Manual tool change + tool lengh touch off

swalts wrote: LukeH,

You may be the same person I subscribed to and asked to make a video about this very same subject.

The sub-routine looks for M6, when it finds it then it halts the machine tells me to insert a tool (Tn M6?).
Then after i change the tool it runs over to the location where i tell it to touch off the plate.

The process sounds simple enough. I think my hang up is where do i tell linuxcnc or fusion360 to invoke sub-routine on M6? How do i find the program (even an example copy) to remap m6 command to the new sub-routine?

Thank you again for your time.
-swalts

Ha, yes I'm the same person.

An M6 calls the sub routine which in my case runs the Z to the top of travel then a message pops up on screen asking to insert Tn. Clicking okay then carries on with the measure routine.

Orangecat's reply on Page 4 of this thread will give you all the info you need to get started. It's what I based mine on however I modified it because I didn't want to automatically return to the part, so I could do a part touch-off each time the tool is changed. To make this practical I try to group my operations by tool and I post a separate g code file for each tool. It really doesn't take much time to load each file.

Also, note that some post processors will automatically add an M6 into the G code and will send the Z to zero before a tool change. I modified my post processor (Fusion360 LinuxCNC) so that I take care of tool changes entirely in the sub-routine. All the post processor does is insert an M6.

Give me a shout if you need any help. I'm happy to share my ini and sub-routine files to you.

Luke.

Hey Luke, I also use Fusion360 and would appreciate you sharing your current sub routines. Thanks mate.

trentster wrote: Hey Luke, I also use Fusion360 and would appreciate you sharing your current sub routines. Thanks mate.

Hi

I have been meaning to write this up ever since I got it all working. Hopefully this will be useful to some of you. It works for me and could probably be improved. I have produced lots of accurate parts on my mini CNC using this setup.

I have attached my LinuxCNC config files for reference.

Changes required

1. Created tool-change.ngc and saved in /macros/ folder on CNC - I've attached mine for reference
2. Downloaded LinuxCNC Post Processor from - cam.autodesk.com/posts/
3. Saved Post Processor into - /luke/Autodesk/Fusion 360 CAM/Posts/ - you will need to locate your Fusion360 folder. I'm using a mac
4. Removed retract to G53 Z0 from post processor by deleting these lines (appeared twice)

else {
writeBlock(gAbsIncModal.format(90), gFormat.format(53), gMotionModal.format(0), "Z" + xyzFormat.format(0)); // retract
}

5. Edit your cnc.hal to include the manual tool change stuff. Refer to my mf70.hal for reference.
6. Edit your cnc.ini to include the M6 remap under this heading [RS274NGC] - refer to mine for reference. I also commented out
tool_change_at_G30

CNC config you will need to do

Note. Z zero for my CNC is at the top of travel i.e. tool furthest away from table. All of my tools have a negative length value and all z references in the config files are negative value as a result.

1. You will need to update the X & Y co-ordinates of the touch of sensor in the tool-change.ngc config file
2. You will need to update the height of the touch of sensor in the tool-change.ngc config file - I opened up the pin viewer for the probe pin, 13 in my case (I will update this section with more detail once I've gone through it again on my cnc) and jogged down to the sensor until the pin updated to True. This Z position was added to tool-chang.ngc under <_Ztravel> heading
3. You might need to update the min & max tool length values in the tool-change.ngc file

Fusion360 steps

1. Produce G code for each tool within your part. I try and group tool ops by the tool to avoid lots of tool changes. This isn't always possible.
2. Select the post processor stored on your computer rather than the cloud version - Fusion will remember this next time and use automatically.
3. I tend to add a comment into the g code before I save it with part coordinates and any tool order reminders.
4. I name my gcode in this format - sample_part_PT1.ngc, sample_part_PT2.ngc etc... - this makes it obvious when you come to run the g code on your cnc.

Bonus - getting your g code over to your mill

1. I have setup mega.nz on my Fusion360 Mac and my CNC located in my garage. I have a "watched" folder on both systems so each time I generate a g code file in Fusion I save it to a folder called "CNC". This automatically syncs to my LinuxCNC machine so no need for USB sticks.
2. You could use Dropbox to achieve the same however, mega.nz gives you 50GB free and its encrypted end-to-end so no fear of your files being leaked.

