Haas Heaven or Hell

[Programinator]

Started a new job and they have Haas machines. 6 of them. I worked on haas machines at my last job and i thought they were ok but they were not old. But now at this new job They have 3 older machines. one was manufactured in 1998 one in 1999 and the last in 2000. The 3 newer ones seem to run fine vf2ss, vf3ss, minimill. I am having problems with the older ones though. the thing i am seeing is the holes that i interpolate come out .008-.010 small and every linear move with the same endmill cuts to size so that im forced to put a differant D value in for when it cuts holes.

 

Is this typical for older haas machines? Is there any way to improve the situation.

 

I know lots of you hate haas but i am stuck with them and would appreciate some help.

[john316]

.

 

You could try adjusting the backlash but I don't think you'll get them tight enough for for close tolerance holes. They'll work for looser tolerances, though.

 

.

[The_Evil_Machinist]

adjust for the backlash in the ballscrews.

[SydwazShawn]

We have one of the first generation Haas's 1993(AKA Luner Lander)! It still has no problem doing holes like you speak of. Maybe the ball screws are shot in that particular machine.

The bad thing about the old Haas machines, is they really cant read ahead and process code very fast. They get real jurkey if you push them.

[Greg Williams]

Hell

[kool]

Haas has a custom couterbore cycle G13, which is good for tight tolerance holes.

My old shop had there post modifed to out put G13 for circular move

[SydwazShawn]

Not sure if it makes a differance, but on setting #85 what is it set @? ours is .002

[Columbo™]

+1 HELL......ask Pinky

 

[Leigh @ Kodiak]

Check the bearings at the end of your ball screws. They were loose on our older one when we were having problems like what you describe. Be careful tho, it is possible to over tighten them.

[[email protected]]

If your using vises move one as far as you can in X and Y and try it again. The ballscrews might be worn in one spot. At least by doing that you can tell if it is the ballscrews.

[MotorCityMinion]

5 V series here, 1 mini mill. 3 to 7 years old. Other than a few leaks and toasted boards,they seem fine. Mini mill is kind of a joke though. Hold .001 on size all day with mild steels, don't know about roundness though. FYI, MPMaster works great with the Haas.

[Cad-Camr]

The older Haas Verticals dont seem to perform well at high feed rates. Antything over abot 60 ipm accuracy and finish go south.

[chris m]

Is the hole round? If so, it ain't backlash. Cad-Camr is right, look-ahead at higher feedrates [and by "high" I mean 40IPM] could cause you some issues; you might want to try Exact Stop [G65, typically] and see if your holes are magically larger.

[SydwazShawn]

I would say on a machine like that, we would use a G13 @ F15. s7500. Thats for a 38 e.m. If its a small hole you need to go slower on the feed.

[Tony35]

are you making a big enough interpolation?

the haas i use to run could not handle small circles fast

[3R!< W3NG3R]

Instead of using a different D value for the tool, use the stock to leave function. You can put a + or a - in there too. Just remember it is a radius value.

 

Can't help with the machine.

[Programinator]

"Instead of using a different D value for the tool, use the stock to leave function. You can put a + or a - in there too. Just remember it is a radius value."

 

ya then if you run it on another machine that cuts good the next time your holes will be oversize

 

the holes seem to be round So what it sounds like is I have to feed slower or use d values

[Alvaro Gil - Cimquest-inc.com]

Also try using IJK instead of R values in G2/3... Dont know if its an issue on haas machine, but a fanuc set up with loose tolerances will cut totally out of round with R values.

[Programinator]

Ijk does make a diff on haas and that's what I have been using. Can't wait till I become fimiliar with the machines and I can post out good code the first time as far as the speeds and feeds that these old haas machines can handle.

[john316]

.

 

+1 on the slower feedrate.

 

If the holes are round you're doing good. If the hole is small use a slow feedrate. I'm talking about something like a 1/2" e.m. cutting a 3/4 to 1" dia. hole. On low cost machines like a Haas or Fadal they can't get in position fast enough to make an accurate hole. I used to run Fadals and had that problem. I would slow the feed down to about 5 ipm and not have a problem anymore. When you're cutting a small hole the extra time is no more than a couple of seconds.

 

.

[Programinator]

It's only a problem with the older ones. I love the two ss machines we have. Very accurate and fast enough for me

[SydwazShawn]

quote:

---

It's only a problem with the older ones. I love the two ss machines we have. Very INaccurate and fast enough for me

---

Fissed!

[Programinator]

[Alvaro Gil - Cimquest-inc.com]

Also, High Feed/High speed helps with these older machines. Figure out what acceleration values work, and then run though high feed. This will really smooth out the motion for older machines so they dont bang to stops and so they slow down on sharp moves and small radius's.

[Salt4cad]

Sperial mill works great you can use higher feeds Uses less cutting preasure a rough and a fininsh pass holding .0005 on dia. on a 97 vf3