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

[sn8kboy]

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

 

[JimDawson]

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.

That piece looks thicker than 1/8 inch, more like 3/8 inch, but maybe it's just the camera angle. That could explain why it's not cutting through. But check the depth of cut with a caliper and see if it hit about 0.277

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.

Is this what your setup looks like?

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.

It should start at +0.084 per the G code, and this is normally about the correct starting height, then ramp down into the work. The tool should not engage until things are moving.

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.

That is correct.

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!

Basically except for the X0,Y0 position, it looks OK. Do you have your machine coordinates set to conventional directions?

X+ = table moves left
X- = table moves right
Y+ = table moves toward you
Y- = table moves toward column

The speed up at the end is highlighted below, it's in the G code

****************** 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

 

[Flyinfool]

You never mentioned how you are setting the end of the tool to zero the Z axis. IS it as simple as the tool is to far up in the collet? Did the tool move since you set it?

 

[sn8kboy]

Wow you really have a good eye! The material thickness is .184 which is closer to 3/16 but I am amazed that you noticed that. I measured the depth of the cut and it is .034 so it is not even close to the 1/8 deep cut I was hoping for. Maybe my Z axis motor tuning needs some more tweaking?

Also I checked the direction of the X, Y axis and it is going in the opposite direction from what you are telling me. I had it go in those directions due to the instruction videos from Mach3 Artisoft. I must have misunderstood what they were telling me. If I change those directions I would have to move my limit switches to the rear right hand side of the mill correct? I would then have to change the directions in the Mach3 software to reverse the directions. Is that correct?

The speed up at the end is from this command? X0.54 F39.4

 

[sn8kboy]

You never mentioned how you are setting the end of the tool to zero the Z axis. IS it as simple as the tool is to far up in the collet? Did the tool move since you set it?

I zeroed the Z axis the old fashioned way with a piece of paper and slowly jogged the Z down until it lightly touched the paper. I do have one of those Z axis touch off plates which would give me a better measurement I guess but I was just in the testing phase.

 

[JimDawson]

Wow you really have a good eye! The material thickness is .184 which is closer to 3/16 but I am amazed that you noticed that. I measured the depth of the cut and it is .034 so it is not even close to the 1/8 deep cut I was hoping for. Maybe my Z axis motor tuning needs some more tweaking?

Maybe Z calibration is not correct, or the tool is slipping in the collet. Most likely one or the other.

Also I checked the direction of the X, Y axis and it is going in the opposite direction from what you are telling me. I had it go in those directions due to the instruction videos from Mach3 Artisoft. I must have misunderstood what they were telling me. If I change those directions I would have to move my limit switches to the rear right hand side of the mill correct? I would then have to change the directions in the Mach3 software to reverse the directions. Is that correct?

It could be that the instructions you looked at were for a router. Normally a router would be opposite from a mill because you are moving the tool, not the table. Yes, you would need to go through and position limit switches correctly as well as changing motor directions. You might be able to do all of this in the Mach3 software setup, but not sure about that.

The speed up at the end is from this command? X0.54 F39.4

Yes

View attachment 491635

This looks correct.

 

[sn8kboy]

Maybe Z calibration is not correct, or the tool is slipping in the collet. Most likely one or the other.


It could be that the instructions you looked at were for a router. Normally a router would be opposite from a mill because you are moving the tool, not the table. Yes, you would need to go through and position limit switches correctly as well as changing motor directions. You might be able to do all of this in the Mach3 software setup, but not sure about that.


Yes


This looks correct.

Jim

Thank you very much for your assistance! I will make the changes to the mill this Thursday and reply to this post to let you know how it all went.

Thanks again!
Paul Scott
AKA Sn8kboy Proud 1965 Shelby Cobra owner.

 

[RJSakowski]

I don't use Fusion to generate G code and I haven't used Mach 3 for quite a few years.

In viewing your video, I see two issues. One, the the program makes seven passes before it contacts the material. This appears to be operator error either in Fusion or in setting up the machine. The first contact occurs in the program at around Z = 0, so it appears that the Z =0 reference is set up at the top surface. However, there shouldn't be seven passes before contacting the material.

The second issue is that after the eighth.2 pass, the speed increases and the program shuts down. the G code shows that the program should continue cutting to a depth of -.227". To me, this indicates an issue with either Mach 3 or the machine controller. Had the program continued, the slot would have been cut through and the second slot would have been cut.

 

[jocat54]

I know nothing about mach3 (4) and not much about fusion, but I think G43 in your gcode has to do with tool offsets. Might try deleting the G43 command and see what happens. Disclaimer= I don't know a lot about gcode either

 

[sn8kboy]

I don't use Fusion to generate G code and I haven't used Mach 3 for quite a few years.

In viewing your video, I see two issues. One, the the program makes seven passes before it contacts the material. This appears to be operator error either in Fusion or in setting up the machine. The first contact occurs in the program at around Z = 0, so it appears that the Z =0 reference is set up at the top surface. However, there shouldn't be seven passes before contacting the material.

The second issue is that after the eighth.2 pass, the speed increases and the program shuts down. the G code shows that the program should continue cutting to a depth of -.227". To me, this indicates an issue with either Mach 3 or the machine controller. Had the program continued, the slot would have been cut through and the second slot would have been cut.

Good point I will try using another CAM software package to see if that improves anything. Mach3 comes with a program called Lazy Cam and I will watch a few videos on how to use that and try it again. That should determine if the problem is with Fusion 360 or not.