M198 and compact flash card on fanuc 18iM control

[Chris Parish]

Hello:

 

I have a program to big for the memory... how do I drip feed from the compact flash card using M198... I have changed the "I/O" channel to 4 to see the card but it still won't let me run the program... are there any other parameters that need to be set/ changed ??

Please let me know

Thanks,

Chris Parish

[Guest]

Check this thread out Chris

 

Linky

[Chris Parish]

John:

 

Hey ..we have an "open house" next week.. Ijust tried evrything on the "sheet".. it didn't work

 

gives me "071" data not found

 

I have a main using M98 P1234.. and on my memory card is O1234 (no extension)

 

Do you have anything else to try... please let me know

Thanks,

Chris

[iowajim62]

quote:

---

M98 P1234

---

Shouldn't it be M198 P1234 ?

[Guest CNC Apps Guy 1]

Here's the nuts and bolts of it...

 

quote:

---

Set the machine into "MDI" Mode.

Press the OFFSET/SETTING button.

Change/Set the “I/O Channel” to “4”

Set "Parameter Write Enable" to "1"

Press the Cancel AND Reset buttons simultaneously. This will clear the alarm you get stating parameter write is enabled.

Press the "SYSTEM" button.

Press the numbers "138" on the key pad then "NO. SRCH" on the soft keys (below the CRT). You'll need to set bit 7 to a 1

(Bit order is as follows - 7 6 5 4 3 2 1 0 - so you'll want to change the furthermost bit to the left to a 1)

Press "3404" on the key pad then "NO. SRCH" on the soft keys. Arrow over to bit 2 (3rd bit from the right) and change

that to a "1"

Press "6030" on the key pad then "NO. SRCH" on the soft keys. Change it to "198".

Press the OFFSET/SETTING button to get back to setting and set Parameter Write Enable to a "0". Press Reset.

---

It should be M198 if you're following the topic.

 

Never tried M98, it may work if you have "98" in parameter 6030 but I WOULD NOT do it.

[Chris Parish]

IwoaJim:

 

typo -- was supposed to be M198 (I had program right just not in forum)

 

James:

 

bonehead I am -- I changed bits from "left to right" not "right to left"... (thank god I write them all down)

 

Thank you all for helping, can't wait to cut

 

THANKS

[Storkman]

Storky misses another Optipro party.

[Moldmaker74]

Hey Storky, you didn't miss it yet. The open house is going to be on November 5&6. They don't have vodka but they usually stock alot of beer.

[Storkman]

I know Dave, but they never let me go to those things.

[MMT-USA]

Prm 0.0 = 0 (TV Check)

Prm 20 = 4 (I/O Channel Memory Card)

Prm 138.7 = 1 (Memory Card DNC Function Enable)

Prm 3404.2 = 1 (DNC Using Program Number)

[Chris Rizzo]

Can't get it to work here.

 

Program listed on card directory is: O0011

No extension, no nothing. That also is my program # within the actual program.

 

any ideas?

[iowajim62]

quote:

---

any ideas?

---

Power Down and Power back up for changes to take effect ? Just a guess. Another thing I have heard about is that certain large MB flash cards don't play well, may want to try an older 16 or 32 mb card

[Guest CNC Apps Guy 1]

Depending on the year the control was built, you may only be able to get a 256MB Card to work. (this is the size I use... and it's been a LOOOOOOOOOOOOOOONG time since I've touched a control that does not read my card.

[#Rekd™]

Hey Chris,

 

Make sure you format the card FAT32 or FAT, then try it.

 

Can you punch a file to your card from the control?

 

John

[Chris Rizzo]

I can DNC off the card no problem (been doing that for a while). It would be "more foolproof" for the operators to find and load a local main program than having to call the correct program via tape mode off the card. Not to mention the option to add all sorts of comments in the local prgrams. Right now I have them start DNC in single block, so they can confirm the correct program is running, and if there are any special notes.

 

I'm getting alarm 071, data not found.

[Guest CNC Apps Guy 1]

8-/

 

Chris, you've got mail...

[Chris Rizzo]

Ok, figured it out. After a power down/up it now works.

 

Sometimes leaving things for another day fixes the problem!

[iowajim62]

quote:

---

After a power down/up it now works.

---

Nice

[TK-32™]

Well, I run into this problem today and searched the forums.

This was driving me nuts because this worked on our robodrill but not on the Hwacheon.

My problem was in parameter 3404 Bit #2. Machine was set at 1. We had to set it to 0.

I guess setting it to 0 means calling a "Files Number" from the memory card

I know the majority prefer to set it to 1. I'd like to know if there's a benefit to running it like this. Maybe in case the file number changes?

 

This is our first attempt at lights out and for a moment I though this was not gonna happen. We made fixtures and other stuff to put four large parts on the machine. I was worried haha

 

This forum is a wealth of knowledge!!!

and thanks Ron, CrazyMillman, for letting me know about M198!!!

 

Posting the following picture in case it helps someone down the road.

[Alvaro Gil - Cimquest-inc.com]

Just wanted to revive this old thread to say thanks!  After two reboots, the search by file name started working for me also!

 

Just a note, with a dual stream machine you can only DNC to one control at a a time. The other stream must be run off the controller.Thanks, works great.

Post from Guest_CNC Apps Guy 1_* was awesome - just waht I needed.