G54.

This is one way that ppl have multiple setups on the one table( if table is large enough) ie vice1 uses G54, vice2 uses G55, etc, etc