[yoya]

Hi, can any one help me how to drip feed fanuc omc. I have tried to change the parameters on cnc but it doesn't work, and can only send the program in the memory (which is too small).

thanxs in advance

[lakeside]

what file extension are you sending as .DNC

[yoya]

The file extensions are .nc or .nci
My problem is I can excute the programs from the memory of cnc. but directly from the pc is impossible . specially for large one's, is a headache, dividing them in small parts.

jud s
thanks

[Sharknose]

What program are you using in the PC to send the file to the Fanuc? Whatever it is, it needs to support XON/XOFF ( = ASCII 17 decimal/ASCII 19 decimal, or DC1/DC3) handshaking (flow control). That is, when it receives an XOFF character from the Fanuc, it needs to stop sending, and resume sending only after receiving an XON character. Can you send a program from the Fanuc to the PC properly? You can use this to verify communication in that direction - if you can, then the flow control characters ought to make it through too, provided the Fanuc is sending them. I think it sends them by default, but am not sure what parameter(s) if any can turn them off. Note that it may also be possible to set the Fanuc up to use different flow control characters than DC1 and DC3, via other parameters. Hopefully you have or can get a communications manual for that control.

[diggityds]

On My Fanuc 15m And 11m Controls Were Pretty Easy. Fortunatley I Didnt Have To Change Any Parameters, Most Of The Problems I Had Was In My Software And Aslo The Computer. Make Sure Your Dnc Software Baud Rates And Parity Bits Are The Same As The Cnc Control, Then I Found Out What Helps If You Go To Your Computers Com Port Settings In The Device Manager And Set Your Buffer Speeds To The Lowest Setting. If Your Control Is The Same As Mine You Should Push The Tape Mode Button On The Control And Hit Start, Then The Machine Is Waiting For Transmission. As Long As Your Getting Any Type Of Communication To The Control Is A Good Sign Wether It Be An Buffer Overflow Or Whatever, Then You Just Have To Mess Around With Some Of The Settings Or Parameters In The Machine. Let Us Know How It Goes.

[tahlinc]

Excellent DNC that does drip feed.
CodeShark lite $20
http://www.softsquad.com/products.htm

Cat 5 network cable makes good hardware handshake.
Look at offerings:
http://www.l-com.com/item.aspx?id=5129

Drip feed on Fanuc use Tape mode. You will not see program on display.
Recommend hardware handshake for trouble free usage.

We use for OMC. Works great.

GL
Jim

[Sharknose]

If he can send short programs to the control, but just can't drip feed, his basic download communications parameters (baud rate, data bits, etc.) are probably OK, but Fanuc controls allow you to set a different upload baud rate than the download baud rate, so that's something to watch out for. Also there's a way stop bits can be a problem. The stop bits are just the minimum amount of time between characters in a serial transmission (which RS-232 is), expressed in units of single bit times. (That's why you sometimes see 1.5 for a stop bits setting - there's really not one and a half bits of anything being sent, it's just waiting that long before sending the next character.) If the sender has a longer setting for stop bits than the receiver, it'll work fine, because it's a minimum. But if the sender has a shorter setting for stop bits than the receiver, every character except the first one will be garbled, because the receiver wasn't ready to take in the next character before the sender started to transmit it. Now, since the flow control is just one character at a time, this ought not to be the problem in this case, but if he tries to send a file back to verify Fanuc-to-PC communication, and gets junk, it'd be worth checking.

[Fish]

Hey Yoya,

Just another annoying little problem that becomes a big problem.....'aint machining fun!!!!

Some questions,
1) What control is it?
2) Do you have the manuals that show how to change parameters, The 8000 setting is the one I'm referring to. It must be changed to allow you to change other settings.
3) What communication software are you using?
4) What operating system are you using on your pc? I have found that Windows 2000 is the absolute best for DNC to all of my machines - Fanuc and Mazatrol - no hang-ups like Windows 98, and better control than XP.
5) Are your cables wired properly? The machine will accept programs without having the cables right for DNC'ing. One connection will make all the difference.
6) Does your machine allow DNC? Can you put the machine into "Tape" mode?

I have set up all my machines using OneCNC's free DNC software called NC Link. I use it for Fanuc OT, 10T, 15MA, Hass and Mazak. The help file in it is the best. It has all the info for settings, wiring diagrams for your cables etc. I presently use it for DNC lights out operation at up to 19000 baud with absolutely no issues (limited by machines computer speed).

Let me know if you want a copy of NC Link, and I can e-mail it to you. Or if you need any more help. I'm not a "specialist" but I have done this many times with the pressure of customer's pressing for deliveries, vendors looking for money, employees waiting etc. If you want, e-mail me at [email protected]

Fish

[drachir8]

I think the problem is that you are trying to drip feed your program in the memory in the edit position. With fanuc there is edit run and an auxillary run that is used for dnc. Do not try and drip feed in the edit position. drip feed in the auxillary run position. Dont forget to place a M0o in the begining of the program or the machine will start without you at the control, ask me how I know

[Fish]

Hey Drachir8,

If you set your communication software to "start at machine", then you won't have the problem of the machine starting without you. The program is sent at the pc, which then waits for the machine to send the "send" signal, which is the sent when you press the start button on the machine. If you set it up this way then you have full control, including single blocking to make sure your co-ordinate settings are right. DNC done right is just the same as running from the machine's memory.

