Problem with CNC mill not starting at Z0 --- Mach3 and Fusion 360

Use the single block setting to execute a single line of code at a time. Then you will be able to determine exactly where the program goes wrong.
 
JimDawson said:
sn8kboy.zip contains 3 files. Open the f3d file in fusion, review the drawing and the manufacturing setup. the part is a 3'' square, 0.200 thick, with a 1.5'' hole in the center. This should create that hole wherever you set X0, Y0. Run the Adaptive first, then run the Contour.

I'll be around to answer questions.
Click to expand...
Hi Jim

Here is an update. I triple checked all of the axis and did find a problem with the Z axis when I re-calibrated it. When I ran G1 Z1 it moved more than one inch WTF. I re-calibrated it a second time and then ran the G1 Z1 command again and it moved perfectly one inch. I then attempted to run Jim's adaptive G-code and it ran perfectly until the bit got loaded up with aluminum. That could have easily been remedied with my mist coolant system that I did not think I needed "woopsie". I saw the aluminum starting to build up on the bit and should have stopped it at that point but I wanted to see it through. When the chatter got too bad I did have to stop the program. Other than that I see this a successful CNC run.

Thank you to all of the people here on the forum for helping me get this far especially Jim Dawson. Hey Jim if you ever make it down to Oxnard California I owe you a ride in my 1965 Shelby Cobra!

 
sn8kboy said:
Thank you to all of the people here on the forum for helping me get this far especially Jim Dawson. Hey Jim if you ever make it down to Oxnard California I owe you a ride in my 1965 Shelby Cobra!
Click to expand...
Glad to help. If I get down there I'll take you up on that.

OK, we proved the machine runs but you have a lot of learning to do. The first thing is to get your machine coordinates set up correctly to match the rest of the world so you don't have to flip your CAM setup to match the machine. Or you could just check the Flip X box in the CAM setup for any given part, but that just feels weird. Air cuts and simulation both in Mach3 and Fusion are your new friends.

Using the free version of Fusion does have some limitations, one being is that you pretty much have to run each operation as a seperate G code file. It may run OK in Mach3, but combining operations in the free version causes my DC_CNC program to do some strange things on the transition to the next operation.

If I can be of any more help just let me know. I'm not an expert in Mach3, but I have a pretty good knowledge of Fusion 360 and CNC machining in general.
 
sn8kboy said:
I have finished fixing a Little Machine Shop CNC High Torque Mini Mill which was given to me because it had a blown cutting motor and it also had a blown controller circuit board that probably burned out due to the cutting motor going bad. I ordered a new motor and found a guy that repaired the blown controller board for the cutting motor. The Little Machine Shop mill was converted by a previous owner to CNC and has a Probotix CNC controller board in it. I have a Windows 7 32bit computer with a parallel port in it to connect to the Probotix Controller. I have mounted the CNC mill in an 80/20 extruded aluminum cage and have installed some nice limit switches. I have done all of the motor tuning and setting up the soft limits and other related items to the mill. I am running the Mach3 CNC software on this machine. I am also trying to figure out Fusion 360 for designing simple parts and then trying to machine them on the milling machine.

My first project is a simple part with two slots milled all the way through some 1/8" aluminum piece of scrap material. I had a couple of problems that I had to figure out when I tried to run the G-code for the first project. In Fusion 360 I picked the lower front left hand side of the part as my starting origin point. When I tried to run the part the machine was not starting at the lower front left hand corner but after hours of scratching my head I figured out that it thinks its starting point is the rear right hand corner of the part. This is okay I guess now that I have figured out that is what it is doing but I do not know why. If anyone knows the answer to this please let me know.

My second issue is when I run the G-code the endmill does not engage the part as expected. It starts at about .0844 above the part and then when the program completes it did not mill all the way through the part as expected. I am bewildered as to why Fusion 360 is doing this. I do see that while it is milling and watching the DRO that it does engage the part when the DRO reads the Z axis finally going to zero. So I am not sure if this is a Fusion 360 problem which I suspect it is or if it is a Mach 3 problem. Below I will include the G-code and give you a link to a YouTube video of what it is doing.

Please let me know what you think I am doing wrong!


****************** G-code Start*****************************
(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
Click to expand...
One thing I noticed now that I understand G-code a little bit better is that at line 15 I see that Fusion is sending my machine to G54 instead of my offset at G55 which is where I set my X and Y offset to. Why would Fusion 360 tell the machine to go there instead of my offset at G55? If this is normal how do I get the machine to start machining at a spot closer to the center of my X and Y location on the machine?

Thanks,
Paul
 
sn8kboy said:
One thing I noticed now that I understand G-code a little bit better is that at line 15 I see that Fusion is sending my machine to G54 instead of my offset at G55 which is where I set my X and Y offset to. Why would Fusion 360 tell the machine to go there instead of my offset at G55? If this is normal how do I get the machine to start machining at a spot closer to the center of my X and Y location on the machine?

Thanks,
Paul
Click to expand...
Unless you are cutting multiple parts you would not normally use a G55-G59. The WCS (Work Coordinate System) would stay at G54. It sounds like you are trying to force it to start cutting near 0, 0, but normally it won't do that. Many times it move to an opposite corner and start there. 0, 0 is not a starting point, it's just a reference. Sometimes you can force it to start where you want by setting Positions on the Linking tab.

1718056390397.png

I rarely use this. I just let it start cutting wherever it wants.
 
You must log in or register to reply here.
Back
Top