Stuttering Haas

[Rick Morrison]

I was doing a finish cut on my 2000 Haas VF2, trying to avoid polishing by making the cut very fine. But the machine was running code so fast, it was stuttering. I had to slow the feed rate was down to stop it. My tolerance was set to 0.001. I was using surface project blend. How do I reduce the code so the machine can swallow it fast enough to run without stuttering.

[Jack Mitchell]

Rick,

 

"My tolerance was set to 0.001. I was using surface project blend. How do I reduce the code so the machine can swallow it fast enough to run without stuttering."

 

It is not so much the tolerance as it is the feed rate used. Certain surfacing commands will impart thousands of small moves but the underlying factor is can your machine keep up to the code. Without the high feed machining option you probably have the same problem as I. To overcome this I tend to use one feed rate for all three input options, from there I override at the control.

 

Hope this helps.

 

Regards, Jack

[gcode]

Rick,

The Haas control has an accuracy setting (I think it is #57????).

The value set is the maximun allowable overtravel.

The machine is not stuttering because it can't read the code fast enough, it is slowing down when it needs to to maintain the value in Setting #57.

Raising Setting 57 will get rid of the stuttering, but your workpiece will be gouged.

In short you are running you Haas beyond its

physical capabilities. Haas has a High Speed option you could purchase for your machine, but from what I've read on this forum it doesn't work very well.

 

Running file though Mastercam's High Speed package would probably help.

[Mike Mattera - TFM]

Arc filtering will help (depending on the shape). Set the filter to 2:1 and the total tolerance to .0008. One Way Filtering, and create arcs in XY YZ ZX. If it was a Finish-Contour I would only use XY only. But again, not knowing the shape, you might get arcs in all planes.

 

It may also be that the gains for your axes drives need to be adjusted. There could also be a code you can use to reduce the postiion tolerance. G61 should be Exact stop mode (that may be the default). G64 is a a kind of "Flow Thru The Points" mode for faster cutting.

 

Mike Mattera

[Rekd™]

gcode, I think you're confusing the G187 Corner Rounding Control with High Speed. I've heard very good things about the High Speed option on HAAS.

[Mike Whitten CAD/CAM Contractors]

Rick,

 

You may end up having to go to a type of machining pattern that will mill in only XZ or YZ. If you do this, you can usually filter it much nicer. It should be able to fit more arcs in there.

 

Mike

[Phil Orenstein]

That's a +1/2 Rekd. For positioning accuracy and to avoid position stops in your program you can use G187 on the Haas. But to set the postioning accuracy permanently for all programs, use setting 85. G187 overrides the #85 value. A setting of 0.0 will give you absolutely accurate position but will cause a stop after every move. I set mine to .005 and it flowed nicely thru all points in surface cutting. Try settings of between .005 - .010 and check the accuracy. To change the settings in your program use G187 E.005 and put a G187 at the end of your program to return to setting 85.

 

Also setting the baud rate higher might also help if your buffer is getting starved for data while reading dense data points. Try 19,200 or 34800 if you can.

HTH

Phil

[gcode]

quote:

---

I've heard very good things about the High Speed option on HAAS.

---

I have too-- from a Haas salesman. J/K

 

I read somewhere on this forum that it was a

band-aid approach.

 

I have zero personal experience with it as I've

never run or programmed a machine that has it.

 

The bottom line is Setting 85, G187 and High Speed Option are attempts to fix physical limitations with software.

 

G85 worked pretty good for me when I ran Haas's , but I was not doing high end mold work like some of you guys.

 

Don't get me wrong, $ for $, Haas is the best machine deal on the planet, I've owned 2 of them and I'd buy another in a heartbeat. but... they are not high end mold making machines.

[htm01]

The high speed machine didn't hold up to what we wanted to do but they have a mold making machine that has a finer lead screw and can follow over 100 ipm so far.

[MACHINEMASTERG]

we have a haas with the high speed option and it does what its suppose to do other day ran a surface tool path on an older haas and it was jumpy ...then put it in the new haas and ball milled a half moon surface at 300 ipm and it cut smoth and accuratly !!!

[htm01]

it does what it's suppose to do but it blends the tool path,we cut with many balls on the same surfaces and they wouldn't match.

[Müřlıń®]

Question........setting 57 is set to off on our controls.

Setting 85 is set to .025.

 

I have slight stuttering on toolpaths that use more lines than arcs(Shallow & Project& Scallop),

 

Has anyone tried to set 57 to .0002 or .0005 and seen any diffrence?

 

We use 80 - 120 IPM feedrates, I would like to go faster....

