Guest CNC Apps Guy 1

Fanuc 16/18i Series Tip - Dataserver

Recommended Posts

Guest CNC Apps Guy 1

Hey folks, here's a way to avoid RS-232 DNC with a Fanuc16/18i control using an ATA card. This runs as fast as machine memory. We call it the "Poor Man's Dataserver" biggrin.gif So for less than $100 you can get like 4MB program storage as opposed to spending thousands. The only real draw back is the ATA card will stick out of the operator panel and you have to keep it in the slot.

 

Enjoy,

 

ATA DNC, Sub-program Call, Fanuc 16/18i controls

 

Parameter Settings: #138.7 = 1

 

DNC operation with memory card is:

0 = disabled

1 = enabled

#3404.2 = 1

 

Address P in M98 block of subprogram call function is:

0 = indicating a file number

1 = indicating a program number

#6300.4 = 1

 

External program number search

0 = disabled

1 = enabled

#6080 = 0

 

I/O Settings:

Channel = 4

 

ATA Card:

File name on card must match program number, DO NOT use filename extension. (.txt)

Example:

card filename - O0001

program number - O0001

 

Use % at beginning and end of program file.

 

Program Call:

Create program in NC memory:

 

%

O0001

M198P2 (calls O0002 on ATA card)

M30

%

 

Hope this helps someone.

 

[ 01-29-2007, 02:40 AM: Message edited by: James Meyette ]

Share this post


Link to post
Share on other sites

James,

very slick man!! this is definitely going in my cool things to save folder

cheers.gif

thanks, phil

Share this post


Link to post
Share on other sites

Hmmm..... sounds pretty neat-o. Unfortunately, I'm not as up to speed on this end of things. Can you point me to a site that shows an ATA card and how/where the thing fits into the control?

 

Thanks!!!

 

MF

Share this post


Link to post
Share on other sites

We're in the process of setting up the new machine now. Definitely will give it a try. Thanks James cheers.gif

Share this post


Link to post
Share on other sites

Well fi you got the machine to handle it here is a 1 gig card.

 

1 GIG ATA CARD

 

PC Fusions had these never used it but they had it also.

 

HTH

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

At the Operator Control Panel usually along the side of the screen is where there's a little rectangular door with a slot behind it. You put the Card in the slot.

Share this post


Link to post
Share on other sites

James,

Is this on your Mori Seiki with the Mapps front end, I have some of the older ones with the card slot on the inside of machine cabinet. Do you think it will still work.

Share this post


Link to post
Share on other sites

James also the 21i control.

 

I have found these on OKK,Yasda,Mori Seki. I know there were more just have to remember.

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

It should work with an "i" series control, but to answer your question yes this works on our CRAPPS(sic) front end.

Share this post


Link to post
Share on other sites

Thanks

I have a Mori DL151Y that I'm surfacing machining the bullet ramp of a 9mm barrel and its a lot of G-code.

Share this post


Link to post
Share on other sites

James,

I've been doing this with my new Cinci. It work great.Its a lots less of a pain than using a RS232 drip feed.

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

Craig,

 

Sounds cool. Let us know if it works out.

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

:bump:

Share this post


Link to post
Share on other sites

James,

We've been using a 128 meg compact flash card in our fanuc 18i control. Bought a couple for about 50 bucks each from Staples. Is this similar to what you've suggested? Is there a difference between the compact flash and an ata card? I'm told the control reads directly from the card. Down side is all the walking (front office PC to the router).

Marv P.

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

Sometimes the machines have compatability problems with compact flash which is why we went with ATA. I'm not exactly sure of the differences other than price ATA is about 4x more. Yes the control reads directly from the card. It's a great way to run long programs on Fanucs without having to spend a fortune on more memory.

Share this post


Link to post
Share on other sites

James you ever run a Kitamara Hortzional before with a Fanuc control and dual tombstone with full 4th axis indexing before? I think it is a 16 series Fanuc control but can not remember of the top of my head.

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

If it's say 8 years old or newer, I'd have to say yeah it's a 16...

Share this post


Link to post
Share on other sites

It is 4 years old looks pretty striaght foward but looking at some of the stuff you have put up lately was wondering if there are some off the wall things I might need to think about if I were to write programs for one. I have been keeping notes of different stuff you and others have posted. If you got a good example of tombstone stuff and maybe what I need to look out for with the exchangable pallet or tombstone would be much appericated as a reference. I am also wondering does the machine have look ahead codes as well as accel/deccel codes and amounts that you can control with G or M code or is it done with parameters.

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

It probably has look-ahead at the very least. Try it out. In MDI command G8P1, and if you don't alarm out you have it, make sure you cancel it with G8P0. Next Try AICC/SHPCC which is G5.1Q1, if it does not alarm out you have it, cancel with G5.1Q0. Next try HPCC which is G5P10000 and G5P0 to cancel. These have some specific no-no's while in effect, canned cycles, program re-start, etc...

 

 

quote:

...off the wall things...

headscratch.gifheadscratch.gifheadscratch.gif

Share this post


Link to post
Share on other sites

Well all machines have their quirks. Just was wondering what if any stood out in your mind might be. Like I seen the stagetool not to long ago where if the persons machine it had that same tool it would alarm. Not that important just more what you think of the machine more than anything.

Share this post


Link to post
Share on other sites

I've got apx. 8 Fanucs on our shop floor. One of them is a 16i with this ATA slot, but I cant get it to read/write to the same card as all the other Fanuc controls(16i - 21i). It does read a Panisonic 4mb card. The others read a Sandisk 32mb compact flash card in a adapter. Anyone hear of this? Any ideas?

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

Unless you have an "i" series control, it aint happening. The 0 control is pretty much the bottom of the barrell as far as capability goes.

 

Usually if stage tool does not work (on a machine capable of it)and alarms out it's one of three things 1) Wrong tool change format, 2) Keep relay setting needs to be changed so that it won't alarm if the tool in the spindle gets a repeat call (ex. T1 is alread in the spindle, and your program calls T1, and 3) Something is wrong with your machine.

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

quote:

...I need to look out for with the exchangable pallet or tombstone would be much appericated as a reference...

Say you have two seperate programs running on two seperate pallets. On Side A you have program O323 and on Sibe B you have program O355, you can set by macro which side will/can run what program...

 

#147 is pallet position

 

Oh the possibilities...

 

[ 07-21-2004, 05:23 PM: Message edited by: James Meyette ]

Share this post


Link to post
Share on other sites

quote:

...Like I seen the stagetool not to long ago where if the persons machine it had that same tool it would alarm...

No worries Ron. The mpmaster post won't stage a tool in the spindle. How are you going to use the HMC? High/low production? Moldwork?

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us