Rapid moves with Haas

[Odell]

I just watched a $175.00 end mill explode first thing today. ( Good Morning! ) I wrote a program yesterday and went over it at least 3 times and made sure everything was perfect. I looked at every detail and missed one thing. In my program I start of with surface rough parallel at a 20 deg. angle, when it shows the tool path everything looks okay. I ran verify and no problems. What I missed was one rapid move across the part below the top surface. Not hard to miss with a million lines to look through. In verify it don't show any crashing, but in reality a Haas doesn't rapid straight at an angle it moves to the nearest tangent point and then to where it belongs. ( CRASH ) If I was cutting at 0 or 90 deg this probably wouldn't happen, it hasn't yet. Does anybody know a good way to catch or prevent this? Will the program Vericut show this or prevent this ?

[gcode]

Yes.. properly set up, Vericut will catch this.

So will Predator VCNC or even Cimco Edit 5.0

 

There are other solutions..

Some machine allow you to turn off dogleg rapids.

My early 90 Haas's didn't. Maybe newer models do??

 

On the Mastrcam side, the simplest solution is to keep your retract plane high enough to avoid the crash

 

or

use the new high speed surfacing tool paths.

You can specify G01 rapid motion and define

the rapid feed rate.

Mastercam high speed surfacing with minimum

retracts are sweeet.

[Odell]

I have a 2007 Haas so I just sent them an E-mail to see if there was a way to turn this off. I didn't think that you could turn this off but I am going to find out. What use is a dogleg rapid anyway. I have used the high speed paths and do like them a lot. This was just a small program and kinda simple and I guess I wasn't thinking of any problems like this. I hate breaking end mills.

[gcode]

quote:

---

What use is a dogleg rapid anyway.

---

They don't do it on purpose, its just the result of both axis rapiding individually at max speed.

We have 5 big Ikegia HBM's here and we were able

to turn off dogleg rapids with a parameter switch.

I hav'nt run a Hass in 10 years and you couldn't

change this behavior with those machines.

I don't know about modern Haas VCM's

 

[ 02-05-2010, 09:23 AM: Message edited by: gcode ]

[mgsanchez]

As far as I know, you can't turn off dog leg rapids in a Haas. You need to make sure you have clearance or convert your G0's to G1's with max feed rate.

[Mr. Wizzard]

Another thing to check is the rapid movements in your Control Definition..... Z, then X/Y, etc...

I had the same thing happen 2 years ago. You have to be careful in the HST's. Minimum retract cuts down on time greatly, but that's where you can get the unforseen crash. Sometimes i just set it to Full Vertical Retract to be safe. It runs longer, but you can just let it go when you have a ton of other things to do.

[gcode]

quote:

---

Minimum retract cuts down on time greatly, but that's where you can get the unforseen crash.

---

Minimum retract with G01 rapids enabled is perfectly safe..

Minimum retract with G0 rapid virtually assures a crash

[Leigh @ Kodiak]

Despite what many people think, and contrary to what Haas themselves will tell you, you CAN turn off dog leg rapids. The problem is that once you change to this setup, canned drilling cycles will no longer work, and need to be programed in long hand style.

[Hardmill]

Are you using ABS retracts ??

I NEVER, NEVER, NEVER use INC anything if

I can avoid it.

Accident waiting to happen.

 

 

PEACE

[Chris Rizzo]

quote:

---

Minimum retract with G01 rapids enabled is perfectly safe..

Minimum retract with G0 rapid virtually assures a crash

---

If you keep the machine in a feed move (g01) mastercam is always controlling tool movement, thus crash free. Letting it go to g00 mastercam in not controlling that portion of the toolpath, and roll the dice.

[mgsanchez]

Leigh,

How do you turn off the dog leg rapids?

Just curious.

[Leigh @ Kodiak]

Parameter 315. Turn the "Rapid -> HS feed" from 0 to 1

[mgsanchez]

Cool, thanks.

[Slick]

Don't feel bad Odell, it's happenned to our shop on more than just Haas mills. Like Hardmill said the best bet is an absoute rapid value.

 

You can usually tell when it's going to happen, when your toolpath rapids across the your part. The way it was explained to me that helps is the machine "rapids at a 45° to the longest axis travelled. Thus like gcode explained, in a rapid move all axis motors go at it's maximum speed until they reach there location... 3-Axis rapids are the worst! I saw a Haas 5 Axis machine do this with a curve 5 axis retract... WHAMMY!

[Jmick]

Leigh is right. Although Hass has had some issues with crashes when you do that. That is why they recommend that you not change until they have a fix. We tested the cycle time of both and the times were identical.

[Leigh @ Kodiak]

They have been "looking for a fix" for 3 or 4 years now. I guess it's more important to make Tony Stewart edition machining centers.

[Colin Gilchrist]

Hey Slick,

 

We know about this first hand. Still makes me sick thinking about it.

 

How's life man? We should get together for lunch or a brew soon. Tell Nick I say Hi.

[MotorCityMinion]

I de-select the retract box period and set all my opps to default like that. In my 1st few months of surfacing, I also got burned by that on a Haas.

[Odell]

I just got a reply back from Haas and they say that rapids can't be turned off. I guess i will just have to be more on top my ABS retract moves to keep this from happening or keep things feeding when doing this.

[Leigh @ Kodiak]

Odell, see my earlier post. They CAN be turned off, but you will be sacrificing the use of drilling cycles to do so...at your own risk of course, seeing as the function is not acknowledged by Haas.

[Odell]

I think I'm going to go beg for some better verification software. I don't usually do a lot of drilling, mostly surfacing but I can't just do away with drilling cycles. Thanks for yalls help

[John Morris]

I'm not clear on what type of machine you are on here, 4 or 5 axis VF or a horizontal. Either way when working on the 4th on our VF and on the our EC horizontal I setup a safety zone in Mastercam and it does a good job of keeping the the tool out of trouble on rapids most of the time.

[gms1]

It would be really cool if mastercam could handle the independent axis feed rates for rapids. You could add another feed for rapids and mastercam could calculate clearance moves in the toolpaths!

 

I can dream can't I??

[Odell]

I MC could put a button in backplot that would display dogleg rapids would be nice. This Haas is a 07' VF4 3 axis milling center.

[gcode]

quote:

---

It would be really cool if mastercam could handle the independent axis feed rates for rapids. You could add another feed for rapids and mastercam could calculate clearance moves in the toolpaths

---

you don't have to dream... ALL of this is available in the high speed surfacing toolpaths.

Hopefully, these features will be expanded to cover all toolpaths someday.