General Help

More
07 Jun 2018 20:41 #111935 by andypugh
Replied by andypugh on topic General Help
I have fixed it in the master (development) docs. 2.7 is so different with the joints/axes split that it doesn't make sense to fix it in the 2.7 docs.

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

More
10 Jun 2018 16:14 #112137 by tjd
Replied by tjd on topic General Help
Hi all,

I've finally got the HURCO running off LinuxCNC. Axis tuned, homing fine. Everything is running as it should - thanks for all the help thus far!!!

Now I'm getting stuck with actually using it!
From my previous experience on the old HURCO system I would have a G code program (usually produced in CamBam) that would have a 'part origin' - the point from which all moves are made. I would load the material and set the part origin in the setup procedure.
I can't work out how that is achieved with Axis? I can see that there are several coordinate systems and I think, if I've got this right, G53 is the machine Zero (set by homing) and that the majority of the time I would be using G54.
How do I move my part/material to a point and then set this as the 'part origin' - my apologies for the poor terminology, I'm somewhat used to the old HURCO interface. Is this all done with the 'Touch Off' function?

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

More
10 Jun 2018 22:00 #112154 by Todd Zuercher
Replied by Todd Zuercher on topic General Help
Yes the machine coordinate systems g54, g55... are set using the touch off or G10 commands
linuxcnc.org/docs/html/gcode/coordinates.html

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

More
10 Jun 2018 22:13 #112155 by tjd
Replied by tjd on topic General Help
Great - I think I've got that.

While experimenting a little with the Axis interface I typed in T1 M6 in the MDI text box, hoping to see what kind of text/messages came up for a tool change.
Unfortunately it moved the Z axis to the home position and then showed me that the limit had been reached, despite overriding the limits I wasn't able to get any kind of message for manual tool changes.
At the moment I have
TOOL_CHANGE_QUILL_UP = 1
in the .ini file, do I perhaps need to delete this and replace it with something like
TOOL_CHANGE_POSITION = 0 0 2

??

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

More
10 Jun 2018 23:38 - 10 Jun 2018 23:38 #112160 by andypugh
Replied by andypugh on topic General Help
TOOL_CHANGE_QUILL_UP means that the Z-axis moves to the G53 Z=0 position.

It sounds like you might have configured with the home/limit switch at zero and home at -(small number)

Try setting the home switch to be at +(small number) and home at zero.
Last edit: 10 Jun 2018 23:38 by andypugh.

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

More
12 Jun 2018 22:34 #112266 by tjd
Replied by tjd on topic General Help
Yep - that was it. Working now, thanks very much.

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

More
18 Jun 2018 15:25 #112546 by tjd
Replied by tjd on topic General Help
Hi all,

So far I can see that axis will let me set X, Y and Z for a single job and, for that matter, a single tool.
How do I calibrate/home/zero/offset (not sure of terminology) multiple tools.
For example, a job/part needs 4 tools to machine it, where in AXIS GUI can I set up each tool relative to part zero??
I can't see if this is done from the tool table or somewhere else in AXIS.

Best regards, tjd.

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

More
26 Jun 2018 12:33 #112880 by andypugh
Replied by andypugh on topic General Help

For example, a job/part needs 4 tools to machine it, where in AXIS GUI can I set up each tool relative to part zero??
I can't see if this is done from the tool table or somewhere else in AXIS.


You use the tool table, but you can populate the table from the Axis GUI.

You do this using the "tool touch-off" button.

Here is one way to work.

Choose one tool to be your "master" tool, this should always have a zero-offset in the tool table.
Then use this tool to "touch off" the workpiece (using the normal "Touch Off" button)
Then change tools (M6 Tnn G43) to load another tool, and touch that off to the same point, but this time use "Tool Touch Off".
The result of this is to populate the tool table with the difference in length between the master tool and the other tool.

The G43 is very important.

If you have a probe then it is best to make that the master tool.

One way to touch-off is to use an accurate dowel (I use one of my many broken 6mm carbide milling cutters). Lower the tool to be close to the work and then jog _up_ until the dowel just slips through the gap. This is far safer than jogging _down_ to something.

Once you have set up your tools like this then you can use any tool to touch-off the work, as long as it is loaded with M6 and G43 has been applied.



An alternative way to do this is to actually measure the length of each tool and populate the table either directly or using the G10 commands.

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

More
28 Jun 2018 07:27 #112973 by tjd
Replied by tjd on topic General Help
Great, I had managed to work out some of that with trial and error since posting but had omitted the G43.
What does the G43 do to the touch off/tool touch off process?

Also, I select spindle speeds manually on the HURCO, consequently I haven't made any configurations for spindle encoder/pwm values.
I was expecting LinuxCNC to show me some kind of dialogue box (like for when changing tools) to indicate the spindle speed to set manually but it doesn't. How do I set this up? or is it not a feature of LinuxCNC?

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

More
28 Jun 2018 16:49 #112994 by andypugh
Replied by andypugh on topic General Help

Great, I had managed to work out some of that with trial and error since posting but had omitted the G43.
What does the G43 do to the touch off/tool touch off process?


It applies the tool-table offsets. With those not applied, or with the wrong offsets applied, the G10 calculations (which is what "Touch off does" will be incorrect.

Also, I select spindle speeds manually on the HURCO, consequently I haven't made any configurations for spindle encoder/pwm values.
I was expecting LinuxCNC to show me some kind of dialogue box (like for when changing tools) to indicate the spindle speed to set manually but it doesn't. How do I set this up? or is it not a feature of LinuxCNC?


As far as I know there isn't anything existing that does this.
I would strongly advise arranging for LinuxCNC to have control of the spindle. But if you can't then a Python userspace module (just like hal_manualtoolchange) shouldn't be hard to create.

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

Time to create page: 0.228 seconds
Powered by Kunena Forum