Fanuc difficulties

[Tommy Thompson]

We have a number of fanuc controlled vmcs from various machine tool mfgers. Most are oi-mf. The machines are generally great and the controls usually perform well but our shop is struggling to load the new high speed machining tool paths or multiple programs for part arrays onto the fanuc machines. Without engineering know how, adding memory or ftping or getting a control to recognize a cf card in an adapter to a pcmia port (must be the last place on earth for such a thing) is all extremely time consuming and frustrating. The tiny memory on the average fanuc control is hard to understand. I’d like to know why they do not just put a tb of memory on these machines or make them connect easily to a computer. It seems like it takes patient dedication or an cs degree to make them work. Endless nuance about partitioning cf cards, etc.,embedding ethernets. It might be fine for a large firm or some of the wizards out there, but for the average job shop, it’s a failure. If you are an engineer who speaks fanuc and wants to earn some money please let me know. If you want to say it’s a piece of cake, save it bro. 

[Newbeeee™]

If you look here https://www.fanucamerica.com/docs/default-source/cnc-files/brochures/function-catalog.pdf

Or if it doesn't open for you - Web search "fanuc cnc functions communication software" then look at the Fanuc Brochure.

Then search the 2023 Brochure for "memory" and read 098, 099, 558, 564, 774, and these tell you the latest options available for the latest controls.

It looks like, for the F model, you have a 2MB maximum limit.

If memory serves me, the available function is a Fanuc card that stays inserted into the PCMCIA slot with Fanuc installed software, and the control reads and processes it as "internal" memory. The best thing to do, is collate a list of your machines and control numbers, and email Fanuc explaining what you want to do, and asking what exactly you need.

It seems you'll need a service visit to configure the machines to a network/DNC and at the same time they could install the extended memory and supply training for everything.

 

[Leon82]

does m198 work?

 

it works on our 0 control feeler pallet machine.

 

we use under 500 MB cards they don't like the bigger cards

 

I got this from james

 

Set the machine into "MDI" Mode.
Press the OFFSET/SETTING button.
Change/Set the “I/O Channel” to “4”
Set "Parameter Write Enable" to "1"
Press the Cancel AND Reset buttons simultaneously. This will clear the alarm you get stating parameter write is enabled.
Press the "SYSTEM" button.
Press the numbers "138" on the key pad then "NO. SRCH" on the soft keys (below the CRT). You'll need to set bit 7 to a 1 (Bit order is as follows - 7 6 5 4 3 2 1 0 - so you'll want to change the furthermost bit to the left to a 1)
Press "3404" on the key pad then "NO. SRCH" on the soft keys. Arrow over to bit 2 (3rd bit from the right) and change that to a "1"
Press "6005" on the key pad then "NO. SRCH" on the soft keys. Set Bit 0 to a 1.
Press "6030" on the key pad then "NO. SRCH" on the soft keys. Change it to "198".
Press the OFFSET/SETTING button to get back to setting and set Parameter Write Enable to a "0". Press Reset.
Now, this will allow you to run directly off your memory card.
Your main program in your machine control will just need to look like the following;
%
O100(MAIN PROGRAM)
M198P1234
M30
%
Optionally, you can add a Q to the M198 Pxxxx line (M198P1234Q101) and it will jump to that line number within the Sub Program.
Your program on the memory card MUST be named Oxxxx (the exes being a 4 digit number that MUST correspond to the actual Sub Program Number in the sub program. (ex. O1234) with NO file extension.
Your program on the memory card must be as follows (making sure the M198 P call AND the O number AND the Sub Program Number match as I've shown)
%
O1234(YOUR PROGRAM NAME HERE)
(YOUR PROGRAM AS NORMAL)
N101
M99
%
You MUST have a memory card in the slot when “M198” is called or you will get an alarm.
NOTE:
You’ll need to have the following on hand as well;
• USB Reader/Writer for your PC so you can load programs to the Compact Flash Card.
• PCMCIA to Compact Flash Card Adapter so you can load programs from the Card to the machine.
• 1MB to 1GB (MAX) Compact Flash Card. The smaller the capacity, the more likely it will be compatible with your machine.

Quote

 

 

[Kyle F]

17 hours ago, Tommy Thompson said:

The tiny memory on the average fanuc control is hard to understand. I’d like to know why they do not just put a tb of memory on these machines or make them connect easily to a computer.

