Cons of drip feeding

vmipacman · Oct 5, 2017

I "discovered" drip feeding on my Fanuc OM a while ago and love it. No longer limited to memory and I can do come HSM toolpaths and such. What I found difficult was restarting a program midway. That scared me so I never really did it. Since the code for starting the spindle, coolant and ZYX position had already passed it was just not worth making a mistake to try pick up where it left off before a tool break or stopping the program to make an adjustment. I mostly just started the program over. Is there some mini computer just for dripfeeding that would do some program look back, or make it easier to dripfeed? I half consider making it a Rasberry Pi project but wanted to see if there was something already. Seems like with a little touchscreen and user interface I could expand the OM memory and add alot of functions with a little device velcro'd to the side of the OM (kinda a pain walking from the computer to control every time I want to run a program). Am I just doing this wrong to have these gripes and think they need fixing?
Paul

mkd · Oct 5, 2017

Not saying there could not be such innovations in this area (I'd actually like to see it). But the conventional wisdom is if you want Cadillac functionality it's best served through OEM with their available memory upgrades.
fanuc can be had with data server etc.

I know Haas won't DNC any macro codes but not sure about fanuc. If yes, then a "GOTO 1234" n number block callout might jump ahead in the program. There are lots of ways to screw this up, such as remaining in G00 depending on where you drop in the GOTO command after the tool change,

mjk · Oct 5, 2017

Probably not a solution your looking for.
A friend who had the same concerns and frequently ran long die programs at his home shop, had to restart after a power blip would cut out his RPC or tool breakage
What he did was to add/duplicate the spindle ,coolant and tool information at locations in the program that allowed him to restart without running the whole program
making notes of line numbers allowed him to find a safe restart point.
These weren't changes but confirmations of conditions.
There was probably some cutting of air, but not the 6-12 hours from the original start

mkd · Oct 5, 2017

I use Moxa to go from ethernet to rs232. pretty awesome.
with enough setup there *may* be a way to call programs from CNC where the moxa is already setup to pull out of a dedicated network folder. Could just be a wild guess on my part, pushing from PC works for me,

mhajicek · Oct 5, 2017

mkd said:
I know Haas won't DNC any macro codes but not sure about fanuc.

No control will run macro flow control through DNC, it's simply not possible. With DNC the code can only be sent sequentially and is not saved in memory, so flow control (GOTO etc.) is not possible. The correct answer I believe is to add dummy toolchanges or tool-checks which will retract the tool and then re-issue all the preparatory codes as if it were a toolchange. Then you can restart at any one of those of something happens.

mkd · Oct 5, 2017

mhajicek said:
No control will run macro flow control through DNC, it's simply not possible. With DNC the code can only be sent sequentially and is not saved in memory, so flow control (GOTO etc.) is not possible. The correct answer I believe is to add dummy toolchanges or tool-checks which will retract the tool and then re-issue all the preparatory codes as if it were a toolchange. Then you can restart at any one of those of something happens.

Hey get back to your VF3SS!!! :mad5:

J?K

mhajicek · Oct 5, 2017

mkd said:
Hey get back to your VF3SS!!!

J?K

She's pumping out a batch of bone plates as we speak!

vmipacman · Oct 5, 2017

But if you has a smart dnc software you could start at line 5000 and would look back through your code and say: do you want to start spindle, coolant? Do a dummy tool change if needed, and go to an xyz start location. It could send the controller those commands at the start of the drip. My dnc software doesn't even really do a good job starting from a specific code line. It's much happier starting at the beginning.
I don't care about macros (but I think it will still do a toolchange in dnc if I recall and that is a macro). I'd just put it long form in the code. Or even better the dnc software would know what code to feed the machine if you called a macro. Idk, just saying. Aren't there still a ton of people dripfeeding? Seems to me even later model Cnc still have terrible memory capacity right?

mhajicek · Oct 5, 2017

Such software is theoretically possible, but to the best of my knowledge does not exist. I don't think there's that much of a market for it to justify the development costs, since many newer machines have megabytes or more of memory and/or built in file-servers.

D Dubeau · Oct 5, 2017

I drip feed almost everything. Restarting long programs is always a bitch. What I do is find where in the program it left off, and read backwards a bit to find a safe entry point. Then go to the start of that tool, and read forward past all the modal (might not be the word for it, arc plane, feed, etc) stuff and find a safe point (i.e.) a retract. Cut out the bits in between and you usually have something that can be restarted somewhat where you left off.

It helps when you're reading through to stand with you mouth open and an index finger hanging down pretending to be the cutter, moving it along with the g code ha ha.

Sometimes there's just no easy way and I start over again.... or I'll go back into cam and reprogram it to start from where I think it left off. It's all very much situation dependent.

Im talking all in the context of long 3d contouring paths.

