[Gururaj]

Hi All,

This thread was very helpful in putting my Z touch-off probe in place. Thought to share some small information to great minds here.
My Z-axis was moving down slowly towards the ground plate, touching it, and used to sit on the plate without rapidly moving away as programmed in the classicladder. After spending lot of time, I found that the third MDI command was commented out. Un-commenting the following line in custom_postgui.hal made my Z-probe to work as expected.
net rapid-away classicladder.0.out-02 => halui.mdi-command-02

Ho yeah, I also added debouncing for the probe to avoid noise/mdi errors, as many have suggested in the earlier thread. Following were the changes I did in my main.hal file.

#added for probe debouncing
loadrt debounce cfg=2
setp debounce.0.delay 200
addf debounce.0 base-thread
#end of probe debouncing

#Commented out the existing configuration
#net probe-in => motion.probe-input
#net probe-in <= parport.0.pin-13-in-not

#added for probe debounce
net debounce-probe-in debounce.0.0.in <= parport.0.pin-13-in-not
net probe-in debounce.0.0.out => motion.probe-input
#end of probe debounce

Hope this helps

-Regards,
Gururaj
ideaguru

[Paulnd]

sorry I have been gone for awhile. Yea i'll upload the files, you need the input wire ran and the probe port turned on.

shoot me a email, seeing that I check it more regularly when you get this reply and i'll send the files.

[email protected]

Hello,

Does anyone have the O code files please? I've sent an email to strokercrate but haven't received a reply. I'll be very grateful if someone could upload or send the files to me please.

thanks

[Paulnd]

sorry I have been gone for awhile. Yea i'll upload the files, you need the input wire ran and the probe port turned on.

shoot me a email, seeing that I check it more regularly when you get this reply and i'll send the files.

[email protected]

Hello,

Do anyone have the O code files to share please? I have emailed strokercrate but have not received a reply yet.

thanks in advance

[strokercrate]

Hello,

Do anyone have the O code files to share please? I have emailed strokercrate but have not received a reply yet.

thanks in advance

I haven't received a email about the O codes in a couple of months, and those I replied to.

Try again, [email protected]

Also, you could just post your email and I could fwd them.

Thanks

[Paulnd]

Ah, just realised that I misspelled your email address! Sent you another one

[Paulnd]

If it doesn't work, my email is pdumke at gmail dot com. Thanks

[Paulnd]

I received your email, thanks. Unfortunately there was no zip file attached

[WJHildreth]

After reading this thread several times, digging around and using the tutorial at For Science » LinuxCnc ? Touch plate ? Part 2 I have managed to learn more about HAL, HALUI, and classic ladder than I ever thought I could. Just wanted to thank all of you for your hard work. But I do have one question and don't know if it is even possible.

If I do a manual touch off the display of the plot of my gcode will move to the new location. This is a great visual indicator of the touch off happening. When I use the touch off button from this thread, the offsets are set but the plot stays in it's original location. Is it possible to get the plot to move when the touch off is set like in manual mode? I just think it would be a great visual indication that all is working as expected.

Thanks,

Joe Hildreth

[pippin88]

strokercrate kindly provided the code for me to get my touch plate going. It's great.

I've written an article: 7xCNC - Minilathe CNC :: LinuxCNC Probing / Touch Off
I think O codes are the easiest way to get it going.

[WJHildreth]

Pippin,

Just looked at your article. So, this method removed the ladder program and replaces it with a sub-routine. Nice and clean!! Thanks for sharing it. One question. If the probe does not make contact, what happens after you get the error message? Does it just return from the sub-routine without running any more G-Code, Or does it continue to set the offset reguardless?

Many thanks again for sharing!

Joe

[strokercrate]

Pippin,

Just looked at your article. So, this method removed the ladder program and replaces it with a sub-routine. Nice and clean!! Thanks for sharing it. One question. If the probe does not make contact, what happens after you get the error message? Does it just return from the sub-routine without running any more G-Code, Or does it continue to set the offset reguardless?

Many thanks again for sharing!

Joe

You have to set the search distance in the 100.ngc file, if your Z travel is say 6 inches that should be your search distance, or if you go in mm and your Z travel is say 15mm the search should be set about the same, of course it doesn't have to be exactly that much accounting for a bit, but close enough.