I do have to say, I agree with you there. We just recently went through a little memory card debacle at our shop with the DN TT2100SYYB, spend near a half a million dollars on a machine and it has less than two megabytes haha I'm struggling to make that make sense. What kind of dual turret dual spindle lathe wouldn't be running large(ish) programs??? smh  add that to the laundry list of crucial info we had to find out "the hard way"

IIRC our matsuuras have 1gig of internal memory on the data server but I've only loaded a handful of small programs so I haven't even had to go that route yet.

[Newbeeee™]

8 hours ago, Kyle F said:

I do have to say, I agree with you there. We just recently went through a little memory card debacle at our shop with the DN TT2100SYYB, spend near a half a million dollars on a machine and it has less than two megabytes haha I'm struggling to make that make sense. What kind of dual turret dual spindle lathe wouldn't be running large(ish) programs??? smh  add that to the laundry list of crucial info we had to find out "the hard way"

IIRC our matsuuras have 1gig of internal memory on the data server but I've only loaded a handful of small programs so I haven't even had to go that route yet.

That Fanuc Options brochure - I noticed #563. You probably have it installed, but if not, might be good as an addition for you? I noticed it in reading through....there's a ton of options that I thought "that looks good"....

 

[Kyle F]

On 4/21/2024 at 1:58 AM, Newbeeee™ said:

That Fanuc Options brochure - I noticed #563. You probably have it installed, but if not, might be good as an addition for you? I noticed it in reading through....there's a ton of options that I thought "that looks good"....

 

I wouldn't be the best person to ask, but if I had to guess I would say that is not installed. I know we run 2 programs at once obviously, on S1 and S2, but I don't believe we have the ability to edit both simultaneously. I believe if the machine didn't come with it, sales never offered it to us, and we never asked about it. It was our first lathe outside of Haas so I think we just figured it would come with "the basics"

As far as I know, even things like smoothing settings don't seem to work for them on that machine, or they never got it figured out? idk not my department so I gladly don't involve myself LOL

Since purchase of the machine I think we've gone back 2 or 3 times and added features, more memory, etc.

[SuperHoneyBadger]

On 4/20/2024 at 12:47 AM, Tommy Thompson said:

We have a number of fanuc controlled vmcs from various machine tool mfgers. Most are oi-mf. The machines are generally great and the controls usually perform well but our shop is struggling to load the new high speed machining tool paths or multiple programs for part arrays onto the fanuc machines. Without engineering know how, adding memory or ftping or getting a control to recognize a cf card in an adapter to a pcmia port (must be the last place on earth for such a thing) is all extremely time consuming and frustrating. The tiny memory on the average fanuc control is hard to understand. I’d like to know why they do not just put a tb of memory on these machines or make them connect easily to a computer. It seems like it takes patient dedication or an cs degree to make them work. Endless nuance about partitioning cf cards, etc.,embedding ethernets. It might be fine for a large firm or some of the wizards out there, but for the average job shop, it’s a failure. If you are an engineer who speaks fanuc and wants to earn some money please let me know. If you want to say it’s a piece of cake, save it bro. 

Our shop has a handful of 90s FANUC controls, lack of memory is my top concern when programming for those machines. I have a few thoughts that may help you out:

-You should look into an operation repeat macro to make multiple parts. It will save you from needing to use Xform + subs to make a bunch of parts. Our posts are set so that we can specify how many times we need to run a tool at the machine, based on setup needs, with a default of 1 part. At the end of the tool's work, it checks to see if there are any more offsets to run, then increments and re-runs, or moves to the next tool. Our machines use G54-9, J01-29, so we increment the J value to repeat multiple parts. YMMV based on your control and how many offsets you have available. This method lets you program for one, and make 3 at once. Then next time make 10 at once if you need to.

-Take a look at your filtering settings, and hi-speed ruff with 0.005-0.010 as the tolerance (~1/2 stock to leave usually). Be sure to check the box that says "Output 3D arc entry motion" too. That will clean up your helical entries. Know that while dynamic HSM is fun, and fast to program, if your machines can't handle it, they can't. Often a facing, pocket, contour or 2D blend toolpath with a 10% stepover can get you into HSM feed numbers and keep your tools running on lines and arcs.

These methods will take a bit more time and effort to set up, but well worth it for memory starved machines. I have run hi-speed, or hi-speed-lite™ on our machines with 60-128K of memory.

