Haas Single Surface Probing Macro

[CHAD PEZZLE]

Please bear with me as I'm new to all this, I've been reading and searching for a while but can't quite find what I'm looking for. I'm brand new to Haas control and probing, and I'm trying to write a short probing cycle to insert at the beginning of my program to locate a single surface.

 

So, I load my part into a set of soft jaws and probe the first part to set my G54 zero a run my first part. My soft jaws will locate each additional part accurately in the y and z direction, but I need to probe the part in the x direction in order to update the new x zero based off that surface. There's a bit of variation in each part so using a stop is not accurate enough. I've read through the provided Inspection Plus Manual, but can't quite get exactly what I need.

 

Using the Inspection Plus Manual this is what I came up with (below), but running the cycle I get an error as it tries to probe the part.

 

T20 M6 (select tool probe)

G54 X0 Y0

G43 H20 Z3.5

G65 P9832

G65 P9810 Z1.5

G65 P9811 X-2.9 S1

G65 P9810 Z3.5

G65 P9833

 

Basically I want to probe a single surface in the x direction and have that measurement update my fixture offset accordingly. Machine is a 2015 Haas VF2

 

Thanks in advance for the help,

Chad

[paulmac]

where are your datums set from ,assuming your datums are x & y center of your part & z bottom face.

T20 M6 (select tool probe)

G54 x-3.2 Y0

G43 H20 Z3.5

G65 P9832

G65 P9810 Z1.5

G65 P9811 X-2.9 S1 

G65 P9810 Z3.5

G65 P9833

[CHAD PEZZLE]

My x and y zero is the center of my material. Z zero is the top surface.

[paulmac]

in that case this will get you what you want

 

T20 M6 (select tool probe)

G54 x-3.2 Y0

G43 H20 Z3.5

G65 P9832

G65 P9810 Z.5  F10.      (PROTECTED MOVE ABOVE MATERIAL)

G65 P9812 X5.8 R.2 Z-.5 S1 (PROBE AND SET X  DATUM IN CENTER OF YOUR MATERIAL)

G65 P9810 Z3.5

G65 P9833

 

THIS CYCLE PROBES BOTH SIDES IN X AND SETS THE DATUM IN THE CENTER OF THE MATERIAL

[CHAD PEZZLE]

Thanks Paul, but I'm realizing my description of my setup wasn't good enough. The material I'm machining isn't just a square piece of stock. I'm machining a slot in a piece of 1" round tubing. The tubing has several compound bends that make the web macro difficult to use. My x zero isn't actually the center of my material but the center of the slot I'm machining. Sorry for the poor info.

 

I'm also realizing that the single surface probing macro is only the beginning of what I need in the macro. I want to probe a single x surface and have it update my fixture offset, what I didn't think about is that as I touch off that single surface that's not actually my x zero, I want to add a given amount to that measurement to make that point my new x zero for my offset. 

 

Essentially, I want to probe a single surface in the x direction and have the macro add a given amount to move my offset a given distance from that probe position every cycle and make that my new G54 x zero.

[paulmac]

THEN YOUR ORIGINAL MACRO IS ALLMOST RIGHT JUST THE X START POINT AND THE Z DEPTH NEED CHANGED

G65 P9811 X-2.9 S1 WILL SET G54  X ZERO +2.9 FROM THE SURFACE THE PROBE TOUCHS OFF

T20 M6 (select tool probe)

G54 x-3.2 Y0

G43 H20 Z3.5

G65 P9832

G65 P9810 Z.5

G65 P9810 Z-.5 F10.

G65 P9811 X-2.9 S1 

G65 P9810 Z3.5

G65 P9833

[jlw™]

A lot of people don't know that you can put in a Q for overtravel. Sounds like you may want to do that.

 

I have some parts I play it safe with my approach and the run the probe 3 to 4 inches to find the part.

 

Just a thought.

[Machineguy]

And what is wrong with the Probe cycles that are in the machine?

 If you bought the probe from Haas, they are there to use.

 

Just asking?

[cncchipmaker]

Thanks Paul, but I'm realizing my description of my setup wasn't good enough. The material I'm machining isn't just a square piece of stock. I'm machining a slot in a piece of 1" round tubing. The tubing has several compound bends that make the web macro difficult to use. My x zero isn't actually the center of my material but the center of the slot I'm machining. Sorry for the poor info.

 

I'm also realizing that the single surface probing macro is only the beginning of what I need in the macro. I want to probe a single x surface and have it update my fixture offset, what I didn't think about is that as I touch off that single surface that's not actually my x zero, I want to add a given amount to that measurement to make that point my new x zero for my offset. 

 

Essentially, I want to probe a single surface in the x direction and have the macro add a given amount to move my offset a given distance from that probe position every cycle and make that my new G54 x zero.

It sounds to me like all you need to do is update your G54 work offset. The system variable for G54 X is #5221. So lets say that you would need to shift your X  .1 after you initially set G54 off of the part. All you would then need to do is write this macro:

 

 

(Probe Parts Set G54 X)

(Then:)

#5221=#5221+.1

[CHAD PEZZLE]

 

THEN YOUR ORIGINAL MACRO IS ALLMOST RIGHT JUST THE X START POINT AND THE Z DEPTH NEED CHANGED

G65 P9811 X-2.9 S1 WILL SET G54  X ZERO +2.9 FROM THE SURFACE THE PROBE TOUCHS OFF

T20 M6 (select tool probe)

G54 x-3.2 Y0

G43 H20 Z3.5

G65 P9832

G65 P9810 Z.5

G65 P9810 Z-.5 F10.

G65 P9811 X-2.9 S1 

G65 P9810 Z3.5

G65 P9833

 

Thanks Paul, I got it dialed in and this looks basically what I ended up with. Just had to adjust my z depth a bit to get the correct offset from my center location. After reading the manual I found the info about adjusting the overtravel as well so I added that in.

 

Machineguy I'm not sure if I'm using the terms correctly but the code I've quoted above is what's loaded by Renishaw into the Haas. I wanted to add this code to my program to make the probing automated rather than having to probe each part manually.

 

Thanks for the help.

Chad