New Job, New Machine, Need help setting up DNC from PCMCIA

I have started a new job at a wonderful little shop and I have the pleasure of running a brand new Doosan DNM 500II. I also have the pleasure of figuring out all the normal stuff that is "already taken care of" at most machine shops. Little things like programming tweaks, DNC, setting up a tool library, setting up.... well.... most everything. We are not a machine shop, though we do a lot of machining, and this is their first VMC.

I was a little leary of the Doosan at first, especially with the Fanuc control (I have not had much good experience with them) but I am humbled at the abilities of this machine. I program from Solid Works which is a dream and a breeze (most of the time).

The issue I have been running into is the insanely small memory on this machine. It is somewhere in the neighborhood of 240K. We are using HSM Express (Free 2D and it is awesome) and even with some boring cycles and adaptive clearing we have issues with program size. So I am trying to set the machine up to DNC from a CF (PCMCIA) card to negate this issue until we have time to hook the machine up to our network and set it up to DNC drip feed.

My problems are pretty basic. At this point if I put a CF card in the machine, the machine errors and says it is not formatted. If I format the card on the machine, my computer will not read it, saying it needs formatted.

I am formatting the card at startup as the formatting in the machine control always gives me "card failed to format". I have tried different cards.

I am SURE I will have more questions once we get past this issue. Any suggestions? What am I doing wrong?

Maybe check out this thread... http://www.practicalmachinist.com/vb/cnc-machining/flash-card-work-fanuc-but-not-mitsubishi-234192/
Hopefully it can help you out a bit.

What is your I/O channel set to? (Found on the SETTINGS display screen, under "Handy Settings". I believe for the PCMCIA card, it should be set to 4. I believe for a USB drive to work, it should be set to 17.

Have you tried loading a program onto the card, and see if you can see it from the directory screen? Edit > Program > Directory > Operator > Device Change > Memory Card should display the card, if it's enabled. FYI, I've never had any formatting issues with our machines, and I use the memory-cards for all file transfers.

I/O channel is set to 4, normally it is set at 17 as we transfer the majority of our programs via USB.

Ok, tried loading a program into the memory card, though I am not sure if I am doing it right. Here is what the control looks like in Edit, Device, Memory Card

Make sure your flash is 256 or 512. I think the cards with more memory are formatted differently and are not compatible with fanuc.

What about a 64MB card? I laughed when I saw the card. I did bring a 1G from home to try, but don't want to use it unless I have to, it is for my camera, and is a high speed card.

On our doosans, they wont take the larger capacity cards. not sure why, but i can only get the 1 and 2 gb cards working.

Fal Grunt said:

I/O channel is set to 4, normally it is set at 17 as we transfer the majority of our programs via USB.

Ok, tried loading a program into the memory card, though I am not sure if I am doing it right. Here is what the control looks like in Edit, Device, Memory Card

View attachment 127681

Click to expand...

That's the right screen, although the card is empty. Are you saving your files as .NC extensions? Also, make sure the first and last lines are a % symbol, with nothing else on them... My card is 512kb.

I'm curious - if you have a USB drive, why not use it?

Yea, the card is empty, that is the issue! If I format it at the machine, I cannot use it at the computer. If I format it so I can use it at the computer I cannot use it at the machine.

I tried loading a program from the control to the card and was unsuccessful. Though that may be me and not the machine.

Subsequently, the programs are written as .nc, I modify them to be nothing (as I was told by Doosan) and they do have the % at the beginning and end. But at this point, that is a moot subject because I cannot get them onto the card and then to the machine for it to even be an issue.

We use USB for the majority of the programs, however the control does not have enough memory, about 240K, to load the program I need to load. The program I want to load is 520K or there about.

we used to put long programs on the cards
and use a
m198
that would call out a sub from card
and a
m199 would get you back to your control
so all that was on your control was a small program that called out the big one
instead of .nc
have you tried .iso
that is what our fanucs would read
and like moto said
anything bigger than 2 gig
never worked in our mills
keep your file alone
and not in a folder on your card
they wont read whats in a folder
thats about what i remember
i think

Fal Grunt said:

Yea, the card is empty, that is the issue! If I format it at the machine, I cannot use it at the computer. If I format it so I can use it at the computer I cannot use it at the machine.

I tried loading a program from the control to the card and was unsuccessful. Though that may be me and not the machine.

Subsequently, the programs are written as .nc, I modify them to be nothing (as I was told by Doosan) and they do have the % at the beginning and end. But at this point, that is a moot subject because I cannot get them onto the card and then to the machine for it to even be an issue.

We use USB for the majority of the programs, however the control does not have enough memory, about 240K, to load the program I need to load. The program I want to load is 520K or there about.

Click to expand...

Can you not drip-feed from the USB drive? (I've never been a drip-feed fan, and have rarely ever used it...)

The .NC file extension should work... I know if you output a program to the card, it creates a no-extension file-type. You can load that no-extension program back onto the CNC control, or even another machine. I do this sometimes when copying/transferring programs between identical machines.