Vancbiker · Oct 5, 2017

dnc4u software has a restart from tool break function. It allows you to select the line you want to resume cutting at in one edit box and input the code needed to safely restart in another edit box. Then you send it to the CNC and it resumes drip feeding.

mhajicek · Oct 5, 2017

Vancbiker said:
dnc4u software has a restart from tool break function.

Cool, good to know!

vmipacman · Oct 5, 2017

Since all my experience is with older Fanuc controls (and anecdotally I've hear lots of gripes about even later model controls having tiny sized memories)at what control revision did standard memory size become not a problem. i.e. when (roughly) when did people with new machines (basic without memory upgrades) stop drip feeding? Was it 15 years ago? 5 years ago? I'm sure its a moot point now, but there's a lot of 10yr old machines running (right?).

Vancbiker · Oct 5, 2017

Many new machines are spec'd with a small memory as standard and increased memory sizes priced as options. It is a great profit area for the machine and control builders.

mhajicek · Oct 5, 2017

My two year old Haas has I believe 16MB, plus I can DNC off of a thumb drive. I was pricing out a new Citizen Swiss machine though and that only had a couple K even with the max add-ons. I think this is one area where machine builders are way behind the times; it should be trivial at this point to have gigabytes.

litlerob1 · Oct 5, 2017

OR-----just buy an Okuma, and don't worry about it---EVER, like at all.

You can use Fansuc Macro B!! You just need the variables stored in a local memory program. [GOTO] won't work forward or back in the running program, but you can use Macro for subbing variables locally.

Dripping is a bitch, but once you get used to it, meh. The problem is really when un-qualified people are operating it and need to do something other than screw around on their iPhone.

R

cmccull166 · Oct 5, 2017

vmipacman said:
I "discovered" drip feeding on my Fanuc OM a while ago and love it. No longer limited to memory and I can do come HSM toolpaths and such. What I found difficult was restarting a program midway. That scared me so I never really did it. Since the code for starting the spindle, coolant and ZYX position had already passed it was just not worth making a mistake to try pick up where it left off before a tool break or stopping the program to make an adjustment. I mostly just started the program over. Is there some mini computer just for dripfeeding that would do some program look back, or make it easier to dripfeed? I half consider making it a Rasberry Pi project but wanted to see if there was something already. Seems like with a little touchscreen and user interface I could expand the OM memory and add alot of functions with a little device velcro'd to the side of the OM (kinda a pain walking from the computer to control every time I want to run a program). Am I just doing this wrong to have these gripes and think they need fixing?
Paul

I save the program in a folder on my desktop ,if I need to restart somewhere it only takes a few minutes to figure out where it left off and edit that out
save the edit as DELETE and reload the edited program.

SeymourDumore · Oct 5, 2017

litlerob1 said:
OR-----just buy an Okuma, and don't worry about it---EVER, like at all.

R

Well, as much as I hate the NextGen control on the new Haas, lately ( as in the last 6 months or so ), I don't even bother loading programs in the local
memory anymore, rather everything gets sent to the mapped HD and is run from there.
To date nothing I've found is different from MEM, and it's a shit load easier to send and receive back from.
Local memory has the stuff I use often ( generic face, drill hole etc ), but real part programs are ran from the "User memory" instead.

Works like a charm!

litlerob1 · Oct 5, 2017

litlerob1 said:
OR-----just buy an Okuma, or a newer Haas and don't worry about it---EVER, like at all.

SeymourDumore said:
Well, as much as I hate the NextGen control on the new Haas, lately ( as in the last 6 months or so ), I don't even bother loading programs in the local
memory anymore, rather everything gets sent to the mapped HD and is run from there.
To date nothing I've found is different from MEM, and it's a shit load easier to send and receive back from.
Local memory has the stuff I use often ( generic face, drill hole etc ), but real part programs are ran from the "User memory" instead.

Works like a charm!

Sorry Seymour, fixed it for the Haas fans. I won't take the time to criticize.

G00 Proto · Oct 6, 2017

This thread gave me bad karma... I read it yesterday and thought "I never have a problem with DNC... I never need to restart". Then last night I set up a machine to run for 4 hours overnight on a 6 hour cycle time, and some fucking genius (me)left the shop at 8:00 and at the last second turned around and closed the laptop next to the machine. So the DNC ran until the buffer ran out, and then sat there, turning full RPM, coolant blowing all over the place for the next twelve hours. Great morning... at least I have the weekend to get this nightmare job finished.

So now I get to go restart a DNC program, in the middle of a eight cavity mold (which I of course saved programing time by doing 2 transform tool paths and a mirror tool path).

Cons of drip feeding

Cast Iron

Stainless

Titanium

Stainless

Diamond

Stainless

Diamond

Cast Iron

Diamond

Hot Rolled

Diamond

Diamond

Cast Iron

Diamond

Diamond

Diamond

Hot Rolled

Diamond

Diamond

Hot Rolled

Similar threads