-
I never understood what Fanuc people meant by Fansuck until this 5700.
This is our first Fanuc mill. We have a Hurco mill that we previously had. We asked some questions of the sales guy who suggested tape mode would allow us to run programs of enormous size from RS232 with normal functionality- specifically search, replace, edit, restart.
In reality you lose, search, edit, re-acquiring the program and can only regain some function by programming the single path machine like a cumbersome multi-path machine using 198 calls for multiple programs by tool -(programs that also cannot start in the middle because Fanuc won't allow you to search the 232 program). It's a waste of time, now I realize why people don't want to buy fanuc controls on mills. This is probably the side of the house where Fanuc gets the **** kicked out of them. Our other 5 Fanuc controls are multiaxis turning, and we don't seem to have problems getting programs to fit in the control memory.
When the solution to the problem is do **** harder and get more headaches to get the job done that's a motivator to buy something else. I had about two days of workholding jobs - 4 different jobs all settup with programs supplied in 2 hours on the first day. Dancing around with G68 angle skews and tape mode has probably added two days to that work. I can see the operator body language saying, "I'm really frustrated with this crippled operating condition and these hurdles", and that guy has a good attitude. I dislike strongly when outside conditions effect my employees enjoyment of work because that tells me this stuff is pushing those people closer to a place where I can't compete and keep them.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
OK, running from "TAPE" mode is one way to run a large program. But somewhat balky. I prefer running from the PC card slot, I/O channel 4. Much easier.
You make each tool a "program" on the card, ie - Center drill is O0001, Drill, O0002, etc.
Then, On your CNC memory, you would write a main program -
%
O1000(MAIN 1)
M198 P1;
M198 P2;
etc.
M30;
Now, you can run LARGE programs without a balky RS 232 connection, plus MUCH easier program restart and re-run.
The G68 function would be in one of those programs with your angle tolerances inserted, and you can run.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
When you and your guys are ready. Training is free. For life. As long as you have a Doosan on your floor.
All you have to do is get here. Lunch and coffee are free. Make your own travel lodging arrangements, and two days, hands on, here in the showroom.
You register for free online:
https://doosanmt-training.coursestorm.com/
Knowledge is power. Come get some.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Quote:
Originally Posted by
DouglasR
OK, running from "TAPE" mode is one way to run a large program. But somewhat balky. I prefer running from the PC card slot, I/O channel 4. Much easier.
You make each tool a "program" on the card, ie - Center drill is O0001, Drill, O0002, etc.
Then, On your CNC memory, you would write a main program -
%
O1000(MAIN 1)
M198 P1;
M198 P2;
etc.
M30;
Now, you can run LARGE programs without a balky RS 232 connection, plus MUCH easier program restart and re-run.
The G68 function would be in one of those programs with your angle tolerances inserted, and you can run.
Based on the short time we've been working with this, it doesn't seem there is a training solution to this problem. I do appreciate the offer, but our people are busy trying to produce work with the machine.
It is a pretty large weakness in the machine, and that's obvious, but this is difficult to figure out a solution to. We did call fanuc, and our Ellison application person, who basically confirmed there is no way to run a somewhat normal CAM produced mill program in the machine without using some form of drip feed and awkward method of running the program. We did figure out the
Program start of main program
M198 P0004 (program O0004 ending in M99)
M01
Program continues ending in M30
Method of programming the machine, but that was the less handicapped version that still represents an abnormal way to run the program that costs extra time and takes most of the control away from the operator. (edit, restart, search etc)
In this case we specifically asked a pre-sale question about the small control memory and being able to load and run large programs normally with search, edit, restart, and other functions normally in easy guide I. We were told by sales rep that that was possible through the fanuc card slot and the only weakness of the method was literally the card being in the slot.
That wasn't true- probably a lack of understanding by the rep. "No weakness" doesn't cost 25-50% of the time negotiating 2 days of prove outs. - Litterally oh **** moments where the program is stopped, and we have to re-run large sections of code over just to get back to where we were. - machine movement, spindle rotation, needless wear etc. Fanuc did that. They sucker punched the customer with the lack of control from the card.
Now apparently maybe the Fanuc data server is a way to confront the reality that the machine has insufficient memory for normal CAM programs on mundane parts. I don't know what that option costs, but it should be something Fanuc just does to be competitive, because the machine has nearly no memory. Solid state 250gig drives cost $60-100 and shouldn't reduce the reliability of Fanuc's hardware only machine because they are solid state hardware.
