I have got a vfoe20 and am wondering if there is look ahead on this machine and where i can find itout what it is.

Thanks

look through the settings or look in the documentation that came with the machine.it has to be purchased for it to be there.

my vintage haas has an m code. cannot remember it off hand. but it turns off graphics while running to utilize processing for code.

doug

Depending on the machine age they had an unlock code for all the control options (100 hours or something like that) which you could turn on and off. (I used it on a 2002 VF-1). Turn it on and your surface machining will be so much nicer!

Hmmm. I'm NOT impressed with the high speed function on our Haas VM2 and VM3. Our Fanuc 18i-MB controlled Yama-Seiki is MUCH better than that Haas.

What year is the machine?

Its a 2000 VFOE 20HP It is supposed to have it but i do not know what to look for I have not found any codes that turn on or off

It is an option you must buy from HAAS. Give your HAAS dealer $2095 and they will give you a new serial no that will unlock it/allow you change the parameter to unlocked.

We have a 2000 VFOE also, this is from the HAAS manual:

High Speed Machining

High speed machining makes it possible for an increase in the removal rate of material, improve surface finish,

and reduce cutting forces which will reduce machining costs and extend the life of the tools.

High Speed Machining is most often required for the machining of smoothly sculpted shapes as is typical of

mold making. The Haas High Speed Machining option increases the amount of lookahead to 80 blocks and

allows full speed (500 inches per minute) blending of feed strokes.

It is important to understand that high speed machining works best with smoothly blended shapes where the

feed rate can remain high through the blend of one stroke to the next. If there are sharp corners, the control will

always need to slow down or corner rounding will occur.

The affect that blending of strokes can have on feed rate is always to slow down motion. The programmed feed

rate (F) is thus a maximum and the control will sometimes go slower than that in order to achieve the required

accuracy.

Too short of a stroke length can result in too many data points. Check how the CAD/CAM system generates

data points to insure that it does not exceed 1000 blocks per second.

Too few data points can result in either “facetting” or blending angles which are so great that the control must

slow down the feed rate. Facetting is where the desired smooth path is actually made up of short, flat, strokes

that are not close enough to the desired smoothness of the path.

do you know what the prameter code is?

on our Haas Vf2

Parameter 315 Common Switch 4

it has one called HIGH SPEED....

Not positive if thats the one your lookin for.

Thanx for the info, after looking up that switch and it being on (1) i am assuming this machine has the highspeed function. Could it be that my post is not posting that m code i am using a post modified by my reseller for this haas. Does anybody know what the m code would be and i could search the post the manual does not specify an m code for this at least not under "highspeed" or "lookahead"

thanx to all for the help and information

I could be wrong, but it my beleif that Haas' 200hr trial High-Speed option operates at about 80% of the acual paid version. For $2095, you get a new board with a better processor.

On my machine, the default "accuracy" is controlled by Parameter 191, but can be changed using G187P1(rough) P2(med)P3(fine).

Setting 85 is the default corner rounding parameter. It also can be changed using G187E0250(.025 max corner blend) G187E0050 (.005 max corner blend)

There is no M code to activate highspeed look ahead.

There are 2 codes however that can affect highspeed performance.

1 G187 = this is accuracy for highspeed look ahead. uses a E value in the same line for for max deviation from toolpath (or desired accuracy) to control accel/decel in cornering.

2. G103 = look ahead buffering. uses a P value to limit the amount of block control will read ahead. IE; G103 P10 will only look ahead 10 blocks, G103 P0 will look ahead max number it can.

got post tweeked and now those g values show up in program.will see how it cuts.

thanx to all for the help

got post tweeked and now those g values show up in program.will see how it cuts.

thanx to all for the help

got post tweeked and now those g values show up in program.will see how it cuts.

thanx to all for the help

I'm interested in knowing what you did on the post and what the code generated is. From my experience you have to mess with the E and the P quite a bit depending on the part shape and how much stock you leave if you really want to maximize G187...So I normally input with a "manual input" or by hand.

I have my MISC INT set-up for this. One thing I have to do is to turn it off or revert to medium after each use.

Once you trun that ontion on, its always ON.

Mic6 has the correct settings for the post. I run mine at 2 until I need a tight tolerance and finish. It will slow down going around corners or into corners.

Now I dont remenber for your year machine if the G187 is present. 2000 or so was the year they added the high speed machining. I does work great on your machine if its turned on. I ran one with it on. Its over 100 block look ahead as long as the memory isn't data starved. IE rs-232 feed.

CAll Haas, they can tell you what worked on that year machine.

Machine guy.

Sorry for stuped question.I am just don't understand about parameter 315.For working with HSM it must be 1 or -1?

Thanks.

 1pregunta si en mi programa pongo "g187 e.02" en teoria se activara

quisiera saber si  al final del programa quedara siempre activado con esos valores ?

o con el m30 se desactivara?

 1pregunta si en mi programa pongo "g187 e.02" en teoria se activara

quisiera saber si  al final del programa quedara siempre activado con esos valores ?

o con el m30 se desactivara?

 

One question if I put my program "G187 E.02" in theory it is activated I wonder if the end of the program remain always on with those values? or the m30 is deactivated?

It stays active until the e-stop is pressed.

I don't know where you get the "e" value. Its G187 P 1, 2, or 3 for accuracy control.

P2 is the normal active one in the settings.

e is spanish for P

G187 controls both smoothness and rounding. P is smoothness and E is rounding. so it looks like this G187 P(1,2 or 3) E(.0001 to .200). at the end of the tool path you put in G187 and it clears any overrides you put in at begining