Printable View
We are looking to add a large boring mill to our shop. Our primary product is Hydro electric turbines.
We currently have a FPT with a heidenhain 430 control. With 2gb of expanded memory. Some of our programs are over 100mb in size.
We are looking at 2 machines,
One has a Fanuc 31i-A
The other Fanuc 16i-MB
What are our options in terms of expanded memory on each?
Are they both smooth in complex surfacing applications (NURBS and Splines)?
The 31i has some newer high speed profiling options available. Fanuc memory gets expensive, fast. Data servers should be available for both controls however. Think you can get those up pretty high in the gb range.
I dont know about newer controls, but a few years ago looked at NURBS interpolation upgrade for a 15MA we were configuring for a custom 5 axis machine, think it was like a $50K option just to update...might not have been that much, but it was insanely expensive- and no we didnt get it :)
The 31i is a much better control, and allows the option for DNC operation far easier. 2GB memory cards can be used directly for this. It is also more flexible in the respect of file storage, names can be given rather than just sticking with the O**** program number format, so definately go for the 31. If you can get the 310i (PC based), that would be even better because then you get a built in hard drive.
You can also use a 4GB card for DNC if you get the right one. The one I found was the Transcend 4GB 80x (lightblue). The 4GB Trancsend will also work in your dataserver. If you are willing to spend the time and money to look for it, there is one 16GB card that works. It was a Sandisk CF card but that is all I can remember since I gave it to a customer.
In my opinion, the better option for speed reasons is a memory expansion, then comes the data server; but both options are sold by fanuc and they are not cheap, a memory card works fine and is the cheapest option, we work that way with good results.
GP.
Awesome info guys!
But now i have a couple more questions about the ATA flash card trick, as well as the data server.
1. So on board memory is 640meters (256k) for 2 machines were looking at (fanuc 16iMB, and Fanuc18iMC)
If we are using a 2gb flash memory card and use a main program loaded in the control to call a sub of say 2 million lines, We are in basically Drip feeding this 2 million line program from the ATA card/data server to the machine. Correct?
Program example:
%
O1000
(Main Program)
All your basic start g and m codes
position to machining point
(UPPER BUCKET D)
M198 P100
%
O100
(2MILLION LINE SUB LOCATED ON ATA CARD)
BLAH BLAH BLAH
M99
%
2. Im a complete NEWB when it comes to DNC, so If the above question is correct (99% sure it is). How does DNC effect program restarting after a tool failure. (Our standard procedure: Feed hold, Pressing spindle stop, recording current position, jogging away, replacing the inserts, jogging back into position, restarting the spindle, and resuming program). I know that this procedure works when running a program from the memory (as long as reset isnt pressed) but is the same gonna be true for DNC?
3. Do fanuc controls offer a direct rapid feature?
Direct Definition: The machine is at X1. Z60. Y75. | i tell them to all go to zero, G0 X0 Y0 Z0
The machine will move all 3 axis at once and they will all reach 0 at the exact same time. Just like a feed move, but at Rapid speed
Dogleg definition:
most machine's dogleg, meaning every axis moves as fast as possible and gets where its going at different times.
4.
I understand that some cards have issues being read, and that we might have to purchase a few before we get one that works excellent with our machine.
That aside though, are there any severe issues i need to know about. (Like this canned cycle wont work, or you cant use this g code because....)
#3....usually XY axis moves at 45 degrees until one end point is reached then it moves straight.
if you need that use G1 X Y Z F (F = the max feed rate set in your parameters)
As Ford stated for #3 yes the 16i, 18i and 31i have this function along with pretty much any Fanuc that I have used.
In all 3 controls 16i, 18i, and 31i it is set by parameter 1401.1 (LPR). Which if set to 0 it will move the axis in a non-linear move or along each axis independently. If set to 1 it will move each axis as to create a straight line.
Stevo
does this apply to an older 16M(1995) too?Quote:
Originally Posted by stevo1
Yes. Same parameter, same bit 1401.1Quote:
Originally Posted by VanFLT
Stevo