Doosan did a good job making the machine. Fanuc is just cutting its balls off. Fast tool changes are negated if your people are spending hours to proove out parts because they hit a button and have to restart from the beginning a long section of drip fed code, or because they have to load several programs and weave them together like a programmer to get the machine running.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Or you could do what I did with my lathe and rip out every piece of hardware that says Fanuc on it, and replace it with something that works and is user friendly. :D
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
There is a data server option that can be field installed.
Also, if you are aware of the M198 function then perhaps you can exploit it to your advantage. You can divvy up the roughing sequences etc to make it easier to tackle.
Just tryin' to help.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
I was doing really pathetic stuff like cutting one set of step jaws on a two station vise and having it consume 30000 lines of code roughing with a dynamic mill path, and that was more than the control could let me load, so we were spending more time jockying with files than actually machining parts. I talked to some CAM gurus on a Mastercam forum who gave me tips to condense the paths to 25% of their size.
That doesn't take away the fact that Fanuc's memory is embarassing, weak, and pathetic, but it does possibly reduce the extent to which I will run into the problem. We intend to do production work, up to 24 parts in the machine at a time with workholding we already have, so 25% of the size probably won't eliminate the problem.
I think the Doosan machine is better than the Fanuc control at this point. In my couple of years shopping around, program memory is the worst beating Fanuc takes. The I series Oi's are behind the times in block read speed, look ahead, and program memory. It is easy for people not to notice block read speed, but look ahead and program memory are pretty important today.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Quote:
Originally Posted by
Green0
I was doing really pathetic stuff like cutting one set of step jaws on a two station vise and having it consume 30000 lines of code roughing with a dynamic mill path, and that was more than the control could let me load, so we were spending more time jockying with files than actually machining parts. I talked to some CAM gurus on a Mastercam forum who gave me tips to condense the paths to 25% of their size.
That doesn't take away the fact that Fanuc's memory is embarrassing, weak, and pathetic, but it does possibly reduce the extent to which I will run into the problem. We intend to do production work, up to 24 parts in the machine at a time with work holding we already have, so 25% of the size probably won't eliminate the problem.
I think the Doosan machine is better than the Fanuc control at this point. In my couple of years shopping around, program memory is the worst beating Fanuc takes. The I series Oi's are behind the times in block read speed, look ahead, and program memory. It is easy for people not to notice block read speed, but look ahead and program memory are pretty important today.
I am sorry your having an issue with the Fanuc. I have a couple of comments. First, Doosan picks the CNC they offer on the machine including all the options and storage. The person who purchased the machine also had a say on what the machine specification were. Finally if a Cam system produces 30k lines of code to do some roughing on step jaws, then you should really look for a better cam system. To me it look like someone dropped the ball before you started working on the machine. Fanuc can be a pain some days, but day in and day out if you want to make money with your machine, Fanuc just works, day after day after day......
Best of luck I hope you fine an answer that fits your needs. While data server works it is not a direct replacement for part program storage.
-
1 Attachment(s)
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Dynamic milling is awesome. Here are the tips you probably already know, but the defaults are suck for short programs.
Also remember that the entire point of dynamic paths is to reduce depth cuts, so make your depth cuts your entire cutting length of the end mill. I have seen programs in the wild that are 3MB when they only needed to be 300K.
In the example bellow I leave .02" on the XY. This will guarantee no over cutting. Might want to leave more if more aggressive, tool flex will take off more material than you expect at large depth cuts.
TIP: the total tolerance is what makes toolpaths really small. There is no reason to hold it at .001 especially if you are leaving lots of stock. Open that up and let mastercam make huge arc moves to replace many many line moves.
Attachment 408252
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
I'm pretty sure we actually forgot how to drip feed from the card from a program call. I paid someone to figure it out again and write the procedure down. I guess we should have made that a written procedure. These secondary problems are such that in hindsight I would have just bought a Hurco or DMG mill if I had known what a pain in the ass it would be to run the machine. We have a macro now that does some memory saving function from some CAM guru but we don't even know what it means or how to use it- I'll drop that in below.
