I need help - Linear move on line .. would exceed joint 1's positive limit

[sabina....@gmail.com]

Hello together,

after i had create the toolpath in fusion, i had load the .ngc file in linuxcnc. Homing the the pocket nc and will start the milling part. The axis are moving, after a few second the message is coming up:

-Linear move on line ... would exceed joint 1's positive limit

why is this message coming? What is wrong and where is the issue?

[Xander Luciano]

Hello Manuel!

Welcome to the forums! The pocket NC can only travel so far in each direction, a total of 4.5", 4.8", and 3.3" for X, Y, and Z respectively (see: http://www.pocketnc.com/home-position). 

This error means that the gcode told the machine it needs to go to a position that is further than the axis can physically travel. So if you had G0 X6.0 then the software knows it can't go that far. If you know you part is within the correct size, check and make sure you are using the center of rotation as your origin in your CAM program.

Best of luck!

-Xander Luciano

@XanderLuciano

XanderLuciano.com

[Michael]

Hey Manuel,

Xander is right it is related to the machine not willing to move to the point it is being asked to go to. This is done when you go to run a program. I am pretty sure that Joint 1 is related to the Y-Axis. This means that the table is being asked to move to far down and the machine says it won't do so.

You may look at the NC code and see where the Y movement is happening. It may be related to the start coordinate of your tool, the origin/part relationship in fusion or possibly the g54 coordinate needs to be reset (home machine and then go to machine table > Zero coordinate system > P1 G54)

Let me know if you would like another look at your NC file to figure out where the issue may be at.

Hope this helps,

Michael

[Manuel Schütterle]

Hello, 

sorry for this late reaction. 

I had a look about the sizes of my part and everything is ok. 

I have added a few screenshots in the notes. You can see two red colored numbers and that's the problem. Can you explain what i do wrong and how could it work?

Thank's for your support. 

[Michael]

Manuel,

Is line 1091 near the end of your code or somewhere in the middle? It may be that the machine is retracting away from the part during that part of the code and being told to move away from the part so far that it would need to leave the machine envelope. 

you may also have an issue where the machine is confused on where it is suppose to go due to an offset or something that is causing it to think it needs to leave the machining envelope.

if you want you can send me your code and i can look at it a little closer.

Happy to help,

Michael

[Manuel Schütterle]

Hi Michael, 

thanks for your fast support. In the attachment you can find the gcode. 

[Michael]

Manuel,

Running your code it appears the issue is related to the end of your 3rd operation. 

the Z move on code line N33285 sends the machine to Z27.494 and i think this is when the issue occurs. I didn't do any math to figure out if this is outside of the machine envelope but it is a large Z move in relation to the surrounding code.

Because it is the last line of code in operation 3 i would be willing to bet it is a home or return location in the CAM software of the op. 3 specifications. You probably just need to edit the linking parameter or home position in that operation to get rid of this error. 

you may also check your later ops as they may also have a similar error which would show up after fixing this one.

Hope this fixes the issue,

Michael

[soheil....@gmail.com]

I have the same problem but the error does not make sense. "The linear move on line 0 would exceed joint 0's positive limit"
The first line does not ask any movement.

[Michael]

Soheil,

The errors talking about a max or min limit of a "joint" is talking about the different axis' of the machine. 

0=x

1=y

2=z

3=a

4=b

Accordingly. Then the line that the error is occurring on should be looked at more as a general area where the issue is occurring. Rather than line 1 for sure being the issue I would assume that a X axis move in the first 50 lines of your code is going to have the machine exceed the travel limits of the machine. I assume you have a V1 and the travel limits of that machine are on the website here. (http://www.pocketnc.com/s/HomePositionTravel.pdf )

Hopefully this will help you to find the issue. I am happy to look at your code as well if that is helpful.

Enjoy your day,

Michael

[Richard Tymko]

Did you solve this issue?

[Scott Schroer]

I'm having a similar issue. I have a V1 machine and just upgraded to the V2 UI. Everything seems to run fine, but the last few parts I tried say about 18 lines in that the Z axis will exceed the limit. I'm pretty sure it has something to do with the TLO set for the tool, its a tool and a TLO I've used many times so it shouldn't be a problem. It looks like the tool TLO is adjusting the Z G54 to the same offset so when the Z axis is in the zero position it thinks it's at 2.115 (or whatever the negative TLO is. When I try and move it even 1 inch it thinks it's out of its limits. Is there a way to reset the G54 so it doesn't think the spindle is already 2+in out? Will this effect the TLO? I'm calculating the TLO the same way I have been for the V1 machine (jogging with the 123 block, using the formula, and entering it manually) since there's no tool probe. Is there another way to do this? is this the problem? Thanks for the help!

[Jonathan]

Scott,

Try typing the command G10 L2 P1 X0 Y0 Z0 into the MDI interface. This will reset the G54 offsets on your machine. These offsets are intended to be set to 0. We are not sure how yours would have gotten changed. Would you please give this a try and let me know if it works?

Jonathan