[REVCAM_Bob]

Can anyone tell me how to capture probe output data from the rs232 port into a file on a p.c.?
Thanks, kinda lost on this one!

I would like to be able to access the data from a p.c. to do further calculations on the point(s) provided by the probe.

[bonmotwang]

Google serial port tool, then get the comm operator free version.
It is a very good tool. I bought it for my TCP/IP testing, also for RS232 programming and simulating too.


Sent from my iPhone using Tapatalk

[txcncman]

I have not delved into macro programming for Fadal. On Fanuc, there are commands to output captured data to the RS-232 port. You will also need a computer set up to "listen" for the data.

[skippy]

Hi REVCAM_Bob,
Probing is a subject that interests a lot of us here but very little seems to be documented about the process. There's plenty on edge & centre finding and height sensing but surprisingly little on probing for free form organic surfaces. Assuming this is what you are trying to do, any chance you could document your progress here?
Regards
Phil

[bonmotwang]

If just want to capture the waveform, you will need a data logger to capture the data into a PC.
I am doing that all the time, part of my job is to analysis the communication protocol. Sometimes reverse engineering the protocol in some old machines.
There is a tool called digital analyzer:-D.
Search eBay you will find one for your frequency.


Sent from my iPhone using Tapatalk

[skippy]

Hi BONMOTWANG,
Just to make sure you understand what we are talking about: the object is to capture the xyz coordinates of the machine doing the probing over a free form organic shape in order to reproduce that shape in a CAD program. Is that what you are talking about?

If so, could you please expand on your comment about the digital analyser (pour les nuls comme moi)? I looked at ebay for quite some time and saw all manner of digital analysers (temp, pressure, etc.) but didn't see anything that stood out as being a possible for this application. It's probably me that hasn't understood due to my lack of I.T. knowledge so please excuse me if that's that case.

Regards

[REVCAM_Bob]

Hi REVCAM_Bob,
Probing is a subject that interests a lot of us here but very little seems to be documented about the process. There's plenty on edge & centre finding and height sensing but surprisingly little on probing for free form organic surfaces. Assuming this is what you are trying to do, any chance you could document your progress here?
Regards
Phil

Yes, I can document what I find here, I think it will really help others, and me too, as the more people are engaged the more good ideas come to light.

On that note:
The reason I am doing what I am doing is to improve the usfullness of probes on our cnc mills. From what I have seen there is very little being done "well" that makes a probe a reliable usfull and automated tool. One guy I talked to showed me what you can do from a Haas control, and all these pre-canned cycles are very basic at best, do not include any form of real error checking, redundancy checks etc.
This particular company basically does not use their probes due to the fact that a probe will not detect a chip in the way, does not "self detect" errors in the probe setup etc.
My goal is to automate some of these things so that the probe can be considered a reliable tool.
To do this I don't think it makes sense to delve deeply into attempting all of this with macros on the machine tool, rather I woul like to put the data out to a computer so that I can use real programing language and routines to automatically create probe points on the cad data, i.e. to probe a pocket you do not want to just probe two sides of the pocket and expect the result to be reliable. I think I want to probe two opposite sides, and probe each side in 5 or more places, check the consistency of the data and if one or more points looks suspect (i.e. not uniformly consistent with the others) throw the bad points out, or alert the operator or something.
The goal is to include the probing into the cad/cam routines directly mesure mid cycle, make cutter comp adjustments and finish cutting the pockets.....
So anyways, Yes I will post my results here.....

Thanks!

[REVCAM_Bob]

If just want to capture the waveform, you will need a data logger to capture the data into a PC.
I am doing that all the time, part of my job is to analysis the communication protocol. Sometimes reverse engineering the protocol in some old machines.
There is a tool called digital analyzer:-D.
Search eBay you will find one for your frequency.


Sent from my iPhone using Tapatalk

Hi, I am actually trying to capture probed points from the CNC control.
There is an option on the Fadal (as well as most other controls I am sure) that will send the probed xyz coordinates to the rs-232 port.
So my first step is how to get those points saved to a text file on the pc so I can pass each point to the cad/cam system and the accompanying software that will run calculations on the probed point. So I am not trying to capture free form surfaces per see, however the concept is faily close to being the same procedure I would imagine......

[txcncman]

Post what you have come up with in the way of macros for Fadal so that others can offer input on how to complete and improve them.

[Neal]

Simply use the SPRINT statement to out put the P1 P2 and P3 probed points. Don't make it complcated. You need a waiting program on the remote PC to capture the incoming data.

Neal

[REVCAM_Bob]

Hi Neal, I am guessing the sprint command can be used within a program?
That would be cool. I was experimenting today, and the book says the g31 command is supposed to dumpt the data directly to the rs232 port.
Perhaps the sprint command will work. I will try it.
Being able to control how and when the data is sent will likely be a better approach.
Since you seem to be in the "know", could you tell me if the same cable we use to send programs to the fadal will work for recieving data? I have made the assumption that it will, but when I couldn't get anything to read today, I started questioning everything.

Thanks for the tip!

[txcncman]

The cable is the same. Might need different software. Or use Windows Hyperterminal. Most software has time out setting. unless your software can be set to never time out, you might have issues.

[REVCAM_Bob]

The cable is the same. Might need different software. Or use Windows Hyperterminal. Most software has time out setting. unless your software can be set to never time out, you might have issues.

Making some progress... I was able to use the sprint command you suggested and get the output to go to the software called CommPal and dump the text data to the window in this software.

Now I have to figure out how to get it to dump the data to an open text file so that I can access that file....
Any thoughts on how to get a file that will receive the data?