We called about a memory upgrade today, and Fanuc only offers 2MB (so 4 times not **** for memory) max storage on this low numbered control (there was no higher numbered option for the DNM5700). With our 31I B lathes we did a memory upgrade to 4MB (smaller than the 8 max because lathes don't get too crazy for lines of code) for $1700 per machine $425 per MB. Ellison/Fanuc wants $2000 for these 2MB $1000 per MB. In 1996 Nintendo released Tales of Phantasia and Star Ocean for $69 and it had 48MB of ROM memory- $2.30 per MB when adjusted for inflation. Fanuc apparently punishes customers for their failure to design adequate memory into their control. The program memory is just embarrassing.
here's the Greek macro that is intended to allow recycling code on different offsets to help the small minded Fanuc keep up.
O1000 (MULTI-OFFSET MACRO)
(MACRO RUNS SUB PROGRAMS STARTING AT G54 SUB PROG O1001)
N10 (MACRO SETUP/INITIALIZE)
IF[#510EQ1]GOTO20 (SKIP IF INITIALIZED)
G4X.1 (STOP LOOK AHEAD)
#500=10. (TOTAL NUMBER OF OFFSETS)
#501=1. (FIRST OFFSET, 1=G54.1P1)
#502=1001. (FIRST SUB PROGRAM)
#510=1. (SET INITIALIZED)
N20 (CALL OFFSET)
IF[#501GT#500]GOTO9000
G90G54P#501
G4X.1
N30 (SETUP SUB PROG NUMBER)
G65P#502
#501=[#501+1]
#502=[#502+1]
M01
IF[#501LT#500]GOTO20
G4 X.1
N40 (END ALL)
#501=1.
#510=0.
G4X.1
N9000 (ERROR - OFFSET OUT OF RANGE)
#300=1(OUT*OF*RANGE)
M30
I just got an update, and that remembering how to wrestle with Fanuc and squeeze some capability out hasn't happened yet. I'm just really unhappy with the **** piss memory of this machine. It just handicaps the hell out of a decent machine. You can't for any reasonable cost buy an actual solution to this problem. 2MB is apparently it. Everything else runs differently as far as people are telling me. You just can't pretend this machine is competitive with anything out there like this. Even HAAS has 1GB standard.
Fanuc should send everyone an apology letter with the 2MB for free and say, "We're sorry we're just incapable of being competitive on this."
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Can you post a picture of the part you are doing with a ruler next to it. Or better yet the entire fixture on the machine. Then we can get an idea if its a programming issue that can be solved with CAM or if the part is just too complex for the control.
2MB is a fair amount of memory. Unless you are doing something very memory intensive like 5x milling or intense 3D surfacing it will suffice for the majority of 2D and 3D parts. A picture of all your tool paths in backplot with the dots turned on will also help.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Quote:
Originally Posted by
avongil
Dynamic milling is awesome. Here are the tips you probably already know, but the defaults are suck for short programs.
Also remember that the entire point of dynamic paths is to reduce depth cuts, so make your depth cuts your entire cutting length of the end mill. I have seen programs in the wild that are 3MB when they only needed to be 300K.
In the example bellow I leave .02" on the XY. This will guarantee no over cutting. Might want to leave more if more aggressive, tool flex will take off more material than you expect at large depth cuts.
TIP: the total tolerance is what makes toolpaths really small. There is no reason to hold it at .001 especially if you are leaving lots of stock. Open that up and let mastercam make huge arc moves to replace many many line moves.
Attachment 408252
Thanks for that - I'm going to try that to help make the modern programs off the most popular CAM system in the US CNC industry more compatible with Fanuc's abysmal memory.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Filtering your tool path like that will make it run faster on any machine since it will have to process 10X less code. Please try it. The cam system defaults are set up to work in 95% of cases. Unfortunately that also kills performance. If you can send me your mastercam file and I can inspect it for you.
AG
-
1 Attachment(s)
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Quote:
Originally Posted by
avongil
Can you post a picture of the part you are doing with a ruler next to it. Or better yet the entire fixture on the machine. Then we can get an idea if its a programming issue that can be solved with CAM or if the part is just too complex for the control.
2MB is a fair amount of memory. Unless you are doing something very memory intensive like 5x milling or intense 3D surfacing it will suffice for the majority of 2D and 3D parts. A picture of all your tool paths in backplot with the dots turned on will also help.
