Any freebie ways to speed up look ahead?

[conceptmachinin]

I have a Haas V-F3 2001 model and was wondering if there is any programming method to speed up look ahead? I do a lot of prototype 3D milling, but still don't make enough to justify getting the high speed machining option. That said, I am wondering if anyone out there has any info on speeding up look ahead on a VF-3?

Thanks for any help

Jimmy

[gar]

071112-0655 EST USA

conceptmachinin:

How do you know that lookahead is your problem?

Is your program in HAAS memory or are you drip feeding?
Do you have line numbers?
Are you using any instructions besides G01 for motion?

.

[Donkey Hotey]

Originally Posted by gar Do you have line numbers?

You've got my attention now. Do line numbers slow it down?

[jetpig1]

I thought High speed machining only effected the deceleration in corners and absolute machining, or slight dwell times.... somebody call ol' Gene...

[ckirchen]

Anything that is not required should be left out of G-code. I never use line numbers, because the processor still has to look at them to see that it's only a line number and then decide to ingnore it. The Haas manual also recommends turning off the program display (M76 to turn it off, M77 to turn it on) because it takes processing power to update the program as it flies by on the screen

I like drip feed over uploading the program to memory for two reasons. 1. I only have 1MB installed, and it's common for the G-code to well over 1MB, so it just won't fit. 2. You can start cutting as soon as the drip feed is started, whereas, if you are uploading, you have to wait for the entire program to enter memory before you can start. Obviously, the drip feed connection has to be fast enough to prevent data starving and there is a risk that the connection could go down mid-program.

I do a lot of 3D prototyping as well (mostly proving out plastic part designs before cutting the mold), so HSM is perfect for what I do. I'll routinely finish with a 3/64" BM at 80 ipm, and the cutter tracks perfectly with HSM turned on. When HSM is turned off, the cutter will stutter and dwell at anything above 20 ipm and the surface finish suffers. Most of the prototypes that I make are fixed price, so anything I can do to get the job quicker will mean more money in my pocket. I've calculated that the option will more than pay for itself in a couple of months.

I haven't bought the option yet, but that's because I'm still using the 200 tryout hours. I don't know if your machine has will let you try them out (mine's brand new, your's is 2001), but if you can, I would suggest giving it a try. There are several other options available (rigid tapping, spindle orientation, rotation/scaling, and macros). As soon as the 200 hours run out, I'm going to purchase the license.

Here's a cut and paste from the Haas website that describes how to activate the tryout:
Q: I own a TM-1. I am the second owner, so I do not know exactly what options were installed. On the parameter page with rigid tapping and so forth, next to each item there is either a 0 or 1. But on some items, there is a 0T. What does that mean? Is it installed of not installed. It says this on the rigid tapping parameter, and on some others, as well.

A: If a parameter is set to 1, it is enabled. If it is set to 0, it is not enabled. If the parameter is 0T, this means you can enable the option for 200 hours for a free trial, but the option will be disabled after the 200 hours have expired. To enable an option for 200 hours, turn setting 7 off and push the Emergency Stop in. Then, change the parameter bit for the desired option to 1 by typing in the number 1 and pressing the Write/Enter button while the desired parameter is highlighted. The T will disappear and the 0 will change to a 1. If, after 200 hours, you decide you would like to purchase the option, you can contact your local Haas Factory Outlet for a code to permanently enable the option.

Chris Kirchen

[conceptmachinin]

Originally Posted by gar 071112-0655 EST USA conceptmachinin: How do you know that lookahead is your problem? Is your program in HAAS memory or are you drip feeding? Do you have line numbers? Are you using any instructions besides G01 for motion? .

Haas memory, no line numbers and G1 is the output code. It runs okay, but I cut a lot of plastics (so I could fly thru the stuff). Sure I am flying thru code, and I know that there are things I can do like increase step over etc, but I was hoping there is something that would speed up my 3d machining by using an easier approach. I supposed I can modify my post so that it spits out arcs, if it has the option, but a lot of the times its going to be splines/curves that I'm following regardless

Thanks Gar

Jimmy

[gar]

071112-1634 EST USA

conceptmachinin:

ckirchen has given you some good information from experience.

If you drip feed, then baud rate and unnecessary characters are important.
Arcs might reduce code but increase calculation time. You would need to test this.

The only places you might need line numbers are jump (includes subroutine calls) and restart points.

.

[Rocko1]

I have a VF3 1998, I wonder how much adding High Speed capability would cost? Currently I can cut about 75 IPM with no problems in aluminum.