Tool touch off issue (Resolved)

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

Gary Campbell
Posts: 1491
Joined: Sat Nov 18, 2017 2:32 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: Acorn 238
Location: Marquette, MI
Contact:

Re: Tool touch off issue

Post by Gary Campbell »

Some of the "Auto Z to Plate" macros dont use the internal functions. Try setting "Subtract Height" to NO and dont enter a height. This only applies to macros that have a variable that is set to the Z plate thickness.

When these macros are used AND the internal parms are set, the height may be getting subtracted twice
GCnC Control
CNC Control & Retrofits
https://www.youtube.com/user/Islaww1/videos
neowalla
Posts: 30
Joined: Sun Feb 21, 2021 5:06 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: E415F6F8DF80-0217212488
Location: Windsor, Ontario Canada
Contact:

Re: Tool touch off issue

Post by neowalla »

I appreciate your concern but first I don't even see where to download and install this program. Then I have to spend the time to configure it. With my old controller, I held down one button, pressed another, and the tool touched off the brass puck and I was done. That is all I am looking for here with the Acorn. Right now the Acorn does this; it just sets the Z 0 12mm too high. For whatever reason it is not subtracting the thickness of the brass TT puck so I guess I have to do it manually. I'm not a machinist making parts for NASA. I build guitars out of wood. I don't need fancy probes and automation. Just set the Z0 to the top of a chunk of wood.
swissi
Posts: 471
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Tool touch off issue

Post by swissi »

neowalla wrote: Sat Apr 03, 2021 1:20 pm I appreciate your concern but first I don't even see where to download and install this program. Then I have to spend the time to configure it. With my old controller, I held down one button, pressed another, and the tool touched off the brass puck and I was done. That is all I am looking for here with the Acorn. Right now the Acorn does this; it just sets the Z 0 12mm too high. For whatever reason it is not subtracting the thickness of the brass TT puck so I guess I have to do it manually. I'm not a machinist making parts for NASA. I build guitars out of wood. I don't need fancy probes and automation. Just set the Z0 to the top of a chunk of wood.
I'm sure people at NASA do appreciate your guitars :-)

The macro file being used for the "Auto Z to Plate" button is mfunc44.mac.
These are the lines that set WCS Z0:

Code: Select all

N250 ;Probe TT1

M115 /Z P[#104] F[#102] ;Move at fast probing rate until TT1 detected
G91 Z#9013 F[#102] ;Move up the distance set in P13.
M115 /Z P[#104]F[#103] ;Move at slow probing rate until TT1 detected
G90

G92 Z[ABS[#9071]] ;Set Z pos
The macro does a fast probing speed first followed by a slow probing speed. Looking at your puck it doesn't look like it is solid and does have a spring loaded surface. I would be concerned about my tools hitting a solid puck at fast probing speed and I would remove the first M115 /Z move and the G91 Z#9013 retract line that follows and just keep the slow speed M115 /Z line.

The line "G92 Z[ABS[#9071]] ;Set Z pos" does reset the currently active WCS# to the height of your puck configured in parameter 71 which is -12mm. It doesn't really matter if the value of parameter 71 is +12mm or -12mm because the script is using the absolute value of parameter 71 which is the 12 meekest needed.

That means your DRO for the Z axis should display +12.000 after you touched off your tool and Z0 is exactly on the surface where your puck is sitting on.

If this is not what's happening, please post a screen shot of the full screen of CNC12 when the tool has been touched off on the puck (tool still sitting on top of the puck) and also a picture that shows your tool on top of the puck.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
neowalla
Posts: 30
Joined: Sun Feb 21, 2021 5:06 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: E415F6F8DF80-0217212488
Location: Windsor, Ontario Canada
Contact:

Re: Tool touch off issue

Post by neowalla »

Ok I tried what Gary suggested first. I got the attached error. It would not go away with rebooting so i re-installed CNC12 as the error instructed.
After that and restoring from my last report, in the wizard I set the subtract height to no but got the other attached error about param 71.
swissi, my TT puck is solid brass, no spring, but the downward movement is extremely slow anyway so there is no danger of the tool crashing into it when using the auto Z to 0 function.
My DRO does indeed show +12 after the touchoff but when I run a test job, it cuts air at what looks like about 12mm above the workpiece. So it is not subtracting that 12mm. If I manually subtract 12mm, then hit "SET WCS Z0" and run the job, it cuts material like normal.
CorrectionIt does not cut at "normal" depth. It cuts air for a little bit then as the toolpath progresses, it cuts material but not to the proper depth.
Now I need a better test. I'm running test files I made in Fusion 360. Fusion itself sometimes creates toolpaths that "cut air" for a short time while it ramps the tool down and these are the first toolpaths with a Centoid post processor. I don't really know gcode well enough to write something in it, but I will make a job in Vcarve of a simple circular pocket at a depth of say 10mm and try that out. Vcarve's toolpaths are much simpler than Fusion's.
Attachments
20210405_114259.jpg
fullscreenTT.PNG
param71Error.PNG
wizard error.PNG
swissi
Posts: 471
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Tool touch off issue