I was just making 6 1.25" size approximate parts in aluminum from extrusion per load- that's 2 6 part fixtures half op 1 half op 2, and we used arc filter to get that down to 266KB of the ~512KB so that we could fit it in the control. We originally were thinking of using 2 more stations but that would double the amount of code and wouldn't fit so we ditched half the stations from the start. Everything we've done in the machine has been a battle with memory- I think every job has gone in, needed to come out and be modified or something to get it in and running.
Attachment 412360
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Are you using sub programs? Mastercam will spit them out automatically with a transform operation. If I had to guess with the very limited info I have, you should be in around 32K.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Don't get me wrong - I do agree 512K these days sucks.
What you need to do is:
1 - dynamic toolpath for roughing out all 6 parts in one shot. This should be done with with no depth cuts! Filtered.
2 - the program for every part should be wrapped in a transform operation. The transform operation should be in incremental - the button on the right.
I happen to be working on a similar example right now: https://i.imgur.com/rna8q5H.png
Post the dynamic and the transform operation.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Quote:
Originally Posted by
avongil
Don't get me wrong - I do agree 256K these days sucks.
What you need to do is:
1 - dynamic toolpath for roughing out all 6 parts in one shot. This should be done with with no depth cuts! Filtered.
2 - the program for every part should be wrapped in a transform operation. The transform operation should be in incremental - the button on the right.
I happen to be working on a similar example right now:
https://i.imgur.com/rna8q5H.png
Post the dynamic and the transform operation.
I don't honestly know what memory the machine has. Maybe it is 256. I thought it was 512, but I can only get about 28,000 or so lines and it seems like on the milling side that's not enough a lot of the time for even one program to be stored. Our lathe programs go up to about 14,000 and our lathes have 4MB, so we can store many programs in the control.
The program right now is running we're just running it on half the vises in the machine. I got a quote on the 2MB today, but I wasn't expecting it to cost more than the 4MB upgrades for the 31I Yama Seiki lathes we have at $2000 vs $1700. I have a friend who said he would ask a Fanuc guru if the data server option allowed Search up down, find replace, edit, optional stop, and restart capabilities like the ROM memory. It was my understanding Fanuc had no answer to this problem except to say, we can give you 4 times the nothing you have for $2000 so you can have more nothing, or drip feed.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
I just saw the picture of the parts. That should be a 32K-64K program. Use my example to get it there with sub programs. I think using a main program and subs in incremental is better because it removes any possibility of a stacking error. (I need to test this idea - don't quote me yet)
Also if you have to make some kind of minor change, you just make it in the sub on the controller.. For example a federate in a problem corner.
I do agree it sucks that you need to change your method for this particular part but its always great to learn new methods.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Hey, just saw the crazy macro bellow...
Try the sub program method in incremental. Removes all this hogwash....
Main program goes to X, Y location and runs sub in incremental code. Then the new X Y location and runs it again.... So its say....
:1001(MAIN PROG)
G54 (VISE 001)
G90(ABSOLUTE MODE)
G0 X0 Y0;
M98P1234;
G90(ABSOLUTE MODE)
G0 X2 Y0;
M98P1234;
G90(ABSOLUTE MODE)
G0 X4 Y0;
M98P1234;
G55 (VISE 002)
G90(ABSOLUTE MODE)
G0 X0 Y0;
M98P1234;
G90(ABSOLUTE MODE)
G0 X2 Y0;
M98P1234;
G90(ABSOLUTE MODE)
G0 X4 Y0;
M98P1234;
M30;
:1234(SUB PROG )
G91 (INCREMENTAL MODE)
lots of g-code here...
M99;
Does that make sense?
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
I ran those filter settings by the guys on the Mastercam Koolaid forum on Facebook, and most of those guys were saying they run .001 to .003" on the tolerance setting typically less than half or severely less than half the finish stock value, nobody confirmed .011 would work for .006" of finish stock without gouges. I'll have to just try that your way at some point and see if it works. Those guys obviously mostly have controls with 1GB storage (Okuma, Hurco, DMG etc), and don't ever have to crush a program into a tiny amount of lines of code. This is aluminum so we are taking like 35% stepover where steel would be 12% or so and triple the number of lines of code. I've been told not to use operation transforms in Mastercam because sometimes unintended results happen. I didn't know Mastercam could post subprograms. Mastercam doesn't really push a free and available training doctrine for the product, so every user knows something another user doesn't and no one knows it all, or really even most of it. I've got something like $26,000 invested in Mastercam training and mastercam training video product from third party providers and I realize I'm going to be slowly learning Mastercam for the rest of my life, or until I switch to a different product.
