Advice on toolpath for machines with small memory

[ashes.man]

Hi,

My old Mazak while physically capable, has very limited memory.  It seems that increasing the memory was an optional feature but how to do it has been lost in history!  It has about 48kB of usable program memory.  

I am after advice on how to work with a machine such as this with Fusion 360.  Almost every toolpath it generates exceeds this memory limit.  I can break my job into lots of files and upload them one by one.  Or even beak operations up into smaller operations and upload each file.   But, maybe there is a better way?

An example part I wish to make is attached.  Any advice on how you would break machining of this part into operations my machine could handle would be greatly appreciated.

[engineguy]

@ashes.man 

Couple of questions, one what is the control Mazatrol/Fanuc etc, two does it have "Drip feed " capability.

Lot of years ago I had a similar situation with an old Bridgepor that Had a Fanuc 0M control that had about the same usable memory as you have, when I started with a CAD-CAM software exactly the same issue so I looked into doing "Drip feed" for the code, took a few attempts to get the cable connections right but when it was setup , we are talking I could run a million lines of code or more if I wanted, the machine wasn`t very quick but if I was prepared to wait a few days (Or more) I could do some pretty fancy stuff, we are talking 30 years ago here, old 1989 machine 🙂 🙂 🙂

If it has the capability then worth buying a cheap PC or one of the "emulators" that just sit by the machine and have a lot of memory and you can just put the code on a memory stick and load to the unit and it will feed the code to the control as required, a few ways to do it some not too expensive. The "Shoplink"  one has been around for quite a while and you can pick one up online pretty easily, image below and link to one on **** 🙂 🙂 🙂

https://www.ebay.co.uk/itm/Haas-USB-FLASH-memory-upgrade-for-Haas-CNC-Send-Receive-DNC-Drip-feed-via...

This link is for one that is for a HAAS just as an example, but they do others, there are a number of other makes out there as well 🙂

An old cheap PC with a Serial Port will do fine as well, you can buy some DNC software, EasyDNC is a good one, not the cheapest but very good and reliable  https://www.easydnc.com/ to make the connection or as I did back then just used the built in MS "Hyper Terminal" in Win98 and XP 🙂

You can also run "Subroutines" to say do multiple depths of cut that are not too big and are just repeated by the Subroutines but that will depend on the Post Processor you would be using, might need modifying 🙂 🙂

Hope that`s helpful, the choice is yours 🙂

Stay Safe

Regards

Rob

Stay Safe

Regards

Rob

[ashes.man]

@engineguy Thanks for your reply.  This Mazak is from 1997.   It has a EIA Dash (otherwise called a MAC-TP).  It is a reasonably advanced control for its day.

I cannot find any way to drip feed to it.  I spent a fortune to get all the manuals and there is no mention of drip feeding.  Subroutines are definitely a good option but just means doing manual programming.  I write code for a living so it shouldn't be a big deal but would obviously be nice to just be able to output from CAM so you can tweak things easily.  Most things I do are one off.  The controller has full macro programming but it is 'disabled' along with the additional program memory.  I wish I could find someone who knew about how to enable it!

I had considered making a tool that effectively types the programs into the MDI (by interfacing to the keypad buttons) but I think it would be unbearably slow.  It is kind of breaking my heart.  It is mechanically such a good little machine but this lack of memory really takes it down a notch!

[mattdlr89]

Hi @ashes.man 

We have a machine of a similar age that we can drip feed too as @engineguy mentions. It can also be referred to as "tape" mode. Can you see any setting for that on your machine?

We used a Windows XP laptop with USB to serial dongle adapter and a serial cable to feed into the machine. At the time we were using OneCNC CAM package and they offered OneCNC NC Link as a free download for drip feeding into machines. 

[johnswetz1982]

In your manuals does it mention RS232 anywhere?

[ashes.man]

@mattdlr89 @johnswetz1982 The machine has a RS-232 port that I use to send programs to and from it.  You can also send things like all the parameters over the serial port.  It can also be used for a printer or disc drive.   The "Program File" screen has options like NC->TAPE, TAPE->NC, COMPARE etc.  But nothing that I have found can be used to send programs to it on the fly.  I cant get to the machine or manuals right now to take a picture of the screens.

[mattdlr89]

I think Tape to NC might be what you're looking for. We didn't have a Mazak so I can't be sure. We were able to send files both ways on the tape setting. I am guessing here that Tape to NC feeds data into the machine, and NC to Tape feeds back to the computer.

We were able to load multiple programs into the memory from tape and back to the computer (i.e. if you've edited them) and also drip feed through the tape setting for larger files. We pretty much exclusively drip fed all data to that machine as none of our programs could fit on the memory. 

[ashes.man]

With the TAPE->NC button you have to first enter a program number, then hit start and then quickly hit send on the PC.  It then sends the program to the controller and it appears in the list of the programs in the number you entered.  I cant see a way to make it do anything else.  It would be great if I could find a way to do it as I already have an old laptop with a serial port sitting beside it to run my little router.

[engineguy]

@ashes.man 

If the Serial port is working OK then the procedure I used on all the machines I ever "drip fed" was to have the nc file selected in the transmit/recieve window on the PC of the DNC software and then hit send, nothing actually happened until I hit the Cycle Start on the machine control, the control then just ran the code so as has been already posted get the right configuration and it should just run.

