torch reference question.

[djreiswig]

Happy to help.

[acourtjester]

Ok from you pictures and what you said "when the torch is in the down position the senor rests on the plate beneath it and the led of the sensor is on, when you slide the torch up the led goes out and in mach3 the digitize signal is on then. and the digitize led is lit that means the G-code will need to have the command G31 Z that tells Mach to move the Z down until it trips that led/sensor. here is screen shot of short G-code the shows that command.

psot1.JPG

This is a Post processor and a short G-code that will look like it cuts a straight line for a few inches at a feed rate of 48 IPM that may work for you as it is setup for a Probe sensor and using the G31 Z command it is in a ZIP format you may need to get WinRar on you system to unpack it. It is a free program. You will need to copy the post processor into the folder the sheetcam has the post processors stored so you can then select it in sheetcam to use.

Mach3 STEVEplasma mod by tom THC Proma with probe ohnic touch.zip

[djreiswig]

acourtjester, I was wondering if that sensor might have some offset between when it touches the material and when the signal breaks. If it does, then G31 might not read correctly. That's why I was going with the G28.1 and an offset in the post. Thoughts?

Edit. I see you have a .002 Z raise built in. I guess that would be a round about way to handle some offset.

[cruz]

thanks acourtjester i downloaded the post processor.
i'll try it tomorrow out.
i'll update you guys on the progress.

[acourtjester]

That 0.002" off set was because the post processor for some reason needed a small off set but normally with the probe is does not.
I am using a different post processor (for the Price THC and the water switch sensor) do not need it. I use it for both plasma and router.
From here I cannot tell how the sensor is setup just that it was sending a sign to the probe (digital input), and that uses the G31 command.
We will see what happens in the morning. Remote troubleshooting is not alway accurate but we try
There may need to have a small offset as that is a proximity sensor, no real contact just gets very close to trigger a sign. I don't like to use them as they require power to each one you use.

[cruz]

okay did some testing today not a real success
tried some different post processors but none with success:
all of them had this issue that when i run the code in mach3.
the torch would go to the piercing point lower to the piercing height,
and then start going up or down (depending on the post processor) without stopping.
i don't know if the problem lies in the post processor or the mach3 setting with the home switch.
with the method i got from djreiswig, i the a switch of set value of 2,78mm.
could this be correct or isn't that possible?


here is a G-code from a post processor where the issue isn't there:

N0010 (Filename: bijna.tap)
N0020 (Post processor: Mach3 plasma.scpost)
N0030 (Date: 07/01/2019)
N0040 G21 (Units: Metric)
N0050 G53 G90 G91.1 G40
N0060 F1
N0070 S500
N0080 (Part: New part)
N0090 (Operation: Outside Offset, Shape, T3: staal 45A finecut 3mm)
N0100 M06 T3 F2700.0 (staal 45A finecut 3mm)
N0110 G00 Z15.0000
N0120 X48.3470 Y52.6015
N0130 Z3.8000
N0140 M03
N0150 G01 X50.0012 Y54.1995 Z1.5000 F240.0
N0160 X51.2238 Y55.3807 F2160.0
N0170 G02 X50.5312 Y56.1019 I123.1997 J119.0190
N0180 X54.7498 Y51.8359 I123.8924 J118.2978 F2700.0
N0190 X49.1585 Y57.5564 I119.6737 J122.5638 F1755.0
N0200 G03 X47.3494 Y57.6194 I-0.9360 J-0.8731
N0210 M05
N0220 G00 Z15.0000
N0230 M05 M30


and here is a G-code where the issue is there (torch going up or down without stopping)
this G-code came from the post processor provided by acourtjester, but other post processor from sheetcam had the
same issue => torch going up or down without stopping