Obviously if the Fanuc data server doesn't operate like program memory we're going to have to start using sub program calls- which is like the second programming task on top of making the program. My macro was intended to allow the same code to be used over and over to condense file size but I don't understand it. This simple memory problem costs a lot of time, it's been probably 10 hours on the floor already in only a few months of machine ownership. I'm going to try to streamline that into a word document explaining to the operator how to run a program, a folder for every job with multiple programs, this will cost some time on every programming solution, and some time for every machine settup and prove out. It's probably going to cost hundreds of hours of lost time over the life of the machine.
Fanuc is just not thinking if they think this isn't a huge problem for their sales on the mill side.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
I don't know how old your controller is, but from your description is sounds like Fanuc is making controllers from the Jurassic epoch. The world has passed them by, no point in changing anything that has been working for the last 30 years.
I don't know what I would do if I couldn't run 1,000,000 line G code files on my mills. Modern adaptive clearing and trochoidal tool paths require enormous files. Memory and modern processors are cheap, but system redesign is a bit pricey.
On the parts that you show above, I would run about 30 of those per pallet on the Haas.
You might also look at Fusion 360 as an alternative to Mastercam, but it won't fix your memory issues. Much more user friendly, and incredible free support and tutorials.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
The tolerance is the value that it will step outside the profile you selected. Typically by about 1/2 of that . You need to leave enough stock to clean up for two reasons:
#1 - the filter settings. If you want a short program try a big number like .01" be sure to leave .020 at least. If you are only leaving .006, then you should certainly use .002 or so.
#2 - tool flex. You have to leave enough material so the tool flex does not dig in to the finish. This could be quite a bit.
Yes, I agree with your % step overs also. Even less for small tools.
Unfortunately, the smaller the part the more memory it uses. You can certainly be under 64K I think.
Certainly use and learn the XForm operation. It is very powerful.
Sounds like you have your Dynamic path figured out. I am going to double down on using the Xform toolpath to make sub programs in incremental mode.
Mastercam is the swiss army knife of CAM for milling. It can be very easy to use, or you can open the more advanced tools and do just about anything. You will learn it forever because of new functionality added yearly.
Send me a PM and send the file over to me, I can take a look at it for you. I'm really swamped though, wont get to it for a while.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Thanks I guess the info I got was right then. Half the stock allowance value. So I can't really make the program smaller. I've seen transform not work properly so I can't trust it. I also don't use it for lathe milling operations for that reason.
I found this page where it appears Fanuc is just being dishonest about reality. Someone said I should e-mail them despite the fact I've already called them and they were no help at that time.
https://www.fanucamerica.com/product...dMXXtxsQU8upFA
This part particularly "Part programs stored in external memory cards or in the Fast Data Server can be edited and executed just like internal memory, providing practically unlimited capacity." That is basically what my sales guy told me - I would have no loss of control functionality on the card- the only difference would be the card sticking out of the slot. I haven't found that solution yet. I couldn't care less if the program is on a card, but I want to be able to search, find and replace, and restart wherever I need to and run the machine normally.
I guess if there is a solution not being able to get that from Fanuc CNC support shouldn't be a big surprise. Fanuc offers courses that they don't even put their own field technicians through. So really the problem with getting Fanuc support is that the guy you call at Fanuc very probably doesn't actually know fanuc. They might have one person who knows the solution if there is one, and he's a special guy that will be hard to find even within the organization of Fanuc.
This is why forward thinking companies like HAAS making videos is so much better than the approach of the industry at large. Fanuc, Mastercam, Hurco for sure, even Doosan could use this kind of approach. When people know how to use the product, they are going to be more successful and that will result in more sale of the product.
I have a MC machinery Mits EDM machine, and that thing has like a 2 hour course on just managing consumables. Basically they had a lot of stuff they wanted customers to pay a lot for, so they designed a complicated procedure to re-use all those products like 12 times so that the high cost of the consumable product could be called affordable. But you have to do all those procedures properly, and you see that stuff for like $200 an hour, and then 1000 hours of operation later you have to recall that information, or pay a field guy to come out and show you again. It's bull****. That's a video. That's how you resolve that and have happy customers who don't live in fear of the future.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
The Transform operation is the solution. It has been around for a very long time. If you check off the options I suggest before you problem will be solved.
