[w102acd]

We recently got a Clausing Kondia FV-1 Mill with a Dynapath Delta 20 Controller. I have been playing around with loading programs and drip feeding programs.

Yesterday, I was able to load a program onto the machine and then run the program.

Today, I tried drip feeding. The program is 14724 lines. So, I started the program and it ran fine until N2496. It gave a "133 Format Fault" and the next said "N####". I am using Hyperterminal to drip feed the machine and am fairly confident that Hyperterminal is set-up correctly as I have used it to drip feed and load programs.

Are there any issues with this file's length and/or memory of the controller??? Dynapath thought it was Hyperterminal's fault??? Is there a time out or sleep mode for Hyperterminal??? Dynapath thought that it sent part of the line, but not the entire line, hence a format fault.

Tomorrow, I will turn on the echo to the Hyperterminal screen and see if that tells me anything.

Here is a paraphrase of the file I was trying to drip feed:

(INSIDE)$
N0001(E)G70$
N0002(E)G90$
N0003(E)M04$
N0004(E)G0X0.0000Y0.0000Z0.1000$
N0005(E)G0Y0.0114$
.
.
.
N2490(E)X10.5000Y0.6477$
N2491(E)Y1.0341$
N2492(E)X10.4886Y1.0455$
N2493(E)Y1.0795$
N2494(E)X10.4773Y1.0909$
N2495(E)Y1.3977$
N2496(E)X10.4886Y1.4091$
N2497(E)Y1.4432$
N2498(E)X10.5000Y1.4545$
N2499(E)Y2.8523$
N2500(E)X10.4886Y2.8636$
.
.
.
N9995(E)X6.3409Z-0.1242$
N9996(E)X6.3545Z-0.1199$
N9997(E)X6.3818Z-0.1127$
N9998(E)X6.4091Z-0.1067$
N9999(E)X6.4364Z-0.1016$
N0001(E)X6.4636Z-0.0972$
N0002(E)X6.4909Z-0.0932$
N0003(E)X6.5182Z-0.0897$
N0004(E)X6.5455Z-0.0864$
N0005(E)X6.6000Z-0.0809$
.
.
.
N4720(E)X2.0665Y2.0339Z-0.8828$
N4721(E)X2.0858Y2.0249Z-0.8975$
N4722(E)G0Z0.1000$
N4723(E)M30$
E

Thanks in advance!!!

[jagardner4]

The pound signs (#) in the sequence number indicate an overflow on any DynaPath control. Based on this fact, and that there is no issue with the program file you are trying to send, there is a problem with the transmission of the program to the CNC.

Buffered Input, or drip feed, allows programs of unlimited length. There is no time out or sleep mode in Hyperterminal.

The description of the problem would indicate that the sending computer is not seeing the XOFF character sent by the control to pause the transmission (if software control is selected) or does not see the CTS (Clear To Send) line go low (if hardware control is selected). This could mean a problem with either the cabling or there has been a hardware failure on the UART in the control.

There is a small chance this is a software error that was found on Delta 20 controls shortly after the Buffered Input feature was implemented. If a sequence number just happened to start on a memory page boundary, a fault would occur. Please call DynaPath with the software level to check. The software level is given on the first screen to appear after booting, before you press the Mode Select key. It is a four digit number preceeded with a 'P' and possibly another letter (i.e. PA5203).

One way to get around this problem without updating the software is to vary the length of the blocks by adjusting the sequence numbers (using 3 digit sequence numbers instead of 4).

[w102acd]

Well, with the help of the extremely friendly folks at Dynapath, we got the porblem fixed. If we switch to a software handshake instead of hardware the problem goes away!!!

Thank you very much jagardner4 for your help!!!

Regards,
w102acd

[w102acd]

Well, the problem came back again. We have the machine in our shop/office space. The machine worked fine for the entire day. We paused the machine over the weekend and I started it up on Monday morning. Well, it us two format errors and then put a nice cut right through the middle of our part. Fortunately we were cutting a piece of wood so no harm done.

I started looking into Hyperterminal more. I found a bunch of links that say don't use it to transfer large files. I started Hyperterminal and told it to send a large text file. I had the machine paused and Hyperterminal filed the machines memory as expected. However, then Hyperterminal would wait about 8-10 seconds and send a character. So if it did this over the weekend, that would be a lot of lost characters. Hence the format errors!!! The cut through the part wimilar problem (I think). The error was close to G1Y2.7076. I suspect for some reason that the G1Y.7076 was passed instead.

Long story short we downloaded "nclink free" from onecnc.com. Got the machine all set-up and started a 277000 line file. It ran flawlessly all day, we paused it overnight, restarted in the morning and it finished just before lunch. It worked perfectly!!!

I should probably state that I have nothing whatsoever to do with onecnc.com just wanted to let whoever know about how we got our machine to work correctly.