"Linear move on line ... would exceed joint 1's negative limit"

[John Makowsky]

Hey everyone,

We've been trying get our Pocket NC up and running in our MakerLab, but no matter what we do, we can't get it to run any of the CAM paths from Fusion 360. I've used the setup file provided by Pocket NC, and followed all the steps, but I'm constantly getting the "linear move on line ... would exceed joint 1's negative limit" error, and when I look at the lines in the gcode there aren't any negative coordinates or coordinates outside the limits of the machine.

I'm at a loss for what the issue is, the .ngc file for the generated adaptive clearing path is attached, and I can provide screenshots of the setup if needed. The lines in question are different every time, the regulars culprits are 708, 711, 713.

I'd really like to get this thing to be able to do more than mill alignment test squares.

Thanks, John

Mentor, MakerLab 2RG

[Xander Luciano]

Hey John! Welcome to the forums!

This error is thrown when a movement tries to exceed the max travel of any given axis. Now reviewing your code I don't immediately see anywhere that it is over-traveling, and I checked the lines you specified. Now this leads me to believe your machine might not have zero set in the correct location, or you are using a work offset inside machinekit. 

Could you please some screenshots of the windows in Machinekit as well as your setup inside fusion? Or if possible you fusion 360 file as well? 

Thanks!

-Xander Luciano

[John Makowsky]

Thanks, Xander.

I don't have access to Machinekit, because the machine is back at the MakerLab, but I'll try to grab them this weekend. 

I've homed and sent a "P1 G54" to zero the coordinate system, but that didn't change anything. 

The Fusion 360 file is attached, it could be that the issue lies there. I come from 3D printers, so I'm used to 3-axis movement, and applications like KISSlicer, Cura, Slic3r, Skeinforge, etc for toolpath generation.

Thanks again for your help, John

[Xander Luciano]

Thanks for posting the file! I don't see anything wrong with the file so I'm wondering if maybe the machine was offset from zero. Have you had a chance to look at the machine set up yet?

Best of luck,

Xander Luciano

[John Makowsky]

I haven't yet, where in machinekit would I find that?

Thanks, John

[Randy Kopf]

John:

I downloaded your Batman.ngc file into my Pocket NC and had zero issues running the file.

I also downloaded your Fusion Model to check the setup. It is properly setup.

I homed the machine. Made sure I had a correct tool length offset defined for Tool #10 as that is the tool your program uses.

The program runs fine.

I recommend:

1) Load the AXIS GUI

2) Load your part program (Loading the file before homing allows a faster load and supports larger file sizes without the GUI crashing)

3) Edit the Tool Offset Table. (make sure the Tool 10 value is correct) The tool offset value needs to be a NEGATIVE number (TLO = -3.600" - Tool Stick out Length from Spindle)

5) Run your program.

I would not invoke any MDI commands prior.

Pocket NC has G54 hard coded to the Centerline of the 2 Rotary tables. And that is where your part origin is. No need to make an MDI call, The program manages the G54 correctly without you doing anything.

Post here if you need further help,

Randy Kopf

http://desktopartisan.blogspot.com/

See your file running by watching this video...

https://drive.google.com/open?id=0BxziiLimgn9SSVlpaEJ1d2F4ZGs

Here is my Tool Table setup

[Martin de Blois]

Got the same kind of error, mine is about exceeding Joint D's negative value...

The program stopped. Despite of this, I was able to complete the cut, so to speak, with the manual control. That would indicate that the machine was still within its limits, right?

Here is the link to the file in Fusion 360, http://a360.co/2aLccUe

And I attached the G code. Error is at line 6069

[Michael]

Martin,

I worked through your code and it is joint 0 that is giving you the issue. this is the X axis. The code does work if you offset the code by +0.3in X-axis. 

Is it possible for you to adjust your work piece so that it is moved over in the X direction? Could you adjust your vise to do this?

The other option is you will have much more travel if you turn your part 90 degrees on the B table so that the long direction of the part is in the Y direction. This would then probably work as you have the part held. You would have much less X travel distance required and your Y axis would be able to move the distances you need it to.

Hope this helps,

Michael

[Martin de Blois]

Michael,

that goes to say how bad my reading is on the small screen ;-)

So what is the work envelope?

This code stopped at about  35mm from the plane of axis B, or 40mm from axis B, the origin. 

I thought I located the origin in the set-up, to be the same as the machine...

This is x40. Is the other limit x-40 ?

What about the other axis?

[Michael]

Martin,

The work envelope of the machine is a littele different on the old and new spindle design. I am pretty sure you have the new spindle design. With that machine the work envelope is as follows.

In inches

X -1.75 to 2.55

y -2.05 to 2.95

z -3.45 to 0.10

A -5 to 95

B -9999 to 99999

In millimeters this is 

x -44.45 to 64.77

y -52.07 to 74.93

z -87.63 to 2.54

a -5 to 95

b -9999 to 99999

So with an X value of 40 you should be good if you are at the origin and only go out 40. is it possible that you have your tool cutting surface going out to 40mm but that the tool center is going out farther? Or do you have any X offsets setup that may be causing other issues?

Michael

[Martin de Blois]

OK, I got a better handle on the work envelope now. Was able to cut a resin base plate, with all the holes found on the B axis plate.

I am using this as a drilling template to prepare stock to mount.

Also using this resin base plate as a sacrificial surface.

So now my plan was to cut the hinge mounting plates for the enclosure I am building.

For sure I thought I had it figured out. No !

My end mill is cutting 5mm higher than it should...

I have tried reselecting the origin in the set-up, and in the tool orientation.

Here is the file, in A360: http://a360.co/2av8hpr

Attached is the code.

One thing that is strange, is that I noticed that when the machine is homes, the DRO for Z is not zero. It reads 2.2011". X reads 2.500, and Y reads 2.500" as they should.

If someone is kind enough to shed some light on this set-back of mine, I would appreciate the help.

Also attached is the enclosure I am building, awaiting the hinges mounts, and the general set-up of my workplace...

[Martin de Blois]

OK, I figured out that my origin point had moved in my Fusion 360 file. Have to look why and how that happened. Have to figure out a bullet proof method for avoiding that in the future.

Still have an incorrect depth. The tool cut too deep ! Fortunately it did not damage anything.

Will look again at tool offset to make sure I calculated the right value.

Also want to look at the Touch Off procedure.

Found this resource here:    http://wiki.linuxcnc.org/cgi-bin/wiki.pl 

More to follow. Beginner's drama...

[Martin de Blois]

I got it to work.

The problem came from the DRO reading in LinuxCNC Axis.

I had the DRO set on relative coordinate, rather than ACTUAL COORDINATES.

The difference was 1.436 mm. The "Over-Cut" I made in my previous test was twice that amount.

Can someone give me a cerificate now?

[Martin de Blois]

Michael from PocketNC reached out and we spent 40 minutes together reviewing the questions I had.

We discovered that my tool offset was still off by about 0.020". 

I want to express how much I am please with PocketNC outstanding customer service. 

Many thanks!