James I have the same problem with the screen that you had , could you post how you fix it, tried every thing I could think of thanks for the help.
GaryB.
Most of the times when I activate z-zero routine the following action is executed: normal pause time- then suddenly instead of moving towards the touchplate the spindle moves (fast) upwards (away) from the touchplate to the safe z height from the tool origanal position. the same action is with the XY center
Do i need to enter the dimention/ thickness of the touchplate(Gauge Block) at the OFFSET screen in Mach 3.
Regards
I hope this is what you are asking. Not being a computer god like some of the other guys around here I miss read the directions and totaly missed the set. file. If this is not applyed properly it will not work. Read through the directions again. Thats how I figured out my mistake. Works great now!!!!! JamesOK! I am a moron!!! Some how I did not get the set file and did not under stand the directions. I am pleased to say that the screen is now in proper opperation!! I will try funtionality later on. Thank you all.
Thank you James, Will read and do again
Cheers
I made a new screenset today for Mach 3 that is the standard 1024 screenset
but with the Offset page expanded to include my Tool Probing buttons and DRO's.
It has the same
Auto Z Setting w/wo Touch Plate
Auto Edge Finding (X and Y)
Auto Corner Finding
Auto Center Finding with DRO Output
Auto OD Finding with DRO Output
You can download the zip here that includes the Hoss1024probing.set screenset,
bitmaps that go in the Mach3/Bitmaps/MillBitmaps folder,
the HossProbeCodesUpdate.zip that contains the text files with the button codes (they are already installed in the screenset)
and the hoss probing screenset.jpg preview.
Hoss
Gosh, you've... really got some nice toys here. - Roy Batty -- [URL]http://www.g0704.com[/URL]
It is connected to port 1, pin 10. Pin 10 had 5.0V on it and it is activated.
If I click any of the directions button on the auto center section it drives slowly in that direction until I click the Stop button.
If I take a wire and bridge it between GND and pin 10 on the BOB the probe test light doesn’t light. So that eliminates wiring from BOB to probe ends.
At one time it was working fine.
OK what’s the next step in troubleshooting?
Hager
Hoss,
That is a super screen.
I downloaded it and installed it on my CNC PC, all the functions work except the sensor touch. I have 5V on pin 10, but even if I jump pin 10 to the BOB GND I don't get a Led light.
If I make it Active High, the scn led lights. But it should be set to active low.
I attached a scn shot of my setup, any ideas?
Thanks
Hager
I installed the updates to Mach3 and setup my probe. This is on a hobbyCNC pro board. After some playing I touch the ref plate to my tool tip and the test probe light comes on. I try ref Z and it seemed to work. Did this a few times and all was well, but my Z retract ammount was very inconsistent. From .25 to .75 inches. I believe the script is trying to set it at .25 or around there.
I decided to make a cut that required tool changes. This was a great time to test out the probe. Once the first tool path completed I stopped the router, changed the bit and hit ref Z. The router came down, touched the pad and proceeded to try to drive the tool into the table. I wasn't sure what the problem was so I reset everything and tried a few more times. Everything seemed to work again. This happened one more time. I thought maybe I needed a Cap on the input line.
The next day I added the cap and tried out the ref Z while in the air, just incase something happened. Everything worked great the first few times, so we set the plate on a piece of 2" foam so it had a little give to it. Well as soon as I did this I had the same problem, bit gets jammed into the plate. While doing this I can see the light come on, sensing the probe touch, I'm not sure if the problem is in the first redrive to correct for over shot, or the last positioning call. And I think it has something to where my Z DRO is before I run the ref Z.
I've looked through a lot of posts on this and I've seen others report this, does anyone know whats going on? I'd hate to ruin another $20 bit.
Thanks Bob
G'day Bob
Sound to me like your zeroing script is not quite right.
Want to post it here so we can have a look?
Greg
Good morning Greg,
This is the script I'm using. I believe this is the same one I'm having problems with. This was copied from my home computer, and the problem is on the shop computer, but I believe I just copied this to a CD and installed it on the shop, so they should be the same. I'm going to check on this tonight. One other note it looks like the versions of Mach3 I'm running are different. The home computer is version 03.042.020, not sure about the shop.
Thanks Bob
PS this is the script I downloaded from this thread. It could be downlevel.