 

Also there is a lot of discussion on "why not drop 2TB SSDs into machine tools", and it boils down to the type of flash they used on these boards. They are designed to last for decades in a shop environment, and still work around the clock. There are threads here, and on PracticalMachinist if you want to look up the specifics. I'm not absolving the MTBs of the insane pricing for memory, but supply is scarce for old parts now too.

[cncappsjames]

On 4/19/2024 at 10:47 PM, Tommy Thompson said:

We have a number of fanuc controlled vmcs from various machine tool mfgers. Most are oi-mf. The machines are generally great and the controls usually perform well but our shop is struggling to load the new high speed machining tool paths or multiple programs for part arrays onto the fanuc machines.

1)Without engineering know how, adding memory or ftping or getting a control to recognize a cf card in an adapter to a pcmia port (must be the last place on earth for such a thing) is all extremely time consuming and frustrating.

2) The tiny memory on the average fanuc control is hard to understand. I’d like to know why they do not just put a tb of memory on these machines

3) or make them connect easily to a computer.

4)It seems like it takes patient dedication or an cs degree to make them work.

5)Endless nuance about partitioning cf cards, etc.,embedding ethernets.

6)It might be fine for a large firm or some of the wizards out there, but for the average job shop, it’s a failure.

7)If you are an engineer who speaks fanuc and wants to earn some money please let me know.

8)If you want to say it’s a piece of cake, save it bro. 

Lots to unpack there so without further adieu...

1) FANUC Program Transfer Tool (available https://www.fanucamerica.com/products/cnc/cnc-software/programming-simulation-software/program-transfer-tool for under $30 USD) . I use it and reccommend it HIGHLY. CF Cards MUST be 1GB or under for 30i/31i/0i-F series controls. I keep a 128MB (yes you read that right) card for older era machines. I get mine from Amazon. I like these for 1GB's https://www.amazon.com/1GB-Compact-Flash-100X-INDUSTRIAL-Pio/dp/B000ZNWOSS/ref=sr_1_2?crid=I99RBMCIPDWH&dib=eyJ2IjoiMSJ9.vy01M8EQ4MyyBDSDjeq_NuppS6M0tWgWrlcoasmKUzHjiYMoBe4U0bq62scns-U3Z0sxEMsM4q6X_kTLHXLVeZIRbO48o0Ipi--Hbq_FKm_aXz3hHfnB-91bIoKmwAUB53WTZHmRWTDJUWArvdnEuFhSkXyZiuemWcvM7BHOfMdrt8mszRDnM4pnfYkaWH1zERpJt7BhJnTVxO8zVuM1eqnIyDCY6XJQqDZxH8O15pWTx-OlI9AUfeXcdAxgw5UvrmuowILrWHeEtGMuZOhPyXp7I7NocgDEelaG2jZaAnk.d2rRem4np6HQzDANiXqa6evpgkauOin78IjLz0UNivw&dib_tag=se&keywords=1GB+CF+Cards&qid=1713845397&refinements=p_n_feature_five_browse-bin%3A673261011&rnid=673240011&s=pc&sprefix=1gb+cf+cards%2Caps%2C126&sr=1-2

It's only frustrating if the company you bought your machine from is not knowledgable. Support matters. Especially today.

2) This is NOT a FANUC issue. This is 100% on the machine tool builder. We spec our machines with 8MB of CNC Memory and 1GB of Data Server Memory. The latest machines have SSD Drives with TB's of storage and they are FANUC so... the problem isn;t with FANUC it's with your builder improperly specing a machine. Assign blame wher it belongs.

3) See #1

4) I barely graduated high school... and by barely, I mean if it weren't for woodshop and PE I woudln;t even have had a 2.0 GPA... and I have no trouble connecting machines to networks if they are equipped with either an Embedded Ethernet port or a Data Server. Been doing it since the 90's. You need better machine tool support.

5)I've not been successful partitioning CF Cards lately. Like for the last 10 years lately. Just get a 1GB CF card or smaller with a PCMCIA adapter and it'll work. Embedded Ethernet is a simple setup. EIther use DHCP or set a static IP address, set the router and DNS IP Addresses, plug it in and it works. Just to prove a point to a customer, I went out to Home Depot, bought a Wireless Extender with an ethernet port, set it up, set the control for DHCP, set the router and DNS, restarted the adapter and I was able to ping the CNC form anywher ein the shop. Once I was connected to their network, I coudl upload and download programs at will.

6) You just need better machine tool support

7) I give away my knowledge for free. It's worth plenty, but so many gave to me freely, I'll give freely until I get burned.

