Z axis fails

More
07 Feb 2021 07:59 #197896 by shahargut
Z axis fails was created by shahargut
Hello there,

I've been using LinuxCNC for a couple of years for my Chinese 6040 3 axis CNC machine. honestly it never worked flawless but recently cut into some weird problem with my Z axis.

I'm using Fusion360 for CAD/CAM and exporting a NFC file for the LinuxCNC it a different computer.
when i open the file in LinuxCNC and zero the axes by "Touch off" for every axis (is there any difference if I'm using "Toll touch off"?).
After pressing Play i suddenly have Z height error claims the Z axis settings will exceed limits, also there is no physical truth in this claim. Also sometimes after hitting Play the Z indication suddenly changes by 12mm or so and often i don't catch it on time and the bit crushes into the part and massing over my job.

Any tips?
is it the driver? LinuxCNC setup? other?

Please Log in or Create an account to join the conversation.

More
07 Feb 2021 09:15 - 07 Feb 2021 09:20 #197899 by jbraun
Replied by jbraun on topic Z axis fails
Could it be something in the g-code?
With Fusion it could be G53 Z0 if your machine has Z0 defined in an unconventional way.
Or G43 if you don't normally run that code.
Or maybe G28.
Or maybe it's not the g-code at all.

On my router I delete all the above codes. It's just home the machine, then G54 touch-offs and run. No tool changes. I'm not familiar with 6040. Are you using tool length offsets ?
Last edit: 07 Feb 2021 09:20 by jbraun.

Please Log in or Create an account to join the conversation.

More
07 Feb 2021 09:55 #197903 by shahargut
Replied by shahargut on topic Z axis fails
It looks like G53 is used here. Could it be the problem?
Attachments:

Please Log in or Create an account to join the conversation.

More
07 Feb 2021 15:59 #197923 by jbraun
Replied by jbraun on topic Z axis fails
It's not a problem if you have run G53 in the past without a crash. G53 moves in machine coordinates unlike most g-code.
G53 G00 Z0 crashes when Z zero is not defined at or near the top of travel. In other words after a machine is homed Z travel should be in negative space if the DRO is set to display machine position.

I'm just making guesses based on the possibility that you don't usually use Fusion or have changed F360 post processors.
When using a machine without repeatable tool lengths I strip CAM created g-code to it's minimum.

Please Log in or Create an account to join the conversation.

More
07 Feb 2021 16:39 #197928 by OT-CNC
Replied by OT-CNC on topic Z axis fails
The G43 will load your tool length offsets. So you probably have an offset present in your tool library after hitting tool touch off.
I use the touch off button after jogging to my work 0,0,0 position so g54 becomes 0,0,0 if you're working in g54.
For simple parts I don't use the tool touch off if I'm not using multiple tools. I just program for one cutter and re-zero the z in g54.

Please Log in or Create an account to join the conversation.

More
09 Feb 2021 00:05 #198102 by andypugh
Replied by andypugh on topic Z axis fails

shahargut wrote: Also sometimes after hitting Play the Z indication suddenly changes by 12mm or so


This sounds like you have Z offsets in the tool table.

FusionCAM will always apply the tool offset when it loads a new tool.

So you either need to apply the tool offset when you load the tool, and before touching-off
(M6 Tnn G43)
or you need to make sure that the tool offset in the tool table is zero.
(G10 L1 Pnn X0 Y0 Z0 )

Please Log in or Create an account to join the conversation.

Time to create page: 0.107 seconds
Powered by Kunena Forum