LinuxCNC setup routine

1. Launch LinuxCNC and Home all Axis
2. Open G code to run
3. Manually run Tn M6 (n being the tool number for that program) from MDI - auto tool touch off runs and sets Z offset by updating tool table.
4. Jog to material and touch off in all Axis using tool. - I use paper method to touch off in Z
5. Run program
6. Program initiates tool change by issuing Tn M6 command. A message will pop up on screen saying "tool already in spindle. no change required"
7. Program runs.

Notes.

1. T0 M6 will reset selected tool back to nothing. Auto tool routine will only retract Z back to zero and will not run the touch-off routine.
2. T1 M6 in my case will select tool 1 and will not run the touch-off routine. This is due to tool 1 being a touch probe for me and I don't need to measure it.
3. If you have an accurate touch probe you can avoid doing the paper method touch off described above by doing a T1 M6 (1 being your probe number) first, touch-off your part in all axes and then just allow the tool-change routine to be called by gcode each time and measure the tool length. - my touch probe isn't highly repeatable so I prefer to touch off in z each time for each tool change.

I hope this helps. Feel free to ask any questions.

Thanks so much mate, much appreciated!

I am having a thorough look at some of your changes and will be implementing them on my machine over the coming days.

LukeH wrote:

trentster wrote: Hey Luke, I also use Fusion360 and would appreciate you sharing your current sub routines. Thanks mate.

EDITED for length...

I hope this helps. Feel free to ask any questions.

File Attachment:

File Name: linuxcnc_28082017.zip
File Size:27.57 KB

Hi Luke,

Great post. I too have a ER Collet gantry based CNC machine and use fusion 360 as well. Because you use a separate program for each tool, is it because of that that you do not use the M600 command?

Hey,
I tried merging this example in my config:
github.com/LinuxCNC/linuxcnc/tree/master...h-tool-length-switch
and it did not work for me. When I finally found out what signals are expected (at first I did not use the VCP) and where they should go I had it ask for tool after M6 Tn and "measure" it. Did anyone use it in real world? In theory it was good, but trying to touch off in G54 (I think used G10 p20 as I did before) and then doing another tool change resulted in need for another touch off and TLO grew along with G54 offset and tool at Z=0 was always above the material. I think it did not change after I discovered the reference tool signal...
It looked like the probing took the G54 offset together with actual TLO and this was no good, and since I can not do G53 G38.3 I found the way from the MF70 files - G59.3 coordinate system which was by default at machine zero (or should be?), anyway it is not moving. With this before the probing I also inserted G49 which cancels actual tool offset - this seems to fix rest of the problem.
I wonder if there is a better way to have the probing relative to hard machine coordinate system? G59.3 worked, but it is "sacrificed" to the probing fun, and could be used for other purposes.

The MF70 code did not work out ouf the box either, so I stick to the first example - I believe it is good and I like the way of configuring it in .ini - after a period of WTF i found out that I have to copy the FEATURES=30 too - it would have helped IF i started by looking at this thread instead of the example config as Andy pointed that out...

@ stidrvr: I believe there maybe was a change at some point and M600 may not be required in the current code, as the reference tool is indicated by being tool number 1. I am not even sure if that makes sense to always update the reference height when this tool is put in the collet. It looks like it can be any tool, and it has to be done at least once after restart so the reference length is not undefined - if everything works it should be possible to do the touch off with any tool and z=0 at the material should stay there. manual-toolchange-with-tool-length-switch has different approach, it expects the "reference tool" button/signal to be present after putting in the tool - if it is present the thing acts similar to using M600 as per this thread some 8 years ago.

All of this should be clear to me after some more testing and I will try to make some kind of a readme/tutorial on this as there is a lot of confusion and not much documentation, and an awful lot of collet spindles.

well, another question: what is the table enable supposed to do? Turn the VCP panel on, apply power to the probe switch on the table or what?