Post by swissi »

neowalla wrote: Mon Apr 05, 2021 11:47 am Ok I tried what Gary suggested first. I got the attached error. It would not go away with rebooting so i re-installed CNC12 as the error instructed.
After that and restoring from my last report, in the wizard I set the subtract height to no but got the other attached error about param 71.
swissi, my TT puck is solid brass, no spring, but the downward movement is extremely slow anyway so there is no danger of the tool crashing into it when using the auto Z to 0 function.
My DRO does indeed show +12 after the touchoff but when I run a test job, it cuts air at what looks like about 12mm above the workpiece. So it is not subtracting that 12mm. If I manually subtract 12mm, then hit "SET WCS Z0" and run the job, it cuts material like normal.
CorrectionIt does not cut at "normal" depth. It cuts air for a little bit then as the toolpath progresses, it cuts material but not to the proper depth.
Now I need a better test. I'm running test files I made in Fusion 360. Fusion itself sometimes creates toolpaths that "cut air" for a short time while it ramps the tool down and these are the first toolpaths with a Centoid post processor. I don't really know gcode well enough to write something in it, but I will make a job in Vcarve of a simple circular pocket at a depth of say 10mm and try that out. Vcarve's toolpaths are much simpler than Fusion's.
If you place the puck onto the surface of your stock, touch off the tool on top of the puck and the DRO shows Z +12.000, then everything works as it should. WCS Z0 has been set on the bottom of your puck which is the top of you stock.

Now if your machine is cutting above the stock, then the WCS Z0 point of your model has not been set on top of the stock or another possibility is that the height offsets of your tools in the CNC12 tool offset library are not set to 0. Make sure all the H values of all 200 tools are set to 0 if you don't have a spindle with fixed tool holding.

If this still doesn't work as expected, please post a fresh report file as you have made many changes since you posted the original one.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
neowalla
Posts: 30
Joined: Sun Feb 21, 2021 5:06 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: E415F6F8DF80-0217212488
Location: Windsor, Ontario Canada
Contact:

Re: Tool touch off issue

Post by neowalla »

Ok I made a simple toolpath in Vcarve Pro. WCS zero is centre of stock, top of material. The toolpath consists of a circle pocket 10mm deep.
I ran the auto Z to plate script and then ran the job. It cut air. So it is not just a Fusion thing. It thinks the workpiece surface is 12mm higher than it is (the thickness of the brass puck).
I then jogged Z down -12 manually, re-set WCS Z to 0 and re-ran the job. It cut to a depth of 5mm, half of what the toolpath calls for. There is more wrong than just the auto Z to plate script.

On a side (post processor) note, After the Vcarve job was complete, the machine behaviour is what it always used to be, and what I like it to be. Z retracts. the spindle powers down, but otherwise the X and Y axes do not move. When it finishes a Fusion job it returns to machine 0 and the spindle doesn't begin to wind down until all the axes have homed. Not what I want.
I attached new report.
Attachments
report_E415F6F8DF80-0217212488_2021-04-05_16-00-24.zip
(762.97 KiB) Downloaded 6 times
tblough
Posts: 1401
Joined: Tue Mar 22, 2016 10:03 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: Yes
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192
Location: Boston, MA
Contact:

Re: Tool touch off issue

Post by tblough »

Upload the VCarve program and the Fusion program you are trying to run.
Cheers,

Tom
Confidence is the feeling you have before you fully understand the situation.
I have CDO. It's like OCD, but the letters are where they should be.
neowalla
Posts: 30
Joined: Sun Feb 21, 2021 5:06 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: E415F6F8DF80-0217212488
Location: Windsor, Ontario Canada
Contact:

Re: Tool touch off issue

Post by neowalla »

Hi Tom,
The Fusion 360 file is a wiring channel for a Gibosn Les Paul-style guitar. It's a straight slot with ends that match the radius of the 1/2 inch bit, 12.7mm deep. I cut the test in styrofoam so an accurate depth measurement isn't really possible but it measures approximately half the depth is should be so it seems to be behaving the same as the Vcarve file in terms of cut depth.
Attachments
op2 .5 EM.nc
Fusion 360
(2 KiB) Downloaded 4 times
large pocket.cnc
Vcarve Pro
(2.6 KiB) Downloaded 2 times
tblough
Posts: 1401
Joined: Tue Mar 22, 2016 10:03 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: Yes
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192
Location: Boston, MA
Contact:

Re: Tool touch off issue

Post by tblough »

Well, both programs are using G54 (OP2 calls it out, pocket does not call a WCS but your last report has it at G54). Both programs are calling T1 and using H1, but from the speeds and feeds, they seem like they are different tools, but using the same height offset.

The fusion job has a N420 G28 G91 X0. Y0. return to reference point move. If you don't want it to return to machine 0, then you need to remove this line.
Cheers,

Tom
Confidence is the feeling you have before you fully understand the situation.
I have CDO. It's like OCD, but the letters are where they should be.
swissi
Posts: 471
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Tool touch off issue

Post by swissi »

neowalla wrote: Mon Apr 05, 2021 3:42 pm Hi Tom,
The Fusion 360 file is a wiring channel for a Gibosn Les Paul-style guitar. It's a straight slot with ends that match the radius of the 1/2 inch bit, 12.7mm deep. I cut the test in styrofoam so an accurate depth measurement isn't really possible but it measures approximately half the depth is should be so it seems to be behaving the same as the Vcarve file in terms of cut depth.
Are you sure your Z travel distance is accurate. When you touch off a tool on your puck and the DRO shows Z +12.000 and you then jog down to Z0, does the tool touch the surface? If not then your turn ratio is setup incorrectly.

Regarding the Fusion 360 Post Processor, if you are setting up a machine profile in Fusion 360, the machine will always go to the X and Y coordinates configured in that machine profile, overwriting any selections a post processor does provide as an option.

If you are using my Post Processor customized for Centroid CNC12, you can select in the properties of the PP at what position you'd like your X and Y axis to go at the end of a job but as I mentioned above, this does not work if you have setup a machine profile and looking at your output, it looks like you did so.

You can get the Fusion 360 Post Processor from this Post.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Post Reply