[REVCAM_Bob]

G90 G10 L10 P99 R0 -5.78500000
T1M6
M00
*
*PUT TOOL 500 IN SPINDLE
M19
# SPRINT "POCKET_ID 1234"
# SPRINT "WALLS_PLUS_TOL 0.001"
# SPRINT "WALLS_MINUS_TOL 0.000"
G0 X2.4167 Y-1.1500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.4167 Y-1.0000 P1
# WAIT
# SPRINT "X1 ",PX1
# SPRINT "Y1 ",PY1
# SPRINT " "
G0 X2.3333 Y-1.1500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.3333 Y-1.0000 P1
# WAIT
# SPRINT "X2 ",PX1
# SPRINT "Y2 ",PY1
# SPRINT " "
G0 X2.2500 Y-1.1500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.2500 Y-1.0000 P1
# WAIT
# SPRINT "X3 ",PX1
# SPRINT "Y3 ",PY1
# SPRINT " "
G0 X2.1667 Y-1.1500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.1667 Y-1.0000 P1
# WAIT
# SPRINT "X4 ",PX1
# SPRINT "Y4 ",PY1
# SPRINT " "
G0 X2.0833 Y-1.1500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.0833 Y-1.0000 P1
# WAIT
# SPRINT "X5 ",PX1
# SPRINT "Y5 ",PY1
# SPRINT " "
G0 X2.0833 Y-1.3500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.0833 Y-1.5000 P1
# WAIT
# SPRINT "X1 ",PX1
# SPRINT "Y1 ",PY1
# SPRINT " "
G0 X2.1667 Y-1.3500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.1667 Y-1.5000 P1
# WAIT
# SPRINT "X2 ",PX1
# SPRINT "Y2 ",PY1
# SPRINT " "
G0 X2.2500 Y-1.3500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.2500 Y-1.5000 P1
# WAIT
# SPRINT "X3 ",PX1
# SPRINT "Y3 ",PY1
# SPRINT " "
G0 X2.3333 Y-1.3500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.3333 Y-1.5000 P1
# WAIT
# SPRINT "X4 ",PX1
# SPRINT "Y4 ",PY1
# SPRINT " "
G0 X2.4167 Y-1.3500
H99 Z0.100
G01 Z0.088 F30.0

G01 G31 F1.0 X2.4167 Y-1.5000 P1
# WAIT
# SPRINT "X5 ",PX1
# SPRINT "Y5 ",PY1
# SPRINT " "
# SPRINT "DONE"

[REVCAM_Bob]

Would anyone have any thoughts on how to tweak tool diameter or length offsets (while a program is running, but paused) via rs232 input? Or maybe change a macro variable value???

[txcncman]

I am not sure you can go back and forth with the RS-232. But since you are going to capture some data with the probe, you need to write it to a variable as well as send it to the remote computer via RS-232. Once you have captured the data, you can do needed math operations and compare to a set value. Then you should be able to modify the needed offset registers by appropriate amounts.

[REVCAM_Bob]

I am not sure you can go back and forth with the RS-232. But since you are going to capture some data with the probe, you need to write it to a variable as well as send it to the remote computer via RS-232. Once you have captured the data, you can do needed math operations and compare to a set value. Then you should be able to modify the needed offset registers by appropriate amounts.

I am afraid you may be correct about not being able to go back and forth.
The only way I know of to alter a variable would be to send a whole new program with the variable set in that program.....
So that opens up a whole new can of worms if I have to do that...
Hmmmm there has to be an easier way???

[txcncman]

You build the math into the program using macros. I won't try to go into details with variables here since you seem to have a handle on that. The logic is something like:

Run final roughing pass
Set size variable (i.e. #100=5.000)
Probe positions X1 (X0.000) and X2 (X5.010)
Calculate size (i.e. X2-X1>>>>5.010)
Calculate difference in size (5.010-#100>>>>> -0.010)
Adjust tool offset variable (#variable number = #variable number + -0.010)
Run finish pass

[REVCAM_Bob]

Yes that may be the only way. I was hoping to do more outside of the control, but hey, whatever works!

Update: With the small inexpensive probe we were able to probe (on first try)
with a repeatability of 0.0001 on two different milled faces.
That's a pretty darn good start for using a $300 probe!

I haven't given up on doing things outside of the control, still researching possibilities.

My only thought would be to run each part of the program as a separate program, then on the fly write the next program with adjusted parameters and download the code etc..... but that is starting to sound more difficult than doing it in a macro. My thought was that with external information we could display results on the computer etc... Still thinking on that one.

[txcncman]

Yes that may be the only way. I was hoping to do more outside of the control, but hey, whatever works!

Update: With the small inexpensive probe we were able to probe (on first try)
with a repeatability of 0.0001 on two different milled faces.
That's a pretty darn good start for using a $300 probe!

I haven't given up on doing things outside of the control, still researching possibilities.

My only thought would be to run each part of the program as a separate program, then on the fly write the next program with adjusted parameters and download the code etc..... but that is starting to sound more difficult than doing it in a macro. My thought was that with external information we could display results on the computer etc... Still thinking on that one.

The way most CNC machines work is they have the ability to use cutter compensation and offsets to adjust tool paths, and have been this way for years. I guess I am not seeing the benefit to "rewrite" a program instead of changing an offset. I have actually seen people do this before, changing a tool path 1 or 2 thousandths, that did not know how to program using cutter compensation and it was a huge time waster. If your goal is to take the control away from the machine operator and put that control in the hands of someone more capable, I would offer the argument to hire more capable employees or train the ones you have. If your goal is to operate the machine remotely, totally hands off, then I would say macro programming is the way to go.