Rem VBScript to probe in the z axis
If GetOemLed (825) <> 0 Then 'Check to see if the probe is already grounded or faulty
Code "(Z-Plate is grounded, check connection and try again)" 'this goes in the status bar if aplicable
Else
Code "G4 P1" 'Pause 1 seconds to give time to position probe plate
PlateOffset = GetUserDRO(1151) 'Get plate offset DRO
CurrentFeed = GetOemDRO(818) 'Get the current feedrate to return to later
Code "F4" 'slow down feedrate to 4 ipm
Rem Probe in the z direction
ZNew = GetDro(2) - 2 'probe move to current z - 2 inches
Code "G31Z" &ZNew
While IsMoving() 'wait for probe move to finish
Wend
ZNew = GetVar(2002) 'read the touch point
Code "G0 Z" &ZNew 'move back to hit point incase there was overshoot
While IsMoving ()
Wend
If PlateOffset <> 0 Then
Call SetDro (2, PlateOffset) 'set the Z axis DRO to plate thickness
Code "G4 P0.25" 'Pause for Dro to update.
ZNew = PlateOffset + .25
Code "G0 Z" &ZNew 'put the Z retract height you want here
Code "(Z axis is now zeroed)" 'puts this message in the status bar
End If
Code "F" &CurrentFeed 'Returns to prior feed rate
End If
That looks right.
Is you machine grounded? I spend hours before I realized the machine wasn't plugged in (therefor not grounded)
I'll check tonight about the active low.
Hlombord,
If your asking "Is the router grounded" the answer is, it was not grounded very good through the plug, so I installed a ground from my control board to the router. The probe touch light come on consistently. I'm going to try a few more tests tonight and see if I can't narrow this down. I might try to single step through the script, if I can figure out how.
Thanks Bob
Chilly2k
It appears to me that there is a problem with the script which might be catching people out in certain circumstances.
There is no provision for if you are in G91 incremental mode. This is a modal command. So it stays in effect until you change it.
So if you happened to be in G91 then the probe move could set off in a direction you are not expecting. That is something I try to avoid in CNC. I don't like those sort of surprises.
Rem Probe in the z direction
ZNew = GetDro(2) - 2 'probe move to current z - 2 inches
Code "G31Z" &ZNew
While IsMoving() 'wait for probe move to finish
Wend
Change this section to,
Rem Probe in the z direction
DoOEMButton (1010)
Code "G4 P 0.2"
Code "G31 Z-1 F4"
While IsMoving()
Wend
This way it matters not which mode you are in.
Greg
Greg,
You may be on to something. I played around with this again last night. The script seems to work fine up to this point.
If PlateOffset <> 0 Then
Call SetDro (2, PlateOffset) 'set the Z axis DRO to plate thickness
Code "G4 P0.25" 'Pause for Dro to update.
ZNew = PlateOffset + .25
Code "G0 Z" &ZNew 'put the Z retract height you want here
Code "(Z axis is now zeroed)" 'puts this message in the status bar
End If
Code "F" &CurrentFeed 'Returns to prior feed rate
End If
It's during this reposition that the machine seems to take off. I couldn't get it to fail last night. (And it could be that I didn't run a program causing it to be in incremental mode). One thing I did notice is even with this line in
Code "G0 Z" &ZNew 'put the Z retract height you want here
The machine retracts to some random value. I thought this should always be .375 which is .125 (PlateOffset) +.25 At the end of the run my Z DRO should be .375 But it's all over the place. One time .478 the next .854 etc.
I've been a programmer for 24 years, so I know that there are things that can happen that are not easily documented. This is my first foray into Gcode, so that should help explain where my next question is coming from.
In Mach3 does the DRO represent the current position? Or is that keep somewhere else. I'm not sure how making the change you suggested would correct the problem.
Rem Probe in the z direction
ZNew = GetDro(2) - 2 'probe move to current z - 2 inches
Code "G31Z" &ZNew
While IsMoving() 'wait for probe move to finish
Wend
Change this section to,
Rem Probe in the z direction
DoOEMButton (1010)
Code "G4 P 0.2"
Code "G31 Z-1 F4"
While IsMoving()
Wend
Never mind I see it now.
I set up a test Gcode file to set G91. Then move Z to a neg value. The actual "Bad code" it the overshoot code.
ZNew = GetVar(2002) 'read the touch point
Code "G0 Z" &ZNew 'move back to hit point incase there was overshoot
While IsMoving ()
Wend
If the touch point is lets say -2. The "G0 Z-2" in incremental mode trys to send the bit 2 inchs (in my case) into the work. And if the touch point is + it raises the Zaxis that distance.