 

 

Murlin

[nomoslogos]

The smaller your Setting 85 is, the slower the machine will run. We leave ours set at .001 in the control, and then use G187 (a post misc setting in Mastercam) to set it at .0001 when we are finishing mold surfaces. With the HSM option we max out at 90-95 IPM with it set this tight, but we get excellent finishes when surfacing with a ball nose.

 

With it set at .001 we can run up around 150 (when roughing or semi-finishing).

[gcode]

Murlin,

Setting 57 is Exact Stop, it should be off for

almost everything. I mentioned #57 in error as

its been 3 years since I ran a Haas. #85 is the correct setting.

nomoslogos@yahoo just gave a pretty good answer on this question.

My apologies for the bad info.

[Müřlıń®]

Thanks nomo.....

 

Hey np Gcode......I have only a few months using these controls.

 

I am not trying to get a mold quality finish as I am machining forging dies and a couple thousandths here or there wont matter much.

 

I am using corner rounding coupled with the high-feed option in Mastercam and getting good results.

 

Trying to keep the operators from overriding the whole program to increase cycletimes is a daunting task.

 

If the machine stutters a little they tend to overcompensate by overriding the feed way down.

 

So nomo.....you are saying that .025 is too much and if I have the operators set #85 to .001 that it wont stutter as bad on toolpaths with lots of lines?

 

I dont know where the .025 came from, probably a default.....

 

 

Murlin

[Midwest]

#85 is set at .005 here, never messed with it.

 

__________________________________________________

 

The smaller your Setting 85 is, the slower the machine will run. We leave ours set at .001 in the control, and then use G187 (a post misc setting in Mastercam) to set it at .0001 when we are finishing mold surfaces. With the HSM option we max out at 90-95 IPM with it set this tight, but we get excellent finishes when surfacing with a ball nose.

 

With it set at .001 we can run up around 150 (when roughing or semi-finishing).

 

________________________________________________

 

I'll have to play with setting, thanks nomoslogos

 

[gcode]

quote:

---

Trying to keep the operators from overriding the whole program to increase cycletimes is a daunting task

---

Check your control manual. You can lock out the

feed and speed override buttons and wheels on the control.

 

I used to work at a place where the night shift

would screw the pooch for half the shift, then

run everything at 200% trying to make the production numbers

Its kind of hard to program for a place like that

[nomoslogos]

Merlin,

 

I have never run one set that high. That is VERY high. I don't know what kind of results it may give, but I am surprised you are getting a decent finish, unless your parts have little curvature.

 

I think .005 is the factory default. This is only too much if you are getting gouges, but at this setting it will overshoot actual coordinates on abrupt changes in direction. I became aware of this setting when I was running up to a wall with a cutter and then going away in the opposite direction. It was gouging the wall, and it wasn't in the program. The setting of .005 was not forcing the machine to actually stop when it reached the given coordinate. I set it to .0005 and it stopped gouging.

 

Also I have a fax of a technical paper from Haas that says:

 

quote:

---

When operating at feed rates above 150 IPMm there is a parameter which will cause a pause at the end of each stroke. If you have a large number o very short strokes, this may be a problem. THe pause is to insure that the tool is wihtin a preset distance of the desired endpoint and is used to guarantee square corners. This default parameter value corresponds to 0.118 inches. If you operate faster that 100 inches per minute and do not need better accuracy or the strokes are well-blended (no sharp corners), this parameter (101..104) can be changed.

---

There is more, but I don't have time to type it in.

[Chip-pan]

From 2000 on (or with a hardware update on '98 or newer machines)the hihg speed option is a turn on in the control for appix $4000. This option adds a 80 block look ahead and some algrothims that allow the machine the machis to run at 300 ipm as opposed to 80 or so. To prove this out I ran a 4 x 4 x 2 in thick delrin in 2 machines. the cutter path is a full 3d and i used 2 tools. feedrate was 300 ipm at 7500 rpm, no coolant. The Haas did it without a hiccup at all. No slowdown could be seen,and the machine didnt shake at all!! The other machine , which had a software version of a high speed option, could not keep up to what the Haas did, and studderd like crazy at 300 ipm.

Needeless to say the OTHER company was pissed at me and said I doctored the file.

 

Not!!

Sore losers.

The Haas was 21 min faster and the finish was better.

 

Chip-Pan

[Müřlıń®]

Nomo, The guys who did all the programming before I came only used Proe and waterline cutting....this is probably why they didn't notice it. I started doing 3-d toolpaths and the stuttering became a factor.....

 

I understand it a little better now, thanks very much.....

 

Yeah Gcode...if I had my way I would lock them all down and run everything at 100%. But the operators would cry a river......they have alot more seniority than me....

 

Thanks for the info guys......

 

 

Murlin