[Jim Dawson]

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.

[avongil]

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.

[Green0]

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.

[avongil]

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.

[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.

[Green0]

.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.

[Green0]

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?

[avongil]

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.

[Heavy_Metal]

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.

[Heavy_Metal]

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.

[Green0]

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=j6c6Qxfk2RM

[avongil]

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.

[avongil]

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

[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.

[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.

[Green0]

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.

[barbter]

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.

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!

[avongil]

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.

[Heavy_Metal]

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.

[Heavy_Metal]

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.