Z axis falling at end of job Fusion 360

LowRider CNC Troubleshooting
1

So I am new to CNC milling and just recently built the Lowrider with a 2’ x 4’ work area. I was very careful in the building process, checking everything multiple times and when I finally ran my first test project it all seemed to pay off as the program ran exactly as I expected it to until it reached the end where the Z axis lifted off the material and then after a few seconds it fell on the table before I had the opportunity to turn off the router. Not exactly sure what had happened I tried another simple test job and sure enough the program ran fine but the Z axis came crashing down at the end before I could get to the router.

I am using Fusion 360 CAD/CAM (still learning this program) with the MPCNC_Fusion360_V10_SDcard post processor and running the Lowrider with the LCD screen. The Mini-Rambo and LCD are both running the firmware they came preloaded with and I haven’t tweaked anything in that firmware.

One thing I have noticed is the line “M84; Turn steppers off” is at the end of all my gcode files. My guess is this is the cause of my issues, but I haven’t found a way to disable it in either Fusion 360 or the post processor.

Anyone have any suggestions?

2

Yes, the M84 is what will cause the router to drop after the job is finished. There should be an option in the post processor or you can manually edit the gcode to remove it. I use guffy’s postprocessor “DIYCNC_Marlin20.cps” and it doesn’t have the M84 (and I’m not seeing an option).

2 Likes
3

I have been digging through the post processor to try to find a way of disabling the M84, but either it doesn’t exist or I’m not familiar enough with editing post processors to see it (both equally possible).

What I have noticed is the M84 is created by a COMMAND_STOP_SPINDLE in the post processor, but haven’t been able to find that command in the Fusion 360 dumper file the processor uses to create the gcode. The closest thing the dumper file has is a COMMAND_STOP at the very end. It seems weird that the post processor would confuse these two but it’s the best theory I have at the moment.

I did see guffy’s post processor but wasn’t sure if it worked with Fusion 360. Will definitely take a second look at it.

4

I think the guffy pp has a manual spindle on /off, and it’s set to manual. Check that in your pp options, and maybe it will stop sending command_stop _spindle

5

This is what I’ve found in my pp:

if (properties.enableM106SpindleControl) onCommand(COMMAND_STOP_SPINDLE);
writeBlock(mFormat.format(84) + “; Turn steppers off”);
//writeln(“%”);

Pretty sure this is where the M84 is coming from and near the beginning of the pp there is a user-defined properties section that has this line:

enableM106SpinsdleControl: true, // enable M106/M107 for spindle speed control

But it doesn’t matter if this line is true or false the M84 always shows up.

6

Weird. Seems like making it false would skip the rest of the if loop

7

Not if it was C/C++. I have no idea what format or language the pp is in, but something like this:

if (properties.enableM106SpindleControl) 
onCommand(COMMAND_STOP_SPINDLE);
writeBlock(mFormat.format(84) + “; Turn steppers off”);
//writeln("%");

Is the same as:

if (properties.enableM106SpindleControl)
{
    onCommand(COMMAND_STOP_SPINDLE);
}
writeBlock(mFormat.format(84) + “; Turn steppers off”);
//writeln("%");
8

I can’t help with what language, but the line I quoted above is a direct copy/paste from the pp, it doesn’t have the curly brackets in the second quote.

If it is C/C++ what command would turn off the M84 line?

9

Just put ‘//’ in front of that writeBlock.

10

But, if this isn’t guffys post processor, you really should consider switching. He did a lot of work, and although I haven’t tried it myself (I am not a fusion user), the feedback has all been very positive.

11

For my own curiousity I’m gonna try ‘//’ in front of the writeBlock.

As far as guffys processor, do just use it or are there some firmware changes that need to be made as well?

12

Well, according to this, the post processors are written with java script. I thought that required brackets, and I think I imagined them there in that block of code. I’m really not sure. I didn’t realize that you could write single-line blocks without the brackets (or maybe I did at some point?) in java script, which I just looked up. I think I remember being able to do that in Java, but I only had 2 semesters like 5 or 6 years ago. I attempted to read up on some java script, but when I saw how different they are I decided VBA and SQL were better uses of my time. I need them regularly for my day job.

13

Just use it.

1 Like
14

So it turns out the pp I’m using it guffy’s. I downloaded the Marlin.zip file posted by guffy and the pp I’m using was in there. Guess it must not be to big a deal to turn off the steppers at the end of a job on the MPCNC, but it is a real nuisance on the Lowrider.

That PP training guide looks interesting, but the link didn’t work.

15

I’m using guffy’s postprocessor and for me it definitely does not include M84 at the end. Maybe it’s a different version?

Here’s what I’m using: https://github.com/guffy1234/mpcnc_posts_processor

Click the green “clone or download” button and save the zip file.

After extracting the zip, I copy-pasted the file into the folder “C:\Users(Username)\AppData\Roaming\Autodesk\Fusion 360 CAM\Posts”. I only copied the “DIYCNC_Marlin20.cps” and “DIYCNC_Common.js” files because it looked like the others were unrelated.

Then in the drop-down box to the left of the “Open Config” button, I picked “DIYCNC Milling/Laser - Marlin 2.0 / DIYCNC_Marlin20”.

At the top of the generated gcode files it has M84 S0 which disables the timeout, so it will stay on forever. There is no M84 at the end (or anywhere else) so the router will never drop.

3 Likes
16

Aw man, i posted it from my pc, even. Maybe I’ll try again after work tomorrow. Might be helpful.

1 Like
17

https://www.google.com/url?sa=t&source=web&rct=j&url=https://cam.autodesk.com/posts/posts/guides/Post%20Processor%20Training%20Guide.pdf&ved=2ahUKEwi_1rmCi-nmAhWkKH0KHT8tCFQQFjAAegQIAhAB&usg=AOvVaw1VSHORoAnyb6-TOHnrBnvp&cshid=1578111452899

1 Like
18

So, that’s the best I can do. The link goes straight to download and that’s probably why the other post didn’t work. I tried uploading it directly, but the forum doesn’t like the pdf. So that link is from a Google search.
Alternatively, just search “fusion 360 post processor manual.”

19

Thanks. Definitely gonna work my way through that guide.

I ended up seeing what would happen if I deleted the Writeblock that was creating the M84 command and the next test I did ran without a problem, but I also downloaded the Marlin pp and have been using that. The only tweak I’ve had to do with the Marlin pp is delete the Z probe section at the beginning of the gcode (cause I currently don’t have a Z probe).