Machine not running smoothly in 5-axis

[Bob W.]

I am porting some cylinder heads and the finished toolpath just isn't running very smoothly on the machine (Haas VM3) The machine tends to jerk and stop during the surfacing though the surfacing path really is very smooth with no sharp transitions. When I drop the feed rate to 80% it runs very smoothly so I assume I am running into a feed limitation on my trunnion.

 

I know it is a Haas, and not a Matsurra, but are there settings I can play with in the surfacing operation that will increase the feedrate at which this will run smoothly on the machine?

[Josh T™]

Hey Bob,

 

I've ran into similar issues in the past and have overcame them with great success. Here are a few ideas to help you out.

 

 

1) Clamp/Unclamp M Codes. This helped alot with the dwelling from the machine automatically releasing the trunnion brakes by producing the M Codes (M10 - M11 - M12 - M13) to force the clamp/unclamp before 5X paths. Thread on Clamp/Unclamp

 

2) Inverse Feed Rates. This was the best improvement to jerky 5X movements.

 

3) Filter Settings

 

4) Point/Line Generators

 

 

These are a few good places to start. Let us know how it goes.

 

HTH

Josh

[Bob W.]

Josh,

 

I have already implemented 1 & 2. Are there filters for true 5 axis machining? Also, what are the point/line generators?

 

Thanks,

Bob

[Josh T™]

When talking about filters there are no "true" filters but there are things you can do. First off, what toolpath are you using? Flowline or the Advanced 5X Port?

[Bob W.]

I am using the advanced 5x port toolpath and it just spirals down into the port but the machine frequently stops abruptly unless the feed is backed off a bit.

[DLG]

Do you have high speed machinning turned on?

I cut ports on our vf3, and the high speed machinng helps out alot.

we use x3 and the flow line tool path.

[Bob W.]

Yes, the machine's high speed option is turned on.

[Greg Williams]

Sounds bad,

 

What a are the toolpath tolerances?

Does the machine have a data server?

What feedrate have you programmed?

[Bob W.]

The toolpath tolerance was .001 and it runs much better with the tolerance set to .00025. The program is loaded in the machine's memory and I am also playing with the G187 settings. Funny thing is that it runs much faster with G187 P3 (finishing) and it is by a large margin. At G187 P1 (roughing) it is miserable. The programmed feed rate is 80ipm

[j.nguyen]

Can you control your lintol and max angle at the post level?

[FLHX95ci]

With G187 P1 it will run the Haas with it's most aggressive acc/dec parmaters, thus making the maching jerk more if you have real tight tolerancing. The maching will try to get up to speed as quick as possible from a dead stop.

 

Stay at the P1 and open up the tolerancing on Mastercam (don't be afraid to go as high as .02).

 

Also, you can use the "E" value which is your deviation. It can be from E.0001 - E.2000 the higher the value, the more deviation (smoother). It doense mean you will make a bad part though.

 

Try G187 P1 E.05 and if it still jerks, try G187 P1 E.1

 

The Haas control can run 1000 blocks per sec, so if the tolerancing is too might it will make really short moves.

 

MATH FOR BPS

F100. IMP = 1.6667 Inch Per Sec (100/60)

If tolerancing is set to .0005, that means it will take 3333.4 blocks to move thru 1.6667 inches of material, of 3333.4 Blocks per Second, which is 3x what the control can deal with.

 

Changing to .002 will drop that to 833 BPS.

 

The solution, make less lines of code.

 

Make sure Mastercam is outputting 3axis arcs, not segmented (G1) moves, a simple 90 deg arc can either be one line command, or hundreds of lines of code, depending on how the Mastercam is setup. The tighter the tolerance, the more code it outputs to move the same distance.

 

Depending on the mfg date of the Haas (I am a Haas dealer Applications Engineer) the HSM machining option will not help a ton. You can actually turn it on as a "Trial" basisfor 200 hours to see if it helps. Talk to your local HFO about that.

[Josh T™]

 

One of my customers has a VF3 (Circa 2006) with the TRT160 and no high speed option and he's porting 3 heads a day. Sounds like the filter is to tight.

 

quote:

---

The solution, make less lines of code

---

+1000 IMO

[Chris Rizzo]

quote:

---

Also, you can use the "E" value which is your deviation. It can be from E.0001 - E.2000 the higher the value, the more deviation (smoother). It doense mean you will make a bad part though.

---

Can you explain usage of the "e" value a bit?

[Bob W.]

The Haas machines have setings 191 and 85 that control smoothness. These can be controlled in the nc program using G187 Px Ey.yyy where p1 is roughing, p2 is medium, and p3 is finishing. The E value controls corner rounding though I believe its value doesn't correlate to inches.

