[stevieboy]

I'm using mastercam v9 and I want to run quite a large program on an old hurco vmc. The machine has a program size limit of around 7000 lines. The program I want to run is just over 46000 lines so it doesn't fit in the machine memory. I have a network cable for this mill from the guys that I bought it off but I've never used it, now I need to. Any help on what I need to do. I've never attempted to do this before so any advice would be very welcome.

Thanks.

[ObrienDave]

Check out this thread, it should answer some of your questions.
If you have any more, please don't be afraid to ask.

http://www.cnczone.com/forums/showthread.php?t=80555

[stevieboy]

Great, got it sorted out and can now transfer a file from the PC to the machine. I can also drip feed the program either from the PC or from the machine's hard drive if I upload the file to that first. However I now have a new problem to fix.

The part I want to cut is a special multiple cam profile and is drawn as a series of ellipses. The toolpath is made up of lots of tiny straight lines, hence the size of the program. What happens now is the machine feeds very slowly as it can't process the information fast enough. I've tried everything I can think of but nothing changes it.

In Mastercam I have the feedrate set as 1000 mm/min for the tool but the machine drops to around 250 mm/min. I'd like to try setting it up as feed per tooth to see if it runs faster. I don't have any specific tool library as I've never got that far with Mastercam. Most of my jobs are one offs and small batches so I just "creat new tool" and fill in all the information in the boxes. I guess I've got to knowing where i am with feeding by mm/min.

How can I set Mastercam up or the tool info itself so I can creat a program that runs feed per tooth.

[ObrienDave]

This has always been a problem with older/slower machine controls and point-to-point programming.
It usually has everything to do with how fast the controller can process the data.
I'm not really sure if programming feed per tooth will make a difference.
There are a couple of things you can try.

1. Try turning the baud rate up as fast as you can until you get data transmission errors.
Then turn the baud rate down until you don't get any more errors.
This has no effect if you are able to fit the entire program on the controller hard drive.

2. In the operations manager, right-click on the operation name and you will see under Options a command for Filter.
This trys to reduce the number of moves by fitting arcs to the point-to-point data at the sacrafice of curve accuracy.
Most older controllers can process arcs much faster than a whole bunch of small linear moves.
If you and your customer can live with the reduced accuracy, this is probably your best bet on increasing feedrate speed.

Lastly, If these steps don't help, you will have to go back to your original toolpath and regenerate it at a reduced tolerance in order to reduce the number of moves.

A combination of reducing the original tolerance and filtering should give you optimal results.
You will have to experiment to see what works the best for you and your customer.

[Superman]

Yeh, The older machines suck trying to process point to point programs

You will find that the machine will do the same for a program running from the control's memory as for one running by drip feeding, this will high-light that the problem is the processing speed of the control. Baud rate will have no effect.

The only solutions are :-
1. open the tolerance to allow for longer line segments of tool motion
2. enable the filter to fit arcs in place of point to point output
( enabling depends on Mcam version )
3. modify your geometry in mastercam to be a series of arcs instead of splines

Generating toolpaths around 2D splines most times outputs point to point code, option 3 would be your best solution

[stevieboy]

Ok, it looks like I'll have to do the job with it like it is. This is a one time very small batch job, I doubt it will be repeated. The customer's drawn up the part and sent it to me as a DXF file. I can't spend any more time on it now so it's chip time (very slowly). At least I've learnt a few things and I've now got the machine networked to the PC. Thanks a lot to all who have helped, it's very much appreciated. Cheers guys.

[foxsquirrel]

I am not trying to slam you for running an older machine but, we bought a new Haas VMC last summer and I will not go back to using any older control!!! Some of our programs have 30+ hour cycle times and it pulls the program from the USB memory stick. Post it in Mcam and save it to the USB memory stick and its done and no head aches.

[ObrienDave]

Unfortunately, there are still a lot of older/slower controls out there.
Like stevieboy's case, it's important to know how deal with the limitations of the equipment you are working with.