Fish

[mrfixit]

99% of the time it is a cable issue. Or the software is not setup correctly.

Not all DNC software supports a basic send/receive cable. You need a full handshake cable which allows the PC and CNC to talk or start/stop the sending of data based on the buffer state of CNC.

If the cable checks ok - i.e. all pins are connected properly. And you are satisified that the software is good then I would check into the possibility that you do not have the correct option for DNC turned on in the Fanuc 0M. As we all know Fanuc loves to make everything an option bit. I think that the DNC capability is in fact an option for all Fanuc controls.

Also be sure you are in TAPE mode not AUTO when trying to run. And you should start the machine by pressign cycle start then start sending data. And the M00 or set your overrides to 0% is a good idea to avoid a crash.

[Al_The_Man]

Most O's the DNC option switch has to be on the machine by the Machine tool builder and is done through the Ladder (DNCI signal).
This is the page from the manual.
Al.

[mrfixit]

That is correct! But I think it has little to do with the problem that YOYA is having. The DNCI is not the option bit I was refering to. The DNCI signal is a input from the CNC to the PMC to intiate the DNC operation and this signal is set high when the first character "%" is sent from the PC through the DNC Cable. This would be a great place to look when troubleshooting. If the DNCI signal is not set high at the start of data flow then the cable or offline software is not doing it's job.

(It has been a long time since I have worked with this type of problem so I apologize if this information is not entirely correct. But, I beleive it is at least close to the idea of what happens.)

[yoya]

Thanks all guys

I will work out on all the solutions that you had given me and will let you know .

hoping to resolve it sooner, cause i had to prepare some mold pieces urgentlly......could imagine my problem..
Any how I am using cimico edit v5 for the trasmission.
The cnc receive programs either edit or auto mode, but to do the job has got to be in auto mode and then start..

But I the only thing I have to check the tape mode..

thanxs again

[yoya]

Hi

There was a big problem on the machine, it doesn't have a function of "tape mode"......
my question is , If I can send and receive programs from cnc, those which are saved in the memory... does it mean that the cnc has "tape reader"???

The fanuc operatore has said that, it has got to be added another appliance to the machine.
How can I resolve this problem?? Is there a possibility to modify it from the cnc parameters???

Grazie mille

[diggityds]

THAT OTHER APPLIANCE HE'S TALKING ABOUT MIGHT BE A BTR CABLE OR AN ATR CARD FOR OLDER FANUC MACHINES. THE ATR CARD CONNECTS TO YOUR MACHINES PROCCESSOR AND COMES WITH SOFTWARE. YOU CAN THEN DRIP FEED AND IT ALSO STORES UP TO 1 MEG OF MEMORY. IT GOES FOR ABOUT $1400 AND THATS THE ROUTE I MIGHT HAVE TO GO WITH MY 6M FANUC. A BTR CABLE ALSO CONNECTS TO THE MACHINE BUT ELIMINATES THE TAPE READER, BUT YOU SAID YOU DON'T HAVE A TAPE READER. THE GOOD PEOPLE AT www.sub-soft.com HELPED ME OUT WITH A LOT OF PROBLEMS I HAD, AND THE ALSO SELL THE COMPONENTS YOU MIGHT NEED.

[Al_The_Man]

The tape input is installed as part of the function switch by the machine tool builder, he may have excluded it.
Normally to run in drip feed on a 0, you have to be in auto, the DNCI signal has to be set on from the PMC side to the CNC, this is bit G127.5 in the ladder, often done with a toggle switch or AUX switch.
You should be able to use a 3 wire cable and use software handshake in your PC program.
Al.

[T_Rex]

Hi Yoya,

Is there a memory selection on the machine....next to edit?
If so....select it into memory mode and get ur sending program ready on "x-on and wait" setting....now press cycle start on ur nc.....this should work.

If still not....check ur cable config...6-8-20 should be bridged and pin 4 and 5 should be bridged on the 25pin plug.....
I'm assuming you are using a 25pin at the cnc and 9 pin at the pc.
on the 9 pin 4 and 6 should be bridged and 7 and 8 too.....you will connect pin 7 at the cnc to pin 5 on the 9 pin at the pc.
The no 2 pin at the pc (9pin) should go to the no 2 pin at the cnc (25pin)
The no 3 pin at the pc (9pin) should go to the no 3 pin at the cnc (25pin)

If this still doesn't work.

Check in ur parameters under 512...513...514....this setiing should be 11.
That'll give u a 9600 baud rate....if it is 10....that'll give you a 4800 baud rate.

If you can allready send and receive normally...don't change the parameters.

If you still can't get it right....please let me know.....these things are usually not that hard to work out.....but u do get the odd exception.

Kind Regards.

T_Rex

[motomitch1]

Fanuc 10-11-12-15-series controls must have a tape reader to do direct DNC

[T_Rex]

hi there,

I agree.....but he is using a omc-fanuc control

Edgecam NC Editor can emulate a tape reader with great success...what dnc software are you using?

Kind Regards.

T_Rex

Hi, can any one help me how to drip feed fanuc omc. I have tried to change the parameters on cnc but it doesn't work, and can only send the program in the memory (which is too small).

thanxs in advance