N0010 (Filename: bijna.tap)
N0020 (Post processor: Mach3 STEVEplasma mod by tom THC Proma with probe ohnic touch.scpost)
N0030 (Date: 07/01/2019)
N0040 G21 (Units: Metric)
N0050 G53 G90 G91.1 G40
N0060 F1
N0070 S500
N0080 (Part: New part)
N0090 (Operation: Outside Offset, Shape, T3: staal 45A finecut 3mm)
N0100 M06 T3 F2700.0 (staal 45A finecut 3mm)
N0110 G00 Z15.0000
N0120 X48.3470 Y52.6015
N0130 Z3.8000
N0140 G90F30
N0150 G31 Z-50 F10
N0160 G92 Z0
N0170 G0 z0.010
N0180 G92 Z0
N0190 Z3.8000
N0200 M03
N0210 G01 X50.0012 Y54.1995 Z1.5000 F240.0
N0220 X51.2238 Y55.3807 F2160.0
N0230 G02 X50.5312 Y56.1019 I123.1997 J119.0190
N0240 X54.7498 Y51.8359 I123.8924 J118.2978 F2700.0
N0250 X49.1585 Y57.5564 I119.6737 J122.5638 F1755.0
N0260 G03 X47.3494 Y57.6194 I-0.9360 J-0.8731
N0270 M05
N0280 G00 Z15.0000
N0290 M05 M30

maybe the codes can help someone find a issue.

[cruz]

also here are some pictures from the setting in mach3 for the home switch:

IMG_20190107_131643.jpg

IMG_20190107_131702.jpg

and here is a pic from the code i got from acourtjester where the command G31 is given.

IMG_20190107_131750.jpg

maybe it helps someone.

[djreiswig]

Code looks okay. I can't see what port, pin is set to what. Left side of picture is cut off. If you use G31 you want the switch set to the probe input. If you use the G28.1 you want it set to z home. G31 doesn't use the offset.

Can you get the input to switch in diagnostics?

[acourtjester]

Well one problem is your table is running metric and my Post Processor is set to inches

[djreiswig]

I thought all of the posts were in metric.

[acourtjester]

I stand corrected The post I send was in inches but sheetcam will change if it is setup for one or the other and the g-code will be that way.

[cruz]

Code looks okay. I can't see what port, pin is set to what. Left side of picture is cut off. If you use G31 you want the switch set to the probe input. If you use the G28.1 you want it set to z home. G31 doesn't use the offset.

Can you get the input to switch in diagnostics?

tomorrow i'll take some better pictures.
what do you mean with switch the input to diagnostics?

[cruz]

I stand corrected

any idea why your post isn't working with my machine?
maybe the settings in mach3 for the home switch?

[cruz]

i used the automated set option when assigning the sensor to the Z-home.
it put it in port 1 and pin number 15.
should i do anything else with the "active low" and "emulated" options?

[acourtjester]

The post processor I sent is set up to use the Probe and in you image of the diagnostic page the digital led was on so that is why I sent the post processor for you to use.
Let check something else, position the torch about mid travel up/down, push the page down key on the keyboard. Z should move down as long as you have the key pressed. Now go to the MDI page, there is a place that you can enter a G-code command labeled Input, enter in G31 Z-50 Z then hit enter on the keyboard, Z should move down, stop it after you see which direction it moves. If it moves up then the home for Z needs to be change. This is done in the Homing/limits menu.
In Motor home/softlimits under Home N column. If it is a green check change it to a red X and then try the G31 command again.

[cruz]

The post processor I sent is set up to use the Probe and in you image of the diagnostic page the digital led was on so that is why I sent the post processor for you to use.
Let check something else, position the torch about mid travel up/down, push the page down key on the keyboard. Z should move down as long as you have the key pressed. Now go to the MDI page, there is a place that you can enter a G-code command labeled Input, enter in G31 Z-50 Z then hit enter on the keyboard, Z should move down, stop it after you see which direction it moves. If it moves up then the home for Z needs to be change. This is done in the Homing/limits menu.
In Motor home/softlimits under Home N column. If it is a green check change it to a red X and then try the G31 command again.

good tip!! i'll try it tomorrow.
thanks!