I can see now why my ending Z DRO is not always .375.
If PlateOffset <> 0 Then
Call SetDro (2, PlateOffset) 'set the Z axis DRO to plate thickness
Code "G4 P0.25" 'Pause for Dro to update.
ZNew = PlateOffset + .25
Code "G0 Z" &ZNew 'put the Z retract height you want here
Code "(Z axis is now zeroed)" 'puts this message in the status bar
End If
First we set the Z DRO to .125
Wait .25 seconds
Znew is set to .125 + .25 or .375
Now we move the z axis up .375. Not to .375 So .125 + .375 = .500
While simulating this it's always ending up .500. On the real machine it's all over the place.
Is there a way to query the coordinate state (incremental Vs absolute)? You could then save that set to absolute (G90) run the script and reset.
Worst case, I may just add the G90 to the front of the script. So far, and I'm just starting, I don't do tool changes in the middle of a program run. So setting it to absolute mode should not cause a problem.
Which ever solution I use will have to be applied to all of the scripts in the probe section.
Thanks for the help.
Bob
I am not saying that will fix your problem. What I meant is that if you happened to be in G91 and Z was at greater than 2" then you would get a G31 in the wrong direction.
From what you and a few other posters were describing I thought you may be running into that issue.
You could include a G90 but then it should be retuned to original state at the end. Far simpler to just use DoOEMButton (1010) That zeros the Z DRO and so covers either state.
Here is one that I and many others use every day,
CurrentFeed = GetOemDRO(818) 'Get the current feedrate to return to later
PlateThickness = GetUserDRO(1151) 'Z-plate thickness DRO
If GetOemLed (825)=0 Then 'Check to see if the probe is already grounded or faulty
DoOEMButton (1010) 'zero the Z axis so the probe move will start from here
Code "G4 P2" ' this delay gives me time to get from computer to hold probe in place
Code "G31Z-1 F4" 'probing move, can set the feed rate here as well as how far to move
While IsMoving() 'wait while it happens
Wend
ZProbePos = GetVar(2002) 'get the axact point the probe was hit
Code "G0 Z" &ZProbePos 'go back to that point, always a very small amount of overrun
While IsMoving ()
Wend
Call SetDro (2, PlateThickness) 'set the Z axis DRO to whatever is set as plate thickness
Code "G4 P0.25" 'Pause for Dro to update.
Code "G0 Z1" 'put the Z retract height you want here
Code "(Z axis is now zeroed)" 'puts this message in the status bar
Code "F" &CurrentFeed 'Returns to prior feed rate
Else
Code "(Z-Plate is grounded, check connection and try again)" 'this goes in the status bar if aplicable
Exit Sub
End If
As you well know if you ask ten people to write code to do a simple task like this you will get ten different codes. Does not make one right and others wrong.
However I do think that G90 G91 issues should be covered.
By the way I did not write this one, I just modified someone else's till I liked it.
Greg
Greg,
Thanks for the explanation. Yes, After looking at the G-code lazycam is generating I believe I'm a victim of a G91 setting. I only question this section of code.
DoOEMButton (1010) 'zero the Z axis so the probe move will start from here
Code "G4 P2" ' this delay gives me time to get from computer to hold probe in place
Code "G31Z-1 F4" 'probing move, can set the feed rate here as well as how far to move
While IsMoving() 'wait while it happens
Wend
ZProbePos = GetVar(2002) 'get the axact point the probe was hit
Code "G0 Z" &ZProbePos 'go back to that point, always a very small amount of overrun
While IsMoving ()
Wend
If you assume we're in incremental mode, we
Rest the dro to zero.
pause
goto 0-1 at a speed of 4 until the probe is hit.
get position Lets say it's -.50 with no overshoot
goto current position+probe position. <--- This is the question Won't this now goto -1 Current position -.5 +probe position -.5?
wait for the move to finish
Won't this still be a problem?
Thanks Bob
No if you look at the code it is more like this,
Reset the dro to zero.
pause
goto 0-1 at a speed of 4 until the probe is hit.
get the variable and return to it 'this variable is where it hit the plate
set the DRO to plate thickness ' variable is now forgotten
go to retract height
Greg
Last edited by Greolt; 03-05-2009 at 09:22 PM.