[Rocko1]

We just bought a used VF3 with 1 meg of memory and have removed all but the warmup programs on it. We do 3d mold work and will DNC drip feed via a 12' RS232 from a laptop. We did a test run with no stock and had no problems. Just curious how fast (feed rate) we can run and still keep accuracy within .001 . I know that our Milltronics 1998 Knee Mill CNC with a hard drive can do about 50 IPM and do fine. Also does corner rounding parameter only affect the X and Y axis? Thanks in advance.

[big_mak]

Does your machine have HSM?

[GITRDUN]

I have a 94 VF-1 which we run at 80 IPM all day long. It tends to round the corners fairly bad. There is a parameter to set the amount of corner rounding allowed, but i dont know which parameter it is off hand. Im sure someone else here will chime in before long with the answer.

[JROM]

It's hard to answer your question because there are so many things that affect what feed rate you can run. I have a VF3 about the same age as your machine with the same problem (not much memory). That said, if you keep your programs small enough to fit into memory you can run as fast as you want. I fear that using rs232 will be disapointing because it's not fast enough to keep up with a complex contor running at a good speed. The control will start to starve for code and you will get a jerky stop and start effect as the control has to wait for the program to load. NOT GOOD! I would sugest you look into putting a DAT drive on the machine then you can drip feed your programs at buss speed but I don't know if a 98 machine will accept a DAT drive. Talk to the HAAS folks.
Good luck

[Rocko1]

We had a Haas Tech out last week fixing a couple of things and he did tell me that you should delete everything off your mem but the warmup programs then you can drip feed without any data starvation because the g code will fill up to the 1 meg of memory we have. I checked with corporate and they agreed with his statement. I did try it on one part at about 90 IPM and it seemed to do fine. As far as corner rounding I have mine set at .005 the last owners had it set at .050 which seems a little high to me but to each his own.
No , we do not have HSM option.

[gar]

070907-1626 EST USA

Rocko1:

Just because you make most of your memory free for buffer use does not mean you won't get starvation in DNC (drip feed).

Suppose your baud rate was 1200, then you would transfer about 120 characters per second. With short cutting segments you will almost certainly have starvation.

You should run at 115.2 kbaud, 7 data bits, even parity, and one stop bit. You must use a handshake mode.

Eliminate line numbers from you program.

.

[Rocko1]

Gar,
I agree with your basic facts and informative as always. The question is also the G Code being created via the CAM software. This can alleviate this issue by using 3d tool path controls like: Smoothed Line segments (This will create a toolpath as a smooth spline curve then segment it as a line segment, but with a more regularly spaced and fit smooth spline within a tolerance set) or Nurbs tool path creation, which creates a nurbs spline curve for posting. I am curious does the Haas control work with Nurb Spline Interpolation?

[gar]

070907-2101 EST USA

Rocko1:

I do not believe so. Our newest is a 2000 machine.

To further clarify my post of -1626.

If at HAAS you initiate DNC receive, start sending from the PC, and immeadiate run HAAS very little data will have been loaded into HAAS memory. Starting out with short strokes you will immeadiately be starved and get stuttering.

If you first get the 1 meg of memory full or at least enough to be adequately ahead of the machine, then there is no stuttering resulting from DNC starvation until you bleed the memory down.

I have one customer that drip feeds and the program run time is several hours. I believe they have high speed machining. At 115.2 kbaud if you get memory partially filled in DNC mode before starting, several minutes worth of load, then there is no stuttering from drip feeding and the drip feed loading finishes about 1/2 hour before the part finishes. I suspect their program is in the 4 to 6 megabyte range. Note: even though 115.2 is probably 3 to 6 times faster than the average rate the HAAS is using data the average rate from the PC can not be much faster because of the limited buffer size, 1 meg. This average rate is determined by the CNC cutting time, and in turn handshaking back to the PC to prevent HAAS buffer overflow.

Note: at 115.2 kbaud you can move about 600,000 bytes per minute if there is no handshake limitation. Ten minutes for 6 megabytes if memory is big enough to hold it all.

.

[chmillman]

I have about the same vintage VF0-E with HSM installed. I can machine contours up to the max feed speed of the machine (12.7K mm/m, around 500 ipm). The control will automatically slow the machine in the sharper sections.

I drip feed at 115.2K. Note there is overhead in the transmission which will always keep you below this figure, but I've calculated around 90K is max real throughput. With this you can still transmit/receive around 500 blocks/second. You are probably not going to execute much more than a hundred or so per second.

I run 25-30 meg programs over several hours no problem. The Haas pulls the data as fast as it needs it. I have never had it run out. The quality of your DNC program may also be a factor. I only have one machine, I found that SE DNC ran flawlessly, never had it fail.

Without the HSM, you will be severely limited on contouring speed (if you have system 10.xx or later). Mine started stuttering at speeds of around 1200mm/m or 50ipm, which is why I opted for the HSM later. It was like getting a new machine.

Paradox is with the HSM, the finer you program your contouring toolpaths (the less the angle between the adjoining toolpath segments), the better the control likes it, and the smoother it goes. --ch

[nervis1]

Keep it under 80 ipm if you want accuracy, maybe slower, like 60 if you REALLY want accuracy.

Roughing? Rip it up....200 ipm

IMO of course.

Dave

[gar]

070908-0709 EST USA

Rocko1:

Where in Indiana are you located. I travel to Ft Wayne from time to time.

Even if HAAS has Nurb Spline Interpolation I think you are better off doing this in your CAM program, or some custom program. If HAAS provided the capability, then the algorithm would be out of your control and not a good idea. Its use in HAAS would reduce data transfer volume, but increase computational requirements in HAAS.

.

[Rocko1]

Gar,
Southside of Indianapolis. Our CAM program GIBBS allows us to create the tool paths with the Smoothed Line Segments (as stated in previous post) also we can post in Nurbs (as stated in previous post).
I will experiment in a week or two to see how the posting affects the Feed rate. I did dry run a part with a half circular tool path and hit 90 ipm without stuttering but again I did not cut material and can not judge accuracy. It will be curious to see if the CAM program can allow smoother toolpaths (less small lines and more radius & splines) to increase feed rates without having HSM . My target feedrate for our 3d work is 90-100 ipm, this is double what our Milltronics can do.

[gar]

070908-1023 EST USA

Rocko1:

If you can find a program that will generate your path with arcs and negligble slope differences at transition points, and works in a predictable fashion, then you could reduce the data being transferred to the CNC.

Another way to reduce data transfer is:
If you have a lot of moves that are a few thousanths, then send data as incremental. For example:

G91 G01
X31 Y2
X29
X28 Y1
X27
X27
X26 Y-1

Instead of
G90 G01
X10.3831 Y8.0002
X10.3860
X10.3888 Y8.0003
X10.3915
X10.3942
X10.3968 Y8.0002

Maybe in incremental intersperse some absolutes every so often in case there are some errors.

It is very obvious that incremental will save a lot of bytes for short strokes. For long strokes in incremental the lost time to send 100000 is not important because the machine takes a long time to traverse this distance.

.