[acourtjester]

Cruz when you enter the G31 code in the input line be sure to have a - in the code so the Z will drive negative like G31 Z-50 F10

[cruz]

okay tried the code.
this is what i typed: G31 Z-50 and the torch went down, so that's alright.
here's a picture from the homing limits screen:

IMG_20190108_143303.jpg

and here are the better pictures from the input signals screen:

IMG_20190108_143354.jpg

IMG_20190108_143430.jpg

[acourtjester]

last thing to check is the native units, go to the setting page and look in the lower right and make sure the MM's led is lit.
Mine is set to inches as that is what I use.

home.JPG

[cruz]

i already checked that it's set in mm.
anything wrong with those settings in input signals?

[acourtjester]

I just went back to your post earlier and what you said does not make sense to me. The sensor in the image at the bottom of torch is not acting like a metal surface sensor but a torch movement sensor. For this to work that sensor needed to be in a position where when the torch is close to the metal surface when moving down will trigger the probe input signal.
It may be setup like a floating head switch so when the torch touches the metal and move up. And this causes the sensor to move away from the meat plate and the probe signal lights. But you say the torch does not stop and it gets knocked off the magnetic mount.

home 2.JPG

[cruz]

i'll upload some picture's to explain in a other way:
SENSOR 1: is the sensor for the magnetic breakaway.
if the plate just under the sensor moves, the machines sees that as a collision and stops everything.

SENSOR 2: is the sensor that i assigned to the Z-home switch.
when just let the torch rest in it's normal state the sensor touches the plate just under it and the led burns.
if you lift-glide the torch up the led goes out and the digitize led in mach3 goes on.

the 2 sensor are exactly the same both with a little led that is on when near the metal and of when the metal moves away.

IMG_20190106_173420.jpg

IMG_20190106_173337.jpg

[acourtjester]

If sensor #2 is attached to the Z home, it must be acting as a floating head switch and the Post processor I send will not work as it is setup of the probe. With that being said it needs to wired to the Z home not the probe. You need to move the pins in mach from the probe (set enable at the probe to red X and pin 0) go to Z home and set enable to a green check and port 1 and pin to 15. the check on the diagnostic page when you move the torch up the Z home lights, if it on with torch down change the Low active. I think this will work with G28 command.
here is a video showing how to set the switch offset in Mach, to move slowly hit the Tab key and the pendant will come up change Jog to step and put a value in the cycle jog step to about 0.2 MM and used the Z up/down keys to move the Z axis for this setting procedure.
https://www.youtube.com/watch?v=6CDml_kosbY

Mach3 plasma snippet Mod .035.zip

home 3.JPG

home 4.JPG

[cruz]

okay just to make sure i understood you correct:

- disable the probe (red cross on enabled)
- set pin number to 0
- go the Z-home and enable it (green mark)
- set port number to 1 and pin number to 15
- check in the diagnostic page that when i jog the torch up the Z-home light goes on.
if it doesn't=> change the low active setting of Z-home.

did i get everything correct?

also in the provided post should i change the "z0.040" to my switch offset?
or is the arrow pointing to something else?

[acourtjester]

yes on the ports and pin info
Well the way I look at it when the torch goes down and touches the metal surface and the z moves a little more down the Z home light should come on. When running a gocode the Z dro should then change to 0.0 and the torch should move up to the pierce height.
Yes the command line should be showing G0 Z xx (the zz is the value of the switch offset but you are using metric so what ever the metric value is) then save the changes. Look at the next G-code you create to see something like this.


N0260 G28.1 Z0.5 (Start Touch-Off ) The .5 needs to far enough in metric so the Z will drive down to the metal surface maybe like 30
N0270 G92 Z0.0 reset to zero
N0280 G00 Z0.001 (Switch Offset Lift) This is where your offset metric value should be used
N0290 G92 Z0.0 reset to zero
N0300 G00 Z0.150 set pierce height metric value metric value should be used
N0310 M03