[rotccapt]

hi all i was wondering if you could help me get my machine going with a touch off plate. i fallowed the instructions on the web sit listed and i though i did everything right but now linuxcnc will not start i got the error message

Debug file information:
Can not find -sec MOT -var MOT -num 1
Can not find -sec IO -var IO -num 1
Can not find -sec LINUXCNC -var NML_FILE -num 1
Can not find -sec EMC -var NML_FILE -num 1
custom_postgui.hal:4: Pin 'pyvcp.o100' does not exist
6098
PID TTY STAT TIME COMMAND
6149
PID TTY STAT TIME COMMAND
Stopping realtime threads
Unloading hal components

can anyone help me resolve this issue attatched are all the files that were modified except the 100.ngc

thank you for your time

[pippin88]

rotccapt. Slow reply, sorry.

The problem is your custompanel.xml
You've commented out (<!-- and -->) all the actual code, and you've doubled up on the xml and <pyvcp> tags.
The whole file should be:

<?xml version='1.0' encoding='UTF-8'?>
<pyvcp>
<button>
     <halpin>"o100"</halpin>
     <text>"Touch Off Z"</text>
     <font>('fixed',10)</font>
</button>
</pyvcp>

If you have other functions on your pyvcp you just need:

<button>
     <halpin>"o100"</halpin>
     <text>"Touch Off Z"</text>
     <font>('fixed',10)</font>
</button>

in there somewhere.



In other news I've got a guide on finding a corner with LinuxCNC and NGCGU

[rotccapt]

thank you for the reply i did get linux cnc back up and running with the new button but the function still does not work when i click the button i get another error saying that "can not open file <100> im not sure if it might have something to do with creating the file in windows or what not. i opened hal monitor and i do see that the pin is active but it still does not work. i have not played with it in a while though. my problem was in the custom panel and i ended up deleting everything in the file and starting over but thanks for the help.

[folc]

hello

[pippin88]

folc,

I'm not sure what the problem is exactly (I'm unclear what you want and what is wrong.)

Can you post your files please?

So you want a single virtual control panel button to run lines of GCode?
Do you have your gcode in an o subroutine file, or specified in the ini?

And to be clear on the code you want to run, my understanding of it is:

G21 (mm mode)
G91 G38.2 F450 Z-60 (incremental mode, probe to Z-60 from current position at 450 feed)
G90 G0 Z[#5063+2.5] (absolute mode, rapid to 2.5 above probe trigger)
G91 G38.2 F150 Z-13.5 (incremental, probe at slower speed of F150 to Z-13.5)
G90 G0 Z[#5063+1.52] (absolute, rapid to 1.52 above Z probe trigger point)
G10 L20 P1 Z3.04 (set G54 Z to 3.04)

I'm a bit confused about why you rapid up after the second probe, before actually setting the value in the coordinate system?

[folc]

So you want a single virtual control panel button to run lines of GCode?
Do you have your gcode in an o subroutine file, or specified in the ini?

Yes, I want to run series of lines of G-code by presing on single button, and YES i have my G-code stored in my .INI file as "MDI_COMMAND = G21" and then next line "MDI_COMMAND = G91 G38.2 F450 Z-60" etc.

And to be clear on the code you want to run, my understanding of it is:

G21 (mm mode)
G91 G38.2 F450 Z-60 (incremental mode, probe to Z-60 from current position at 450 feed)
G90 G0 Z[#5063+2.5] (absolute mode, rapid to 2.5 above probe trigger)
G91 G38.2 F150 Z-13.5 (incremental, probe at slower speed of F150 to Z-13.5)
G90 G0 Z[#5063+1.52] (absolute, rapid to 1.52 above Z probe trigger point)
G10 L20 P1 Z3.04 (set G54 Z to 3.04)

I'm a bit confused about why you rapid up after the second probe, before actually setting the value in the coordinate system?

