Fadal DNC transfer speed

[dksoba]

I'm using NCFadal to do DNC. I am using CD,10 (384k if I recall correctly). My program has a lot of small line moves in it. The control keeps stalling whenever there are a lot of small moves. The NCFadal transfer dialog box shows that I am only transferring ~250 characters per second....which is dead slow. If I use a higher or lower baud rate, I still get the same result.

I went into the parameters menu (setp) and found that buffer size is 255. I tried setting it to 15 to see if it would make a difference, but it didn't make any difference.

The cable I'm using is custom made (by me). It has wires for the TX/RX, ground, and shield, if I recall correctly. It is roughly 15 feet in length, and then it hooks up to a USB converter.

Is there anyway to test the actual throughput of my control system so I can figure out where the problem is?

It would be really really nice to have a faster transfer rate so my program stops stalling.

Thanks,
Matt

[carbidecraters]

Sorry but your control cannot keep up with the moves. Even a Fadal -5 system only moves at 250BPS. Usually not nearly fast enough for fast contouring. Most report 29IPM the fastest for continuous contouring.

[mariojl]

Hi, Matt:
For your comment, I assume you’re DNC’ing a program of a 3D surface with a lot of small moves, created by some CAM software. If this is the case, all you need is a control that has a function of “Look Ahead”, otherwise it just receives an instruction or block, executes it, and then reads the next. This makes the machining very slow (doesn’t matter what speed you’re set at), for it has to accelerate, run too next point, and brake, then start again.
Some controls, ( Haas for instance) are reading sometimes 200 or 500 blocks “Ahead”, so the control “know” what to do next; it makes the difference when you machine 3D figures, as could be plastic molds, models or patterns.
I used to have a VMC whit a Fanuc OM, making plastic moulds, having same problem, and couldn’t understand what happen until I bought a Haas VF3, which will run at full speed all the time.
Hopping this comment may help you,
Regards,
Mario
Inteligent Choices ('...theren't Magic Solutions)

[dksoba]

Hi, Matt:
For your comment, I assume you’re DNC’ing a program of a 3D surface with a lot of small moves, created by some CAM software. If this is the case, all you need is a control that has a function of “Look Ahead”, otherwise it just receives an instruction or block, executes it, and then reads the next. This makes the machining very slow (doesn’t matter what speed you’re set at), for it has to accelerate, run too next point, and brake, then start again.
Some controls, ( Haas for instance) are reading sometimes 200 or 500 blocks “Ahead”, so the control “know” what to do next; it makes the difference when you machine 3D figures, as could be plastic molds, models or patterns.
I used to have a VMC whit a Fanuc OM, making plastic moulds, having same problem, and couldn’t understand what happen until I bought a Haas VF3, which will run at full speed all the time.
Hopping this comment may help you,
Regards,
Mario
Inteligent Choices ('...theren't Magic Solutions)

This isn't the problem. It runs fast, and then all of a sudden it halts and you can see on the screen that it has run out of g-code. I have run the same program on my friends fadal with no issues, and his is a 1991 Fadal 4020. Also, if I upload a program to the control I don't have any issues with it, it's just over DNC that I have these problems.

My DNC setup says that I'm transmitting only 250 characters per second, not blocks per second. A single block can be some 23 bytes. If I remove spaces and line numbers this helps, which doesn't change the number of blocks only the size of each block.

I think what I will do next is to make a test program with a lot of small linear moves at a fixed feedrate to get an idea of what my actual blocks per second is. I will then time its run time over DNC at different data rates, and time it when it's uploaded to the control.

By the way, my board is 1400-4, so what are the implications of that?

Matt

[txcncman]

What happens when you turn the feed rate override down to say 10%? Does it still stop? Does it stop at the same point of the program?

[dksoba]

What happens when you turn the feed rate override down to say 10%? Does it still stop? Does it stop at the same point of the program?

Nope. No more stopping.

[txcncman]

I think this proves your CPS (Characters Per Second) on your DNC is definitely too slow for the feed rate programmed. Possible work around is program for a slower feed rate. Another possible work around is break the program into parts small enough to fit in machine memory and upload one of these parts of the program at a time and machine it. Then delete and upload the next part of the program.

The final problem is that not only is the DNC transfer too slow, the control itself might be to slow to handle the required CPS. You might need to look at the resolution of your tool path for surfacing. You may be running a resolution of 0.001" where 0.005" would still give acceptable finishes.

As far as I know, there is no direct fix in the hardware for these problems. These problems are the limits of the machine control.

[slowlearner]

Have you tried filtering your program by converting lines to arcs?

[Delw]

I run surfacing on my fadal everyday. my programs are anywhere from 4 megs to 30 megs.
I run cd,9 anything more I have issues. I think its due to floresant lights and cable length just not sure, bt 10 doesnt work for me.
if the code isnt going fast enough the machine will pause and wait for more code ( wont just cancle like yours is doing) if your feeding code to fast it will just use the buffer.

check your time outs both on machine and mainly on PC.
if your using a USB port connection on your pc that more than likely is your problem. I have a old PC with serial and dont have problems( but did with UBS convertors)

your wiring may be not hooked up correctly also.
I am guesisng its more of a set-up on the pc side issue than anything else. dont forget just because your software has the numbers set doesnt mena you pc follows them( my pc had that issue and I had to manualy go into control panel and fix them.

[Anders6612]

On Rs232 i had simular problems, but changing setting of FIFO buffer in the serial port helped me. But i dont know about that with USB converter.

Get an IO-card for your computer instead.

[gm3211]

A few ideas:

1) USB to serial hardware
2) Change your protocol

Welcome to USB to serial adapters...not all are the same from our years of experience. There is a reason why we pay alot more for these simple converters for USB to serial. I never can understand why one spends $20 bucks or less on this unit and then will wonder why performance is an issue or possible a scrap parts. The payback on a industrial, tested, proven solution makes the most sense. Save your money, headaches, gas and invest in a solution that is supported and tested by the machine tool industry. Ask your machine tool supplier or DNC provider.

If the Fadal is in "DNC" mode, there is perfect solution called Xmodem. Haas and a few others like Fadal were smart to build in this protocol to allow for an error correction communication method. Furthermore, you can exceed the 38K bottle neck to get the through-put to your machine. Several pieces are still required. Reliable software, PC, serial port, RS232 cable and a valid, programmed NC file. Give it a shot as I have several customers using this communication with our products and it just runs like a champ with 3D contouring. If you don't want to mess with all the PC, cables, and software, look at USB pendant solution for the Fadal we offer. It's screams!

[DareBee]

USB convertor = BAD.

Git rid of it and install a serial card (I did).
I run DNC at 39K from NCFadal into my -4 control.
I have never had an issue since I ditched the USB.
Before - it was roulette.