I have implemented thousands of times and use it at least once a week. I cannot imagine not using it.
-
4 Attachment(s)
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Hello Mr. Green0,
Your link to Fanuc's website doesn't bring you anywhere.
https://www.fanucamerica.com/product...dMXXtxsQU8upFA
Last year a Fanuc-tech guy [Fanuc Europe] visit our shop and I asked him about the [FANUC] memory problem.
He advised me the FANUC Memory Card Progam Edit Tool Version: 5.00 - Fanuc A08B-9010-J700/ZZ11
It's for the 30i - 32i series but on our 0i-MF with 512kB memory it works as well, maybe it works on a 0i-MC or a 0i-MD also.
We run some programs up to 3Mb without problems.
Normally when we machine multiple parts all the g-code (absolute-G90-not incremental) are stored in sub-programs.
We shift Work-Offset by G52 so the code is written for only one part, that's something that you also have to do.
You contacted Fanuc but didn't they told you anything about this tool ???
FANUC Memory Card Progam Edit Tool Version: 5.00 - Fanuc A08B-9010-J700/ZZ11
We purchased it at FANUC Europe for only € 20,- ( $23,- ) !!!!!!!!!!! ????????
Contact Fanuc again and ask them about this tool, A08B-9010-J700/ZZ11
It runs only from (PCMCIA) flash card, not from USB, it can run programs up to 2Gb !
You can make changes into the g-code, when you drip-feed or using M198 that's not possible.
This tool is not tape/dnc dripfeeding but it makes a BIN-file and runs from [MEM].
I ask myself, why is this tool not known by Fanuc users or tech-guys ?
Regards,
Heavy_Metal.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
.020 or more of stock is going to require 2 finish passes so it's not an option in production machining so the arc filter can't really resolve this issue properly. I don't know anything about transform operations. Every day I learn something about Mastercam, but I have a long way to go. There isn't a youtube video on how mastercam posts to Fanuc controls with 512KB or less of memory. This whole time I've been hoping Fanuc could tell me what a solution is, and prove their control sold on new machines isn't totally obsolete. It sounds like Fanuc doesn't have a solution.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Quote:
Originally Posted by
Heavy_Metal
Hello Mr. Green0,
Your link to Fanuc's website doesn't bring you anywhere.
https://www.fanucamerica.com/product...dMXXtxsQU8upFA
Last year a Fanuc-tech guy [Fanuc Europe] visit our shop and I asked him about the [FANUC] memory problem.
He advised me the FANUC Memory Card Progam Edit Tool Version: 5.00 - Fanuc A08B-9010-J700/ZZ11
It's for the 30i - 32i series but on our 0i-MF with 512kB memory it works as well, maybe it works on a 0i-MC or a 0i-MD also.
We run some programs up to 3Mb without problems.
Normally when we machine multiple parts all the g-code (absolute-G90-not incremental) are stored in sub-programs.
We shift Work-Offset by G52 so the code is written for only one part, that's something that you also have to do.
You contacted Fanuc but didn't they told you anything about this tool ???
FANUC Memory Card Progam Edit Tool Version: 5.00 - Fanuc A08B-9010-J700/ZZ11
We purchased it at FANUC Europe for only € 20,- ( $23,- ) !!!!!!!!!!! ????????
Contact Fanuc again and ask them about this tool, A08B-9010-J700/ZZ11
It runs only from (PCMCIA) flash card, not from USB, it can run programs up to 2Gb !
You can make changes into the g-code, when you drip-feed or using M198 that's not possible.
This tool is not tape/dnc dripfeeding but it makes a BIN-file and runs from [MEM].
I ask myself, why is this tool not known by Fanuc users or tech-guys ?
Regards,
Heavy_Metal.
That's really totally bazaar. I opened the manual. Read it. Really didn't understand it. It may be the solution. Like all things Fanuc they made it hard to grasp.
Is that not available in the USA?
-
Use .002 in filter settings if you are leaving .006.
I have fit parts like that on multiple fixtures in 64k. This is easy to do if you use Filter settings and xform properly. Send me your file or call your dealer.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Hello Mr. Green0,
I think the program is available in every country.