8 ) I will say it's easy, because it is. I'm NOTHING special. Believe me. I'm just an average at best guy. Your machine tool dealer has a high degree of incompetence, or they are withholding support from you. Either way, I'm sorry you are going through this trouble. You should not have to suffer because of your machine tool dealer is incompetent or your machine tool builder didn't adequately option their machine.

I hope this helps.

On 4/20/2024 at 4:06 PM, Kyle F said:

...IIRC our matsuuras have 1gig of internal memory on the data server but I've only loaded a handful of small programs so I haven't even had to go that route yet.

Put ALL your pat programs on the DATA_SV. Just use CNC Memory for custom G/M-Codes, Custom MACROs, etc...

[Kyle F]

7 hours ago, cncappsjames said:

Put ALL your part programs on the DATA_SV. Just use CNC Memory for custom G/M-Codes, Custom MACROs, etc...

Will do! So far I've only ran a handful of programs so they are just on cnc memory but I'll swap everything over for my next project.

 

21 hours ago, SuperHoneyBadger said:

-You should look into an operation repeat macro to make multiple parts. It will save you from needing to use Xform + subs to make a bunch of parts. Our posts are set so that we can specify how many times we need to run a tool at the machine, based on setup needs, with a default of 1 part. At the end of the tool's work, it checks to see if there are any more offsets to run, then increments and re-runs, or moves to the next tool. Our machines use G54-9, J01-29, so we increment the J value to repeat multiple parts. YMMV based on your control and how many offsets you have available. This method lets you program for one, and make 3 at once. Then next time make 10 at once if you need to.

this sounds very intriguing. I am currently making a few DIY tombstones for the MX-330 and I've been thinking about programming.. I don't have experience on horizontals so I never really have ran more than a couple of parts at a time, so I have always used toolpath transform. 

[cncappsjames]

So on the MX (or any multi-pallet Matsuura) in the pallet manager you can assign up to 4 programs to the pallet. It can be 4 or the same programs or 4 different programs. Doesn't matter. 

When talking pallet manager with customers I always go over a number of scenarios. Aluminum and easy to machine/non tool-eating materials tool path transform with multiple parts in the same program is typically fine. More difficult materials or materials that generally wear tools out or break tools, I reccommend separate programs that way when using tool life management you don't have to kill the whole pallet to flag the tool, you can just flag the face. Then the face is flagged and will continue to the next face and pick up the backup tool. 

[Kyle F]

18 hours ago, cncappsjames said:

So on the MX (or any multi-pallet Matsuura) in the pallet manager you can assign up to 4 programs to the pallet. It can be 4 or the same programs or 4 different programs. Doesn't matter. 

When talking pallet manager with customers I always go over a number of scenarios. Aluminum and easy to machine/non tool-eating materials tool path transform with multiple parts in the same program is typically fine. More difficult materials or materials that generally wear tools out or break tools, I reccommend separate programs that way when using tool life management you don't have to kill the whole pallet to flag the tool, you can just flag the face. Then the face is flagged and will continue to the next face and pick up the backup tool. 

Ahhh yes I can definitely see that making a difference over a large quantity order. I'll keep that in mind if that becomes an issue for us overnight.

[cncappsjames]

The only real drawback to utilizing the multi-face approach is that you'll have more tool changes. So 4 tool changes over 4 parts as opposed to amortizing 1 tool change for 4 (or however many) parts. 

My personal primary preference is flexibility. There is more to "cycle time" considerations than from program start to program finish.

Like if the machine is running 24-7, NEVER idle, then yeah, you want that cycle time to be as short as possible. If your fully loaded machine runs for 2 shifts then sits idle for one shift, then really you gain nothing by shaving every millisecond off the cycle time because that time savings was killed by the idle 3rd shift. 

"There's no perfect solutions, only compromises." Thomas Sowell

[cncappsjames]

The OP @Tommy Thompson last visited this topic on Tuesday...

[BBprecise]

On 4/20/2024 at 6:21 AM, Leon82 said:

does m198 work?

 

it works on our 0 control feeler pallet machine.