The "handshake" (Baud rate, Xon/Xoff etc) may need to be manually set but most DNC softwares can do a check of the machine to get that data automatically but it should be somewhere in your Manuals ?? Used to dread going through those old Yellow Fanuc Manuals, talk about time consuming 😞 😞

Stay Safe

Regards

Rob

[mattdlr89]

That's how ours worked as well. The machine had a rotary switch to select the input -  MEM, MDI, Rapids etc and one option was tape. You selected tape, sent the file from the laptop and then nothing would happen until you press cycle start. 

[Laurens-3DTechDraw]

We have an old Fanuc control in the shop.

And that has a tiny memory too. That is mainly used for production though so has more parts per pallet.

There is a Fanuc Compact post which might help you a bit. For us the generic Fanuc is better options though. Such as useSubroutines & useSubroutinePatterns. Even with the option to push these to separate files. That way we only have to output a pocket once even if it is used 20 times in the program.

For doing one part at a time where there is no repetition of anything that's a little harder. Advice would be to stick to 2D operations as much as you can, use the smoothing option to get as little points for the given toolpath. Sometimes it can be beneficial to actually use a lower value for the general tolerance, and higher for the smoothing so you get nicer curves in the path which make it easier to smooth afterwards. For that machine my generic setting is 0.025mm tolerance and 0.05mm smoothing for 2D roughing operations. There is a thread here where the tolerances have been tested for the best results: https://forums.autodesk.com/t5/fusion-360-manufacture/understanding-smoothing/m-p/6636266/highlight/...
The wording there with tolerance greater than smoothing tolerance feels weird to me. As I would it describe it the other way around, but the numbers should make clear what is actually going on.

[ashes.man]

Thanks to everyone for your advice.  I went through the machine menus again tonight and also the manual.  There is no mention of anything but loading files from tape into memory.

I will try some experiments soon to see what happens if I try send on RS232 while in MDI mode.   The machine has only MPG, rapid, feed, auto and MDI modes.  The auto mode requires a program number to be set of a program already in memory otherwise an error occurs.

Pictures of the screen and manual pages are attached for anyone interested.

[ashes.man]

And the other manual pages attached....

[daxpatel45]

if you don't have space in Controller use Live Command Sending software from Pc Like GCode sender or Mach 3 . This Software Uses a USB cable to send DATA like GRBL Controller. You need to modify your controller.

[mcd540]

My first machine, which I still have, was a 1995 or so Mazak with a Mazatrol EIA/Yasnac control. Mine had a small amount of memory like yours, so I upgraded the memory to 1 meg.

Try here for a memory upgrade, I think it's where I got mine many years ago: https://www.memex.ca/products/dnc-memory-upgrades/memory-upgrade/

I'm relatively certain you can drip feed your machine, and sometimes that's the only practical option. But having a decent amount of onboard memory makes life much easier.

[ashes.man]

Thanks @mcd540, for the suggestion.  Unfortunately, I contacted MemexOEE and their reply was "Sorry, we cannot help".  I wish drip feeding was an option, but it seems this controller just does not support it.

I have extracted the firmware from the machine and started reverse engineering it to see if I can work something out!

[mcd540]

What control does your machine have?

[ashes.man]

@mcd540 This machine has a Mazak IMAC-TP controller, sometimes referred to as EIA Dash.  I finally got a response back today from Mazak about a memory upgrade.  They said "It is too hard and I should reconsider".  It sounds like there is an expansion memory PCB that has to be installed along with brackets, bus cables and power supplies.

I am going to start looking harder at retrofit options again, at least then I will be able to get around some of the other issues it has too!

[Laurens-3DTechDraw]

Bummer that machine would need some serious investment to be productive.

Retrofit usually isn't all that cheap either. But going the Siemens 808 way could be a solution. Those kits usually are relatively cheap.

See this: https://www.machinetoolproducts.com/3-axes-hardware-only-siemens-808d-cnc-kit-for-milling-with-sieme...

I would go for the 10nm drives/motors though. So still 13k. They also do pre build cabinets. So you only have to switch motors and cabling. As long as your spindle motor is Analog I believe you can hook that up as well.

[engineguy]

@ashes.man 

If you are seriously looking at retro-fitting a modern control system then have a look here :-

https://en.cs-lab.eu/

I have two machines (Mill and Lathe) currently using these controllers, they are industrial quality and if your Motors and Drives are good then this is the place to go, depends on the type of Motor Drives that are on the machine, both Step/Direction or Analog (0~10Volt) controls are available, they also do their own front end control software simCNC that works great, or you could use the Mach4 software but I prefer their own, if you don`t need to fit new motors and drives then these controls are an excellent way to go 🙂

Here is a short video of an old Chiron that was retro-fiited with the Analog control system doing Rigid Tapping, encoders go back to the control as well for accuracy, not closed loop just to the drives 🙂

https://en.cs-lab.eu/technical-support/tutorials/rigid-tapping/

The above is just for your information as something to take up yet more of your valuable time, Ouch 🙂 🙂 🙂

Keep smiling 🙂

Stay Safe

Regards

Rob