Tell us what Fanuc series do you have, it needs at least the 0i-series.
I can make a BIN-file for you that you can try to run from card.
You have to upload some nc-files that you want to try.
Regards,
Heavy_Metal.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Hi guys,
There is a video on Youtube with the Fanuc Memory Card Program Tool v4.
They show the Program Tool on a Fanuc 31i-Model B.
The FANUCPRG.exe file is from 2011-10-12, it's Version 4.0
We have the Version 5.0, date 2014-05-15, it's a small 600Kb exe. file.
I think it's the same as shown in the video.
https://www.youtube.com/watch?v=OTw1kL5ha-A
Regards,
Heavy_Metal.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
I ordered the Fanuc memory software tool and the compact card after a brief conversation with Curt Christensen from Fanuc America - the disc can't be supplied until late March. This is apparently a new product for Fanuc. I'll update this when I get it to tell you guys who don't have it how it works. I informed my Doosan / Ellison Application people, and my sales guy who wasn't aware of it and I'm excited for March to see how it works.
Avongil- any chance you have screen capture software and can make a video? I just made a couple videos teaching some of the harder lessons I've learned in Mastercam. I feel like the only way to improve the Mastercam customer experience is to make the training videos that Mastercam refuses to make. Training is a key to too much time savings and it's just too expensive and unproductive when it's not a video product that doesn't hold back and tries to really teach people something that matters and that they can refer back to later when they forget a detail.
https://www.youtube.com/watch?v=DEvsAEQWdAU
https://www.youtube.com/watch?v=j6c6Qxfk2RM
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
XForm toolpath video: https://www.youtube.com/watch?v=g-h6c819KG0
This video explains it. Don't think I can make a better one.
For your problem, use my screen shot bellow to get the sub programs you need.
----
Mastercam has most likely the most videos out there:
free from CNC software they have tutorials. 7 high quality ones here:
https://www.mastercam.com/en-us/Supp...ials/Mastercam
here are the cnc software paid lessons - https://university.mastercam.com/
Here is a large list they maintain. https://www.mastercam.com/en-us/Supp...Learning-Tools
CNC Software forums are here: 401 - Unauthorized: Access is denied due to invalid credentials.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Holy smokes. I forgot I made the video your are looking for in 2013. Wow, where has the time gone. This is EXACTLY what you need to do. You asked for it - you go it.
https://www.youtube.com/watch?v=he0nKsA7bdY
-
4 Attachment(s)
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Hello Mr. Green0,
The FANUC Memory Card Progam Edit Tool is not a new product for Fanuc.
The Help-PDF from the Fanuc CD I attached is from the B-66484EN-06 Operators manual, the 30i-31i-32i series Model B.
I found it also in the B-64484EN-03, the same series but earlier date, see in the attachment the Version 3.0 of the PC-Tool.
The 30i-32i series started in 2004 I think, I don't know when they released the first version of this PC-Tool.
Which Fanuc control do you have ?
Why can't you download this software and pay it on-line, the complete CD contains only 3 files,
an English and Chinese Help-file, and a 600Kb exe-file, total 1.5Mb ???
You don't have to install the program, only make a folder on the HD and copy the 3 files from CD to that folder and make a link to your desktop.
The copyright in the attachments says it started in 2003.
I wonder and want to ask Mr. DouglasR, Doosan / Fanuc expert on this forum, did you ever heard of this Fanuc PC-Tool ?
Regards,
Heavy_Metal.
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Thanks a lot that was a good example (your example) I had never seen that, and I have a cam instructor account and their example sucks compared to yours. It doesn't show sub calls.
-
1 Attachment(s)
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Quote:
Originally Posted by
Heavy_Metal
Hello Mr. Green0,
The FANUC Memory Card Progam Edit Tool is not a new product for Fanuc.
The Help-PDF from the Fanuc CD I attached is from the B-66484EN-06 Operators manual, the 30i-31i-32i series Model B.
I found it also in the B-64484EN-03, the same series but earlier date, see in the attachment the Version 3.0 of the PC-Tool.
The 30i-32i series started in 2004 I think, I don't know when they released the first version of this PC-Tool.
Which Fanuc control do you have ?
Why can't you download this software and pay it on-line, the complete CD contains only 3 files,
an English and Chinese Help-file, and a 600Kb exe-file, total 1.5Mb ???
