Probe process help please

[bhdavis]

When I purchased my system upgrade parts from CNC4PC I also bought the Wildhorse Innovations Econo Probe. I'm now trying to get that running in UCCNC for simple, basic Z-axis touch down only. I don't anticipate ever needing the 3D side probing capabilities of this. Now that I see the system I think a simple 1" thick aluminum block as I've had on past machines would have been all I needed for a probe.

I've got the CNC4PC probe control card installed and the probe is connected. Touch the spring loaded button on the probe and all indicators activate in UCCNC and on the probe itself.

I've loaded the probe plugin in UCCNC.

When I use the PROBE button on the UCCNC main screen the Z-axis drops and touches the probe. It then retracts upward and then goes down and touches the probe a second time. Then the Z-axis retracts all the way up and hits the Z-axis limit switch, thus triggering the UCCNC RESET button. No change appears to take place in the Z0 location after doing this.

I've tried typing G31Z0 in the MDI window and this makes the probe go down. However it jams into the spring loaded probe button and does not retract upward.

When I try to use the probe from the TOOLS, PROBE screen I get a MACHINE NOT HOMED error message even after homing the machine from there.

I have read the manual (Information button on the probe screen) and tried setting up the parameters there. Again I can't get anywhere because of the "machine not homed" error message.

At this point I have an hour or two into trying to figure out how this is supposed to work. Can anyone give me the basics that I'm missing ?? Again, all I want to be able to do is touch down to set Z0 on my material thickness.

Thanks,
BH

[dezsoe]

The probe button on the main screen calls the M31 macro and that is independent from the probe screen and plugin. If you want to use the probe screen then you have to press the start probing button on the probe screen.

If you have only the 3D probe then it's not easy to use for Z height probing unless you have your tools in tool holders, you have the tool lengths set in the tool table and use G43.

On the probe screen if you have the probe tool mode selected then you need to have your axes homed. However, if you use the UCCNC version 1.2111 and you have slaved axes then you'll have problems. (There was a bug in the probing plugin which is already fixed.) I advice you to update to 1.2113.

Please, write more details.

[bhdavis]

Thanks for the reply. Please ask anything else that you feel is pertinent and I'll try and answer.

The probe button on the main screen calls the M31 macro and that is independent from the probe screen and plugin. If you want to use the probe screen then you have to press the start probing button on the probe screen.

Thanks, from my reading online I was aware that the button on the Main screen is independent of the probe screens and calls up the M31. I didn't realize there was an M31 macro. I just took a look at that and will try editing it by altering what may logically appear related to my experience. Question 1: What does the word "double" do in each of the first 6 or 8 lines?

When I tried using the START PROBING button on the probe screen that is when I got the "machine not homed" error message even though it was homed.

If you have only the 3D probe then it's not easy to use for Z height probing unless you have your tools in tool holders, you have the tool lengths set in the tool table and use G43.

I only have the CNC4PC C48 probe card and the Wildhorses Innovations Econo Probe. I'll have to see if I can plug an aluminum block with an alligator clip to the bit into the C48, and do a probe that way. The Econo Probe is WAY to tall anyway. I don't have enough Z-lift to be able to use it with longer bits. I do not have an ATC so no tool holders. It sounds like this Econo Probe may not be the right tool for my setup ?

On the probe screen if you have the probe tool mode selected then you need to have your axes homed. However, if you use the UCCNC version 1.2111 and you have slaved axes then you'll have problems. (There was a bug in the probing plugin which is already fixed.) I advice you to update to 1.2113.

I probably had the probe tool mode selected but got the error message even after homing the machine from the probe screen. I am using version 1.2111 but have no slaved axes.........only X,Y and Z.

BH

[dezsoe]

OK, check the A, B and C axes. If you have any of them enabled then you need to home it. Because you don't use them simply disable all. This will solve the homing warning problem.

The probe block will work better, because if you measure the surface with the 3D probe then you have to find out the difference to your tool. This will not be precise...

[bhdavis]

Thank you. I will give it a try and report back.
BH

[bhdavis]

"The probe block will work better, because if you measure the surface with the 3D probe then you have to find out the difference to your tool. This will not be precise..."

