fanuc 16k memory limit

[balsaman]

At our shop we have a 25 year old mill with a fanuc control. It has a memory of only 16k. Someone said you can put an old PC between the programming PC and the mill, with some software that acts as a buffer so we can send it larger gcode programs. Is this true? How is it done? What software?

Thanks

Eric

[HuFlungDung]

Hi Eric,

Yes it is true. The process is called DNC. There are several cnc editor programs out there that will perform this function. As a matter of fact, I believe that Onecnc is giving away a free copy of their NCLink software, which would permit you to do this. Check at onecnc.net for it.

It will be necessary to build a comm cable (if the machine does not have one) and to get ahold of the comm setup parameters so you can do this. But a resourceful guy like you will have no trouble doing that, I'm sure

[balsaman]

Hu,

I am an electrician, but the tool makers where I work were complaining. They have new mastercam software but the mill couldn't handle the gcodes of any 3d part. The guy from Mastercam said the mill needs a $40,000 upgrade to make it handle the gcodes. I told the guys I would ask here. Will the Onecnc DNC program work with any CAM software?

Eric

[HuFlungDung]

Hi Eric,

Any DNC program will likely work in the same way. It simply takes your nc-code (output produced by your CADCAM) and transmits it out the serial port a line at a time.

There are considerations, I guess, depending on what they expect the machine to be able to do. NC code for 3d milling can consist of very short line segments. Each segment is transmitted as one line of code. Depending on the communication speed capability, the machine can be "starved for data" if it can cut faster than it can receive. And, if the machine is too outdated, it will not have enough buffering capability to gather enough lines of data "ahead" so that it can assemble a smooth flowing "polyline", which leads to rough machine operation, as it pauses between movement vectors.

This could be what they are including in the $40,000 upgrade. But, just to attain the raw DNC capability should not be expensive, but it may not be satisfactory in the results, as I outlined above.

[CAMmando]

Eric,

The "DNC" method as was mentioned will work, but be subject to the speed limitations of the RS232 port. For very fine point to point programs you will suffer from data starvation. The effect of this is the appearance of a cap on the feed rate, but actually you will have dwells. This can result in poor surface finish as well as increased cycle times.

A couple of alternatives:

Depending on how big the files are you might be able to purchase more memory from fanuc. I think they call it bubble memory and I recal it was a couple grand to get to 64K 10 years ago.

Regarding the DNC method, you set the controller up as though it was reading from paper tape. That control probably has a swich that says "Tape" right on it. What I did was set up my DND server on an AB switch to the RS232 port.

There are also BTR units that emulate the Tape reader and have some Ram in them. Again these use the RS232 port as far as I know.

You may be able to have the programmers use the "Filter" option in Mastercam to generate programs that have G2 and G3 arcs that aproximate the G1 points resulting in shorter code (and usually better looking parts). The machine needs to suport G18 and G19 coordinate systems and the Mastercam post needs to suport it as well. If it is a new mastercam installation with posts based on the MP fanuc post it will.

[cadcam]

You will need to check the manual and see supports Drip feeding being able to buffer the program in the control from PC.

Your machine vat this time supports by what I can tell DNC or direct uploading.

Please tell me what Fanuc control it is please?

[sdwilson]

mastercam comes with a good DNC program, cimeco

i think what you need is a different post processor to take the mastercam code a convert to something that the machine understands, if its not g-code, we did this with a router that used HGPL code, and an old anilam control before, i bet master cam already has on for your control