Help with sending programs to Fagor 8025 control

I have been having problems sending code to our Prototurn Lathe with a Fagor 8025 control. The code is for a chess piece part of our senior project. I am the first in the class to try to get this machine networked to a PC and have been having many problems getting it to work.

The coding is done is Mastercam X2 MR1 with a Fagor 8025 post processer. I have tried using the Mastercam post to send the code direct to machine but this has never worked. The control displays recieving on the screen but hangs on this step, I believe this is because Mastercam is not setup to send the end of transmission codes.

I also downloaded and installed WinDNC from the Fagor website but was not able to get this working at all. I am not sure if I am missing a part of the program but I cannot find the options screen to setup the machine controller type.

Last I installed NCnet Lite, this seems like excellent software for what I am looking to do but when I use it to send the .nc file to the machine it gives me an error, I'm not remembering exactly what the terms were but it seemed like a generic files not compatible/ file type not right error. I also tried to send the code in .txt files with the same result.

If anyone here uses this control I would be grateful if you could explain how you load programs, the software you use, and what connection settings you have set.

Could I be missing a critical setting on the control side or does this sound like a PC side problem to you?

I'm looking for any and all advice so if you think you may know what is happening please post.

Thanks,

Erik Fellenz

Could the problem possibly be in the code? I could post the code that I am using if it may help anyone help me find the problem.

Thanks,

Erik

Fagor files start with this for the first line--

%CUSTOMER PART NUMBER ,MX--,

The file extension is .PIM

We use WinDNC and a PCMIA card to transfer our files.

Thanks for the reply.

I have the %(five digit number) at the head of the program. What is "MX--" I have never seen it mentioned but I'm guessing it may be missing in my code.

I will change the file type and give it another go.

Thanks,

Erik

ARB said:

It may be .PIT for a lathe.​

Click to expand...

I'll be sure to try that too.

Thanks

I getting all this from the manual.

.PIT for a lathe and .PIM for a mill.

The ,MX--, are program attributes.

M stands for Modifiable and X stand for Executable.


Depending on the type of communication required, the serial port machine parameter "PROTOCOL" should be selected.

"PROTOCOL" = 0 if communications is with a peripheral device.
"PROTOCOL" = 1 if communications is via DNC

Ok,

Thanks again for the help. I hope I'm not sounding too dense but I'm still not sure what to do with a "MX--" or where to put it.

In my code my first line is %99996, it then goes right into the G-codes. I have no "MX--" anywhere in the code, should this be added right after the program number?

Is the Protocol 0/1 set on the machine or in software?

Thanks Again,

Erik

Another thought.

On our 8055i when i send a program it needs to be sent with a name like 000020. It need all six digits and all numbers.

Here is some code that i know goes and runs on our machine. We have a mill control so take that for what it is worth.

%
; SET SURFACE AT TOP
; HOME AT SOUTHEAST CORNER
;TOOL 6
;#23 DRILL
;OPERATION 1
T6
G0 X40.345 Y40.345 S6800 M3
Z2.
G0 Z0.1
G81 X40.345 Y40.345 Z0.1 I-0.375 F240.
Y30.8
Y21.05
Y11.3
Y1.755
X30.8
X21.05
X11.3
X1.755
Y11.3
Y21.05
Y30.8
Y40.345
X11.3
X21.05
X30.8
X23.55 Y21.05
X18.55
G80
G0 Z2.
M30
%

ARB,

On your mill where is the program number "000020?" On the lathe code the program number is on the first line of code like %85428.

Thanks for posting the code. It looks similar to the lathe code I am trying to get running. Does anyone have a short bit of lathe code they would be willing to post.

I am also curious if anyone has experience with NCnet Lite?

ARB, I am also curious to know what you use to send the files to your mill.

The 000002 goes on the send screen in WinDNC. This is software that you can get from Fagor. It works very well with the Fagor.

Are you sure your cable is correct ? The pinout info should be in the machine manual.
Try changing the file name to something not using "9" as the starting number.
I don't know on Fagor controls but on Fanuc 9??? series numbers are reserved for
system files. For a very simple, cheap, fix check these guys out http://www.cncrs232cable.net/servlet/StoreFront
The price is cheap at $76, including 50' of cable, and the support is excellent.
Their software is not fancy at all but sure gets the job done.
The protocal setting 0/1 would need to be set at the machine control.
Good luck
Al

allanjs said:

Are you sure your cable is correct ? The pinout info should be in the machine manual.

The protocal setting 0/1 would need to be set at the machine control.
Good luck
Al

Click to expand...

Thanks for the info,

I am a sure as can be on the cable, it have checked it with the diagram in the books and it looks good. I'll bring in a multimeter to make sure everything is OK though.

How do you set protocol on the control? I think this may be the missing link to my problems. All the books we have on the machine are for programming parts and general setup, I don't remember seeing machine interface setting in the book.

If you know where to get the info on how to do this I would love to see it.

Thanks,

Erik

I do not know how to get into the control area to set the protocol settings on a Fagor
control. This would be done in what is normally called the parameter settings.
As you are apparently in a school setting I would recommend contacting a machine
dealer to see if they would send a technician in to set up the communication.
Due to this being a school they may do it for free.

Hi! I work for Fagor. So let's look at it a little. On a website: www.fagorus.com, there is a section under Technical Support about the CNC8025 and RS232. This goes over a step by step process and tries to help you through the RS232 communications

Take a look at the material there. It will save you a lot of time and grief. A lot of what I say in the following information assumes you have read and understood the information from the website. If you can't get there, get back to me. My email address is [email protected].

Please note: If the 8025 is showing DNC at the top of the screen, it is expecting you to use the DNC way of communicating. The 8025 used software called DNC30. There is a new software called WinDNC, which also allows an 8025 or 8020 to communicate, but only for uploading and downloading a program.

The advantage of DNC or WinDNC software is that the program can be sent into the control sitting at you PC. In a pure RS232 communications system (without DNC), you have to turn off the DNC by changing parameters in the control (scary!), then you have to set up the CNC to receive, then you have to go back to the PC and send. And the file being sent MUST END IN ASCII 27. An ASCII 27 looks like a left facing arrow or a filled square box when you see it in a G-code program. One of the best ways to get an ASCII 27 is to download a program already in memory on the Fagor CNC. It will always end with that last figure.

Something good to do first is to try to get a program from the CNC to a PC. It is simpler than sending one to the CNC and would prove the cable is working. A lot of the time, the cable is wrong and nothing will work. In that information on the website, it shows exacly how the cable should be made. Fagor cannot control what your OEM or integrator has done when they place a connector on the outside of the CNC control box. The simple cable shown on the website can be plugged right into the back of the CNC. One of the connectors says "RS232" right on it. Take off any connector there now and replace it with the new cable. That will eliminate any variation caused by the manufacturer. You can copy the ASCII 27 from the program and paste it into the MasterCam post as the last character in a line by itself.


Using WinDNC software and having the DNC showing in the CNC screen, you can make your MasterCam program, SELECT ALL, COPY the G-code program, and PASTE it into a new program in the WinDNC. Then the program can be sent into the CNC with no problems.

Anyhow, let me know if you need more.

WayneCNC