To put a program onto the card...

EDIT > PROGRAM > DIRECTORY > OPERATOR > DEVICE > CNC MEMORY > F OUTPUT > type in the program, do not include the "O" > O SET > EXECUTE You shout see the word OUTPUT flash on the bottom left corner. There is no confirmation, although it might flash back to the normal program screen. Go back and look at the memory card to see if there's a file on there - there should be...

FYI - Everytime I plug a card/USB into my computer (Windows 7) it prompts me to "SCAN AND FIX" the device, or "CONTINUE WITHOUT SCANNING". I open without scanning everytime... See if your computer behaves that way. I don't think I've ever formatted a USB or memory card for CNC use, ever...

Fal,
Glad you like the Doosan. I am an applications engineer for Doosan. You can contact me here, [email protected], for any help you may need. Good advice here, all of it. You should not have an issue with your card. I use them all the time even after formatting them on the PC. You do need to format them using FAT file system and I believe 1K packet size. You can only use the USB to load and save programs, you cannot drip feed from them. That was a safety issue I am told. What if someone yanks the stick or bumps it? On the Oi control, it is easier to save you programs with no extension. On the 30 series controls it doesn't matter. The Oi is not happy with extensions. Just my experience.

Paul

Oh BOY!

I re-formatted the 64MB card on the computer, 1024 file type, FAT system, dropped my program on it and now the machine recognizes it!

Jashley, I was also able to output a file to it.

YAY!

Now, I cannot get it to DNC drip feed from the card. The two sets of instructions I have (one from the Doosan Manual) do not match the buttons I have available.

One set is as follows:
TAPE
Program (hard key)
+ twice (soft key)
DNC-CD (soft key)
DNC-ST (soft key)
cycle start

Other:
Edit mode
Program
+
Card
Oprt
F Read
File #
F SET
Program #
O Set
Exec

Thank you MUCH everyone for your help so far.

LockNut, my experience comes from Hermle, Deckel, and Mazak, most of my experience from running Mazak's. I have to say, this machine is no mazak, but it IS a good machine. Very accurate, VERY quick, sometimes confusing to run, but what I think is intuitive is not always what someone else does.

Fal Grunt said:

Oh BOY!

I re-formatted the 64MB card on the computer, 1024 file type, FAT system, dropped my program on it and now the machine recognizes it!

Jashley, I was also able to output a file to it.

YAY!

Now, I cannot get it to DNC drip feed from the card. The two sets of instructions I have (one from the Doosan Manual) do not match the buttons I have available.

One set is as follows:
TAPE
Program (hard key)
+ twice (soft key)
DNC-CD (soft key)
DNC-ST (soft key)
cycle start

Other:
Edit mode
Program
+
Card
Oprt
F Read
File #
F SET
Program #
O Set
Exec

Thank you MUCH everyone for your help so far.

LockNut, my experience comes from Hermle, Deckel, and Mazak, most of my experience from running Mazak's. I have to say, this machine is no mazak, but it IS a good machine. Very accurate, VERY quick, sometimes confusing to run, but what I think is intuitive is not always what someone else does.

Click to expand...

You won't be able to "drip feed" from the card in the conventional sense. You will need to make your program a sub-program stored on the card. Your main program will reside in memory. You can call the program from the card using M198 PXXXX as described by another member in a previous post. Instead of an M30 in your sub, use an M99. This will kick you back to your main program. This seems to be the easiest way to run a larger program that won't fit in memory.

An M98 calls a program from machine memory, an M198 calls a program from the card. An M99 sends you back to the main program regardless.

Paul

rehello
it will be easier if there is only 1 program on your card
we did this years ago so maybe things changed
but with 1 program on your card
you would use
m198 p0001
the control reads the position of the program on the card
if you have 5 programs on your card
the position of the program as the control sees it is your p #
at least that how it was years ago
hope this helps
left you a pm as well

As others have said to call it from the card you make a main program on your control and call it as a sub

So...
O0001 (This is the program on your control)
M198 P1 (Ok this is where it gets tricky, it depends on how your parameters are setup. If parameter #6300.4 is set to 1 then what you have to do is go to the directory where you can see which number the control has assigned to your program that you want to run. It will be on the left hand side. If parameter #6300.4 is set to 0 then when you save your program to your card you will have to change the file name to a number of your choice. I use #6003.4 to 1 and just see which number the control assigns to it.)

Now what the others have said about file types that the control can read... From my experience all my Fanucs can "see" .NC,.TXT and .ISO it actually has never mattered. Also someone said that at the end of your program on your card that instead of a M30 use a M199 or M99. I have NEVER had to do this from the card. I even read programs from the control to the card that send it back to the control to read subs and back again to the card without issues as long as the subs in the control memory have an M99 at the end (If that makes sense). All my programs on my card have an M30 at the end of them and when they have finished running it still sends them back to the main program on the control.

I have had problems before with formatting cards and it totally messed them up. The best ones that I have bought so far are Transcend 1GIG cards that read straight out of the packaging without having to format them.