You don't have to install the program, only make a folder on the HD and copy the 3 files from CD to that folder and make a link to your desktop.
The copyright in the attachments says it started in 2003.
I wonder and want to ask Mr. DouglasR, Doosan / Fanuc expert on this forum, did you ever heard of this Fanuc PC-Tool ?
Regards,
Heavy_Metal.
I only thought it was new because nobody seems to know about it and because Fanuc is out of stock on it. Doug probably is becoming aware of it in this thread. For $23 they should include it in the Ellison field training PDF and push it at every customer of the DNM5700. It is no different than a feature like flood coolant- it's great to have and doesn't cost much. (granted that's if it runs like control memory like Fanuc says it should).
My ellison Sales guy had never heard of it. An Okuma application guy who now sells Fanuc never heard of it. Other programmers online never heard of it.
I've been told one minor revision will allow the program to output complete when edited. Picture attached.
Attachment 412912
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Quote:
Originally Posted by
Green0
I only thought it was new because nobody seems to know about it and because Fanuc is out of stock on it. Doug probably is becoming aware of it in this thread. For $23 they should include it in the Ellison field training PDF and push it at every customer of the DNM5700. It is no different than a feature like flood coolant- it's great to have and doesn't cost much. (granted that's if it runs like control memory like Fanuc says it should).
My ellison Sales guy had never heard of it. An Okuma application guy who now sells Fanuc never heard of it. Other programmers online never heard of it.
I've been told one minor revision will allow the program to output complete when edited. Picture attached.
Attachment 412912
Just to be clear - the attached pic is for outputting the complete program including subs from memory.
I really do not know if this will work with this new magical Fanuc software though.
But please keep me informed on FB, as I don't get here anymore!
-
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Quote:
Originally Posted by
Green0
Thanks a lot that was a good example (your example) I had never seen that, and I have a cam instructor account and their example sucks compared to yours. It doesn't show sub calls.
Let me know how it works out for you. It should post perfectly, if it does not then there are issues with your post but that is not likely these days.
-
1 Attachment(s)
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Hello guys,
I did an earlier reply on this Fanuc Tool on the Fanuc-forum, but no respons by the Fanuc experts.
Also on this Doosan-forum, 10-2018, I did a reply on this issue, again no repons by the experts.
https://www.cnczone.com/forums/daewo...oftware-2.html
If they read these forums they know that this Tool is available and than they have to do some research on this item.
If you do lots of 3D milling with large programs then you buy a 2Gb/4Gb DATA server, I heard some prices about $5000 or $6000.
Extra internal memory is also expensive, 2Mb max. for the 0i-series, 8Mb for the 30i-35i-series.
For all the other Fanuc 0i / 30i-32i users this €20,- ( $23,- ) program could be a solution, thats what it costs at Fanuc Benelux / Europe.
I wonder what it costs in the USA or the UK, the €20,- was the price we paid in March 2018, ordered at Fanuc Benelux, €15,- "shipping-costs",
but we had 2 products and the invoice says for both products, "country of origin", - JAPAN, so thats the €15,- shipping costs.
Every Fanuc "expert" who sells Fanuc products has to look into the Fanuc Function Catalogue, it a PDF with all the Fanuc funtions and software.
Regards,
Heavy Metal.
The attachment is from the Fanuc Function Catalogue 2018.
-
3 Attachment(s)
Re: I never understood what Fanuc people meant by Fansuck until this 5700.
Hello guys,
This is for all FANUC-0i / 30i - users with max 512kb memory, I don't know if it works on the 0i-MC series.
I made a FANUCPRG.BIN file that you can try if you want, it's METRIC.
It's a Cimco-Edit 800kb sample-NC-file that's also stored in the zip-file, original file-name LEFTOVER.NC, 1Mb.
I removed the line-numbers, minimal Z-value is 0, but for safe run put a value of 100. or 200. in the Z - EXT (WORK) table.
Copy the FANUCPRG.BIN file on your flash-card, use soft-key [MEM CARD], not the [MEMORY-CARD], that key show all files on the card,
the key [MEM CARD] show only O1500, that's the program you need.
Look also on post #30 for a video on this item.
If it works you can run a 800kb file on a 512kb memory, now you can run larger programs.
Good luck.
Regards,
Heavy_Metal.