Fanuc FPT transfer to cnc memory

[Jeff]

It's no secret that I f**king hate Fanuc controls.
We got a new machine with the IHMI Smart Plus and it's connected to the ethernet.

Can someone tell me the procedure to bring a file into the cnc memory?

I have the Multi-List shown where I can see both my computer programs in the top window and the cnc directory in the bottom window.

Every time I select/copy a program on the PC window then SHIFT ↓ to go to the CNC window and then Paste... it says cannot copy/move.
I've only been successful 1 time and that was a couple of days ago.


Anyone got a sledgehammer I can borrow?

[CNCAppsJames]

People that hate FACNUC controls; 999x out of 1000x have not been properly/adequately trained in the control's functions. If I had a nickel for every time I've had to follow up what some hack Applications Engineer screwed up... I'd have fuck you money.

I personally use that FANUC Program Transfer Tool ( https://www.fanucamerica.com/products/cnc/cnc-software/programming-simulation-software/program-transfer-tool ) because it allows me to communicate directly with not only CNC_MEM but also DATA_SV as long as I have the ethernet settings correct on ym machine. It's about $20.00 - ish. Works like a charm all the time. Every time. Even on some legacy controls.

In my travels, I find from time to time that communications with FANUC Controls via ethernet is an IT issue because the network does not recognize the type of network traffic CNC machines produce so it rejects the traffic. The other issue I see frequently is that parameter #929 is set to 0. This should be a 1. Putting it to 1 forces all incoming data to be ASCII.

HTH

[Jeff]

I'm using Filezilla and can see my programs at the machine no problem. Is that Program Transfer Tool better? I'll look at it.

My issue is grabbing it and putting it into the cnc memory.
I have been trying:
Select/copy.... go to cnc mem....paste. It doesn't like that.
I've done it successfully 1 or 2 times but that was a couple of days ago and apparently I forgot something.
My brain is fried the last couple of days. We're busier than a cat burying shit.

[CNCAppsJames]

Drag and drop. Copy and paste is dog shit.

[Jeff]

I figured out the issue.
It was on channel 17 instead of channel 9.
And of course "nobody" did it. Nobody has been fucking shit up for 30+ years and if I ever find that bastard I'll beat his ass.

[CNCAppsJames]

I figured out the issue.
It was on channel 17 instead of channel 9.
And of course "nobody" did it. Nobody has been fucking shit up for 30+ years and if I ever find that bastard I'll beat his ass.

[CNCAppsJames]

FANUC I/O Channels
0 and 1 = RS232
4 = CF Card
5 = Dataserver
9 = FTP
17 = USB

There's a few others for special situations but that covers 99.9% of communication needs.

You could set a G or M-Code or put a G10 line in all your programs to make sure that the IO CHannel is set to your desired device.

G90G10L52(WRITING TO PARAMETERS)
N20R9(CHANGE TO FTP)
G11(FINISH WRITING TO PARAMETERS)

[Jeff]

FANUC I/O Channels
0 and 1 = RS232
4 = CF Card
5 = Dataserver
9 = FTP
17 = USB

There's a few others for special situations but that covers 99.9% of communication needs.

You could set a G or M-Code or put a G10 line in all your programs to make sure that the IO CHannel is set to your desired device.

G90G10L52(WRITING TO PARAMETERS)
N20R9(CHANGE TO FTP)
G11(FINISH WRITING TO PARAMETERS)

No shit? Just an R9 changed the channel? That's neat.
Hey while you're here, supposedly I'm able to program a G500 R,S,C ETC..for my accuracy stuff.
It throws an alarm telling me that I'm trying to switch to metric mode or something.
We don't have the nano smoothing but we do have the AICC II 400 block look ahead.
Is the only thing I can use the G05.1 P command?
Thanks.

[crazy^millman]

No shit? Just an R9 changed the channel? That's neat.
Hey while you're here, supposedly I'm able to program a G500 R,S,C ETC..for my accuracy stuff.
It throws an alarm telling me that I'm trying to switch to metric mode or something.
We don't have the nano smoothing but we do have the AICC II 400 block look ahead.
Is the only thing I can use the G05.1 P command?
Thanks.

Yes if you only have some options then you can only do certain things.

Funny had a vendor for one customer in their shop this week. I was asked to speak to them about the process we are doing since I know it better than they do. Learned a few things, but two things stood out to me. Biggest was their 5 Axis machines are replaced every two years and everything had glass scales and the customer is using 24 year old 4 Axis machines and wondering why they can't keep up. The other thing was the vendor is not held to the same quality and inspection standards as the customer's internal machine shop is. They are given a lot more lead way on things. When I brought this up to management for the customer originally about how insane trying to hold them I was told just do what you can. After hearing this directly from the outside vendor it was oh I see why you keep saying things are different from here verse from them.             

[CNCAppsJames]

G500 doesn't mean shit to me. It's like if I told you just use G131. Unless you have a Matsuura that doesn't mean shit to you.  

Depending on the options you have (if you have a 31i-B series machine there's a few files that if you sendn'em to me I can tell you what your possibilities are. 

G5.1Q1 will activate whatever highbspeed mode you have (AICC-I or AICC-II). You "may" be able to put an R after the G5.1Q1 for accuracy levels R0 lowest accuracy to R10 for highest accuracy. If it does not have that then you would need to know yiur stuff to write a MACRO to change the acc/dec settings on the fly. There's a LOT I will do for free, teaching someone that stuff isn't one of them. It requires on-site testing and a solid understanding of FANUC Servo Guide tuning software. Bybthe time I'm done, it's cheaper to buy the options in the first place. 😆😅🤣😂

[Jeff]

It's like if I told you just use G131. Unless you have a Matsuura that doesn't mean shit to you

Okuma uses 131 also.

I'm not asking for you to teach it to me, I thought you might have an answer as to why it's giving me that alarm.
I figured if anyone knew what it was it would be you. But it appears nobody knows wtf it is.  It must be a Hyundai code then.

[CNCAppsJames]

I was being somewhat facetious in my reply. Each machine tool builder has some codes that are going to be unique to them. FANUC stuff I'm good at. That code is not a FANUC code. It's specific to your machine's builder.

I'd reccommend either calling the machine tool builder direct or your local machine dealer and getting some more info, or drag out that 2 foot thick stack of manuals you got with the machine and start digging. 

[Jeff]

I was being somewhat facetious in my reply. Each machine tool builder has some codes that are going to be unique to them. FANUC stuff I'm good at. That code is not a FANUC code. It's specific to your machine's builder.

I'd reccommend either calling the machine tool builder direct or your local machine dealer and getting some more info, or drag out that 2 foot thick stack of manuals you got with the machine and start digging.

Ok that explains why everyone I've asked has never heard of the G500.
Thanks!

Oh and under your name it says you are part of the Rebel Alliance?  Everyone knows that the Empire is the best.

[CNCAppsJames]

Ok that explains why everyone I've asked has never heard of the G500.

FANUC G-Codes that are mostly universal for all their controls mostly run from G00 to G99. Not including the Manual Guide i stuff which runs in the G2000's. There may be a few in the 100's, like G112, G113 for polar interpolation.

There should be a manual that covers your builder's codes.

[So not a Guru]

I figured out the issue.
It was on channel 17 instead of channel 9.
And of course "nobody" did it. Nobody has been fucking shit up for 30+ years and if I ever find that bastard I'll beat his ass.

Him and that dickhead Murphy!