 

G187 P1 E.1 would be very coarse where G187 P3 E.005 would be very accurate.

[?Mark]

Hey FLHX95ci,

Welcome to the forum.

I'm not a hass user, but must say that it's great to have an apps engineer for a machine tool builder chip in with some great info.

I'm surprised more builders are not encouraging their engineers to do the same.

[FLHX95ci]

The P1, P2, and P3 are more for dead sharp, 90 deg G1 to G1 type moves where as the E value could be more like a NURBS type setting.

 

I have run up to 200IPM on 90 deg square roughing routines (pocketing) and you need to get in excess of E.05 to get the machine to start to slow down at all, meaning it is mainatining the accuracy just fine and no improvment on that particular machine, acc/dec settings, etc... with a number any lower than that.

 

There are allot of dynamics here too. Machine size / weight is a big one. Saw customers buy a VF-6SS and load programs they were running on a VF-2SS, and have surface finish problems / longer cycle times on the 6. Even when using the same "E" value.

 

In the same example as above, testing would show the same program, IPM, etc... and the machine would start slowing down at a E.020. Why?

 

Table mass. The builder has to use allot lower Acc/Dec settings due to table weight and max part weight.

 

My suugestion is to run in the air with really tight accuracy settings out of X4 and mess around with the P1-P3 and E.0001-E.2000.

 

And i do not work for Haas, but one of the larger HFos in the coutnry.

[Bob W.]

quote:

---

Make sure Mastercam is outputting 3axis arcs, not segmented (G1) moves, a simple 90 deg arc can either be one line command, or hundreds of lines of code, depending on how the Mastercam is setup. The tighter the tolerance, the more code it outputs to move the same distance.

---

I'm not sure Mastercam can do 3axis arcs in true 5axis toolpaths. Can it do this? I believe my entire program is with linear moves (G1 commands). For 3 axis machining I filter my toolpaths whenever possible.

[Bob W.]

quote:

---

My suugestion is to run in the air with really tight accuracy settings out of X4 and mess around with the P1-P3 and E.0001-E.2000.

---

I have been doing this and in the process I have tried varying the cut tolerance in Mastercam from .0002 to .02 and I have tried P1, P2, and P3 settings on the machine with various E values. The settings that producd the best results were a cut tol of .0002 and G187 P3 E.025. I had to back the feed rate to 90% but it ran the fastest and smoothest by a mile. Everything else just got worse and appeared to be very hard on the machine.

[Bob W.]

I have been in contact with Haas and I emailed them all of my machine's parameters along with copies of the program with a few different cut tolerance settings. I'll post an update of what they come up with.

[FLHX95ci]

Take a scientific approach to it.

 

If the cut tol is .0002, and it is working good at G187 P3 E.025, then go up on the Cut Tol to .001 for example, and see if we can go up on the E value.

 

If the machine is "bumping" (sounds like someone is drumming on the sheetmetal) the machine is trying too hard to stay tight.

 

Also, being it is 5 axis, and it is a cylinder head, what kind of head? Motorcycle? Car head?

 

How close to rotation centerline are you? You might be at the limit of an angular feed max of the rotary product. The farther away from centerline the slower you can run.

[Bob W.]

Here is a video of one of these heads:

 

 

The machine is bumping and I tried E.1 and it didn't help. I tried multiple E settings and P settings with a cut tolerance at .001 and it did run smoother, but nowhere near the speed and smoothness of the tighter settings. Are there other machine parameters that can be played with (Accel time constant...)?

[FLHX95ci]

THe 5-axis drives may be a issue (how the drives are tuned) not many HFOs have allot of knowledge of the rotary axis products. We had one guy who was real good at tuning the trunions and it would make all the difference.

 

Its hard to diagnose over the web, but if it got faster at .001 then we may be on to something.

[Bob W.]

quote:

---

THe 5-axis drives may be a issue (how the drives are tuned) not many HFOs have allot of knowledge of the rotary axis products.

---

Right! I believe the problem is on the machine. How do I go about tuning the drives? I can't get the program to run any faster than in the video and all parameters are at the stock values other than A & B backlash. I don't really want to go too much faster. It is the smoothness I am after.

[Steve Hattori]

The problem I have seen with using bigger tolerances in mcam, is it then makes the line segments for each block longer, resulting in a facetted surface where you want a round one. The best-running and best finishing paths are huge amounts of 5-axis code. I know my machine is different than a Haas, but the program results from mcam should be the same. And I haven't seen mcam output 5-axis arcs in a simultaneous toolpath.

FWIW...

[DLG]

I had the HFO tech tweak the drives on my vf3,and the differance was night and day for sure on the 5 axis performance, I get perfect finish on the ports. Also a big plus on big amounts of code also, in inverse time.