Rapid UP is there for safe removing my PCB plate, so that there is no fizical contact while draging copper PCB plate out from end mill.
1.52mm = ticknes of the PCB plate
G10 L20 Z3.04 = ticknes of the PCB plate (1.52mm) + 1.52mm above plate = 3.04MM so end mill ends exacly 1.52mm above PCB touch off plate and 3.04mm off the part that i want to mill.

[pippin88]

I suggest following my guide 7xCNC - Minilathe CNC :: LinuxCNC Z Touch Off Plate

Each MDI command in .ini is separate and needs to be called with it's own halui.mdi-command-xx (where xx is 00, 01 etc corresponding to the commands position in the list in the ini). I'm not sure what happens if you try to call multiple MDI command at once.

You need the commands in a subroutine (an o file). It's in my guide.

[folc]

I suggest following my guide 7xCNC - Minilathe CNC :: LinuxCNC Z Touch Off Plate

Each MDI command in .ini is separate and needs to be called with it's own halui.mdi-command-xx (where xx is 00, 01 etc corresponding to the commands position in the list in the ini). I'm not sure what happens if you try to call multiple MDI command at once.

You need the commands in a subroutine (an o file). It's in my guide.

i was just trying to set up my Z touch off by your guide for past hour, what i did is that i comment your 2 lines in custom.hal

#net deb-probe-in debounce.0.0.in <= parport.0.pin-13-in-not
#net probe-in debounce.0.0.out

because i was getting the error that probe is already activated (I did that with StepCONF wizard)

then i managed to do 100.ngc program and call sub program with custom button. Everything works great.
The problem now is G-code ... i want 2 touches ... 1st rapid 2nd slower ...

what would be the right G-code to make the same efect like if you would click "Touch Off" buttom who is already build in LinuxCNC for TouchOff Z axis ..

what i writed ... is that good ?

#1 = 1.47 (PLATE THICKNESS)
#2 = 2 (UP OFF PLATE FOR 2ND TOUCH)
#3 = 8.53 (Distance to retouch)

G21 (metric)

(DEBUG,CHANGE TOOL AND PLACE TOUCH PLATE UNDER TOOL THEN PRESS START TO CONTINUE)
G10 L20 P0 Z0
G38.2 Z-40 F250
G90 G0 Z[#5063+#3]
G91 G38.2 Z-40 F15
G10 L20 P0 Z#1
G90 G0 Z[#5063+20]

(DEBUG,REMOVE TOUCH PLATE AND PRESS START TO CONTINUE)

yours ... what must i add that at 1st touch it moves 2mm above PCB plate and then slowley retouch and then agen move to the hight 10?

o100 sub
( Set current Z position to 0 so that we will always be moving down )
G10 L20 P0 Z0
( Probe to Z-10 at F25 [Uses machine units, I work in mm, this is meant to be slow!] )
G38.2 Z-10 f25
( Set Z0 at point where probe triggers with offset of +1.47 [this is the thickness of my PCB plate. You must adjust this for your plate / setup] )
G10 L20 P0 Z1.47
( Rapid up to Z10 above the material )
G0 Z10
o100 endsub

[pippin88]

Your code looks ok. You need 'o100 sub' at the start and 'o100 endsub' at the end. Try your code.
However you don't actually use #2.
Also your rapid up at the end should just be G91 G0 Z20 because Z0 has been set to the correct height already

I would do:

o100 sub
#1 = 1.47 (PLATE THICKNESS)
#2 = 2 (UP OFF PLATE FOR 2ND TOUCH)

G21 (metric)

(DEBUG,CHANGE TOOL AND PLACE TOUCH PLATE UNDER TOOL THEN PRESS START TO CONTINUE)
G10 L20 P0 Z0 (sets current position as Z0)
G38.2 Z-40 F250 (fast probe down to Z-40 at lowest)
G90 G0 Z[#5063+#2] (rapid back up to 2units above probe trigger point)
G91 G38.2 Z-3 F15 (slow probe down, note it only probes a little lower than the rapid up)
G10 L20 P0 Z#1 (set Z0 based on plate thickness)
G90 G0 Z20 (rapid up to Z20)
o100 endsub

(DEBUG,REMOVE TOUCH PLATE AND PRESS START TO CONTINUE)

If you have further problems please attach your .ini, .hal and custom_postgui.hal