Quote from: rrc1962 on July 31, 2011, 05:47:59 PM

What's your X and Y acceleration set at?  G31 uses that, not the axis that the G31 is using.  If you have a slow accel and a high probe feedrate, it WILL take forever to stop.

If that's the case, it's a serious bug that needs to be reported to Brian.

I'm reminded of it every time I reset acceleration so X and y are significantly lower than Z.  Perhaps someone who is doing G31 probing can verify.  Just reset the X and Y acceleration to something very slow...like 5 or less,and set the Z at 30 or 40.  Run a G31, then bump the X and Y back up and see if the G31 accel increases.

I mentioned it back in 2009 in this thread....

http://www.machsupport.com/forum/index.php/topic,13364.0.html

Hi rrc1962 - Just tried this on my R3.042.020 and G31 uses the correct axis accel setting. Is this a version issue maybe?

Ian

I'm on 3.043.022.  I'll test some more but I noticed it again yesterday when I slowed the X and Y way down. 

I tested again today.  I set all accels at 50 and did a G31 Z-1.  Motion was as expected for an accel setting of 50.  I then reset the X and Y accel to 5 and did the same G31 Z-1.  Accel was very slow on the G31.  I reset X and Y back to 50 and the G31 returned to normal.  Seems like it's definitely using the accel setting from another axis.  I normally run all accel settings fairly close to each other and fairly high, so this is not an everyday issue.

Just loaded 3.043.022 and tried it and accel follows the correct axis just fine for me.

Ian

EDIT: Now back to 3.042.020 - can't be doing with that slower screenset loading...

ok, my script is as follows
PierceHeight = GetUserDRO(1000)
CutHeight = GetUserDRO(1001)
PierceTime = GetUserDRO(1002)

If GetOEMLed(825) = 0 Then
Code "G31 Z-4 F30"
While IsMoving()
Wend
CurrentZ = getDRO(2)
ProbeTrip = GetVar(2002)
SetDro(2,-((ProbeTrip - CurrentZ) + 0.15))

Code "G0 Z" & PierceHeight
While IsMoving()
Wend
DoSpinCW()
While Not isActive(Input1)
Wend

Code "G4 P" &PierceTime 'Pierce Delay
Code "G0 Z" & GetUserDRO(1001)
While IsMoving()
Wend

Else
Code "(Torch is On Surface Hit STOP and Fix)"
End If
Here is the video
http://www.youtube.com/watch?v=2CPgk_kCH20

It does the same thing if I just issue a G31 command by itself


Thank
Dave

Not sure if this is your particular problem or not but whenever you SET a DRO via CB and then do something that depends on the value of that DRO you MUST do a check via isMoving() that Mach HAS actually finished updating the DRO before you continue your script.

Ian

What are the motor settings accell/vel  and what is the turns per inch on your feedscrew for the Z?

  It looks and sounds like you are combatting inertial overrun and having to run slow accel rates to avoid loosing steps. Common with useing High speed stepper values to make axis speed.

As Stirling noted The Macro needs a few more checks / wait points in order to insure it stays in sync. NOTE:Some machines require it some get away with out it. It all depends.


AS a reference(;-)

In the Gcode side all that is replaced with

G31 Z-5 F20
G92 Z0
G0Z.080
G92 Z0
G0Z.100

M3
G4 P1

And is only run after the machine has moved a predeteremend amount of travel. Not at every piercing.

To do what you do it would look similar to this and there is NO CB involved in the motion code. The macropump will keep the #vars up to date with your DRO entries.


G31 Z-5 F20
G92 Z0
G0Z#500
G92 Z0
G0 Z#501

M3
G4 P#502

On a side note(;-)   This brings up one of the reasons that many choose to use the G28.1 method to find the TOM (top of material). The G28.1 cycle stops on contact THEN backs up to reset the switch. This takes out the overun, loss motion, switch travel and material flex variables. When the cycle stops you are at the TOM all that is needed is to Set Z, move to pierce hieght and go.

The G28.1 speed is also presettable in config as a percentage of Rapid.

What you do loose with it is the ability to use the G68 to do coord rotation as the G28.1 will NOT run in coord space. AND it does NOT error out, it just hops over it and continues the Gcode  (that needs fixin to allow Z to home in G68)

Just a thought, (;-) TP

My accel setting it 15 and the screw is 12 TPI. The motor is a 287 ozIn with a G540 and 48 volt PSU.
The rapid jog stops almost instant, and it is set to 150 IMP