 

we use under 500 MB cards they don't like the bigger cards

 

I got this from james

 

Set the machine into "MDI" Mode.
Press the OFFSET/SETTING button.
Change/Set the “I/O Channel” to “4”
Set "Parameter Write Enable" to "1"
Press the Cancel AND Reset buttons simultaneously. This will clear the alarm you get stating parameter write is enabled.
Press the "SYSTEM" button.
Press the numbers "138" on the key pad then "NO. SRCH" on the soft keys (below the CRT). You'll need to set bit 7 to a 1 (Bit order is as follows - 7 6 5 4 3 2 1 0 - so you'll want to change the furthermost bit to the left to a 1)
Press "3404" on the key pad then "NO. SRCH" on the soft keys. Arrow over to bit 2 (3rd bit from the right) and change that to a "1"
Press "6005" on the key pad then "NO. SRCH" on the soft keys. Set Bit 0 to a 1.
Press "6030" on the key pad then "NO. SRCH" on the soft keys. Change it to "198".
Press the OFFSET/SETTING button to get back to setting and set Parameter Write Enable to a "0". Press Reset.
Now, this will allow you to run directly off your memory card.
Your main program in your machine control will just need to look like the following;
%
O100(MAIN PROGRAM)
M198P1234
M30
%
Optionally, you can add a Q to the M198 Pxxxx line (M198P1234Q101) and it will jump to that line number within the Sub Program.
Your program on the memory card MUST be named Oxxxx (the exes being a 4 digit number that MUST correspond to the actual Sub Program Number in the sub program. (ex. O1234) with NO file extension.
Your program on the memory card must be as follows (making sure the M198 P call AND the O number AND the Sub Program Number match as I've shown)
%
O1234(YOUR PROGRAM NAME HERE)
(YOUR PROGRAM AS NORMAL)
N101
M99
%
You MUST have a memory card in the slot when “M198” is called or you will get an alarm.
NOTE:
You’ll need to have the following on hand as well;
• USB Reader/Writer for your PC so you can load programs to the Compact Flash Card.
• PCMCIA to Compact Flash Card Adapter so you can load programs from the Card to the machine.
• 1MB to 1GB (MAX) Compact Flash Card. The smaller the capacity, the more likely it will be compatible with your machine.

 

All of the memory cards we use are 512MB or more. Most are over 4GB and we had any problems in the 10+ years we've been using cards this big Our oldest control in an 16i control from early 2000's and no problems there. Just have to watch the formatting. We have 2 machines that have memory cards that pretty much live connected to the controls.

[BBprecise]

On 4/20/2024 at 12:47 AM, Tommy Thompson said:

We have a number of fanuc controlled vmcs from various machine tool mfgers. Most are oi-mf. The machines are generally great and the controls usually perform well but our shop is struggling to load the new high speed machining tool paths or multiple programs for part arrays onto the fanuc machines. Without engineering know how, adding memory or ftping or getting a control to recognize a cf card in an adapter to a pcmia port (must be the last place on earth for such a thing) is all extremely time consuming and frustrating. The tiny memory on the average fanuc control is hard to understand. I’d like to know why they do not just put a tb of memory on these machines or make them connect easily to a computer. It seems like it takes patient dedication or an cs degree to make them work. Endless nuance about partitioning cf cards, etc.,embedding ethernets. It might be fine for a large firm or some of the wizards out there, but for the average job shop, it’s a failure. If you are an engineer who speaks fanuc and wants to earn some money please let me know. If you want to say it’s a piece of cake, save it bro. 

If your machine is less then 20yrs old it should have a PCMCIA slot. You just need to change the comm. port on the control to use it instead of RS-232. If they don't it's easy to get the cable and slot. You can either buy a new bezel for your screen that has a spot for the card slot or you can probably make a hole in your existing bezel. Change a couple parameters and you're good to go. I have 1 horizontal mill with only 64kb of storage so any HSM toolpath has to reside on the memory card.

However, to edit any toolpath on the card requires putting it on a pc, so if you want to be able to change the feedrate or maybe tool diameter offset if there's a CDC pass on the card you can substitute the F or D value with a variable#. I.E. if you program for F40, change it so it's F#500 (assuming you have extended variables, if not you can use #100-#150) then in your main program that's in the control you just need to insert #500=40. on the line before the M198. It's great for proving out 1st time run jobs to give the operator a way to edit the prg w/o dragging me to the floor for a simple edit like that.

[Leon82]

19 hours ago, BBprecise said:

All of the memory cards we use are 512MB or more. Most are over 4GB and we had any problems in the 10+ years we've been using cards this big Our oldest control in an 16i control from early 2000's and no problems there. Just have to watch the formatting. We have 2 machines that have memory cards that pretty much live connected to the controls.

try  it with a 6 MB program. Ours would stop half way thru with a 2 GB card.