I assume that here you are referring to the situation where the probe is mounted on the spindle? In my case I've swapped the 3D probe tip for the included flat plate. That way my bit is in the router and the bottom tip of the bit hits the flat plate of the Econo Probe which is sitting on top of my material.

Thanks,
BH

[dezsoe]

This stuff is brilliant! I watched some photos and now I understand you. Measure the height of the probe with the plate on it and set this as Gage height. Turn on Axis 1 count gage. Now the probed height will be offset by the height of you probe and you'll get the workpiece zero. (Also, turn on the Zero probed axis.)

[bhdavis]

Thanks !

I think you are talking about doing this on the PROBE pages instead of editing the M31 macro and using the probe button on the main screen.........correct?

BH

[dezsoe]

Yes, of course, sorry.

[bhdavis]

Well, well, well...........success. Not as you suggested in the last couple posts but rather based upon your earlier comments.

Before messing more with the very complex Probe pages I thought of something to try with the M31.txt macro. AND IT WORKED !!

The probe now can sit on top of my material, I can hit the PROBE button on the main screen and the bit will touch down to the probe. Then it will record that point as as Z= 2.65" (probe thickness) and the Z-axis will then retract with a G53Z0 command. Final result is the top of my material is Z=0. Perfect !!!

I'll paste in the text file below. The red characters were settings I changed to suit my needs. The green lines were added. I thought about deleting all the X and Y related lines, as well as the dual probe lines, but decided to leave them in case I ever add an ATC spindle and need to set up a fixed point probe position.

Thanks ! All of your help is very much appreciated. You sent me down the right path.

BH

M31.TXT

//M31 probing macro

double probeX = 200;
double probeY = 300;
double Zmin = -10;
double FeedrateFast = 50;
double FeedrateSlow = 50;
double SafeZ = 0;
double retractheight = .5;
double retractforsecondmeasurement = .75; // Could probably delete this line

bool domoveXY = false; //Enable XY movement
bool dodualcycle = false; //Do probing from 2 cycles, first with Fast and second with Slow feedrates

if(!exec.GetLED(56)||!exec.GetLED(57)||!exec.GetLED(58)) // If machine was not homed then it is unsafe to move in machine coordinates, stop here...
{
MessageBox.Show("The machine was not yet homed, home the machine before probing!");
exec.Stop();
return;
}

while(exec.IsMoving()){}

double Xoriginalpos = exec.GetXmachpos(); // Get the current machine coordinates
double Yoriginalpos = exec.GetYmachpos(); // Get the current machine coordinates

if(domoveXY) // Make XY movement only if enabled
{
exec.Code("G00 G53 Z" + SafeZ); // Move Z up first
while(exec.IsMoving()){}

exec.Code("G00 G53 X" + probeX +" Y" + probeY); // Move to the probe sensor position in XY
while(exec.IsMoving()){}
}

if(dodualcycle)
{
exec.Code("G31 Z" + Zmin + "F" + FeedrateFast); // Do the Z probing with Fast feedrate first
while(exec.IsMoving()){}

exec.Code("G91 G0 Z" + retractforsecondmeasurement);
exec.Code("G90");
}

while(exec.IsMoving()){}
exec.Code("G31 Z" + Zmin + "F" + FeedrateSlow); // Do the Z probing again with Slow Feedrate to get a more accurate reading
while(exec.IsMoving()){}

{
exec.Code("G92 Z2.31"); // BHD add in to set g92z
while(exec.IsMoving()){}
}


{
exec.Code("G53 Z0"); // BHD add in to raise Z-axis
while(exec.IsMoving()){}
}



if(!exec.Ismacrostopped()) // If tool change was not interrupted with a stop only then validate new tool number
{
exec.Code("G44 H1"); // Load tool offset one, note the tool lenght is defined in the tools menu
while(exec.IsMoving()){}
exec.Wait(200);

double Zup = exec.GetZmachpos() + retractheight;

if(Zup > SafeZ)
{
Zup = SafeZ;
}

exec.Code("G00 G53 Z" + Zup); // Move 10mm above probe plate
while(exec.IsMoving()){}

if(domoveXY) // Make XY movement back to start position only if XY movement is enabled
{
exec.Code("G00 G53 X" + Xoriginalpos +" Y" + Yoriginalpos); // Move back to the original XY position
while(exec.IsMoving()){}
}

}