Haas high feed milling settings

[Pilot Plant Supervisor]

I just bought some Seco High Feed milling tools for an upcoming job. The feed rates suggested by the rep are a little scary, and I'm a bit sceptical about the Haas keeping up. I'm going to be running on a Haas VF-3 with High Speed Machining option. I want to program with feed rates in the 400-500 IPM range, but the longest cut will be around 10". Will the machine accelerate/decelerate quickly and smoothly enough? What should I have the control set to (Rough, Medium, Finish, Corner rounding)? I had to change the corner rounding setting when Dynamic milling to keep from snapping a .125 endmill that was hanging out 1.25", but this application is a bit different. Any thoughts?

[mkd]

my thoughts would be to program over- runs, that is lead in and lead out to allow time for the machine to accel. obviously to ensure consistent chip loads.

 

they just don't change direction like the premium Jap brands.

[Chris Rizzo]

You'll be able to get it to work. Several years ago (on the old format forum) there was a huge thread on the actual specifics of this. I copied and pasted the most informative response from a fellow that worked for a HFO. He doesn't really give a recommendation on outright values to try unfortunately. He's refering to using G187 to change the values on the fly. (You can just change them manually in the controller, but you'll have to adjust per op if you are roughing and finishing). There are posts made that have the Misc Values with G187 and E#'s you can control for each op right within mastercam. It's pretty nice. Give the dealer (Mcam) a call and they might have one available, if you really get into using this feature.

 

Oh, also toolpath FILTER is going to be another very important setting, for minimal code and nice big arcs, (vs. little lines). I'd say filter is going to me almost more important than machine settings. Hint: In your backplot, change the color of arcs to orange (or whatever) and you can easily see when you've got arcs and where you got lines. They will still be blue.

HTH

 

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

 

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 doesn't mean you will make a bad part though.

 

The Haas machines have settings 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.

 

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

One more thing to consider when changing setting #191 to rough is that this multiplies the value in setting #85 max corner rounding by four.

G187 Pm Ennnn sets both the smoothness and max corner rounding value. G187 Pm sets the smoothness but leaves max corner rounding value at its current value. G187 Ennnn sets the max corner rounding but leaves smoothness at its current value. G187 by itself cancels the E value and sets smoothness to the default smoothness specified by Setting 191. G187 will be cancelled whenever “Reset” is pressed, M30 or M02 is executed, the end of program is reached, or E-stop is pressed.

 

MATH FOR Bits Per Sec

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.

 

 

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.

 

 

 

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.

[Pilot Plant Supervisor]

Great info Chris, Thanks!!!

[workmantm]

Don't forget to use your G103 for look ahead on the program. You can't use it with Tool Wear offsets, but you can open up the control's ability to move at a constant speed. I use G187 all the time to try to open up the old HAAS Vf-1 and Vf-4 we have here. V9 and V10 controls. When I'm roughing I tend to run G187 E.05 and G103 P15. Cancel using G187 and G103 on separate lines. I leave our Setting 85 at .001 here to ensure we keep features at size when finishing. I'm doing a couple Dynamic path test and I found that keep the tools down using this combo and running the machines at F300. for rapid moves was faster than rapiding up and around. In the past before I found my tuning tweaks it was always faster to rapid up and around the part with the tools. The the "P" designations also can drive a huge increase in productivity on newer controls. I've managed to successfully refine a couple programs on the latest version of the VF-2SS for a friend.

 

Ask if you need something else clarified and I'll do my best to help guide you to the best method for your Haas.

[Machineguy]

When running macros on a Haas, you have to call G103 P1 at the start, and G103 P0 at the end on the macro.

The P1 tells the Macro to look one line at a time. P0 sets it to default mode.

I'll have to play with the G103 P command on our VM-3 and see if I get a difference. The high speed option is turned on so I dont know how it will effect this newer machine. I'll talk to Haas to see what the look ahead is on the newer software.

 

Machineguy

[FTI2007]

Now I am starting to understand why our Haas slow down so much and never make it to the programed feed rates. Where I work they just always said it was just because its a haas. So I never questioned it. Can you Please go in to more detail about the codes needed and what they do and where to put them. Maybe an example would be great also. Thanks

[mkd]

been working on Haas' machine way too long to have never used G103.

how does switching it in the program help?

[FROZEN]

Does any one know if Kitamura 3xi has a high speed G-code

[Pilot Plant Supervisor]

Now I'm really confused. I bought the High Speed Machining option from Haas, but I need to use G103 to limit look ahead???

[FTI2007]

im confused to. we also thought that when we bought the high speed option it would take care of it. Now it sounds like we need to add a bunch of codes to get the machine to run properly. Hopefully someone here can take the time to explain this to us.

[Machineguy]

The High Feed Option turned on the look ahead to 80 blocks. Thats it.

I have the option in the Haas post i have to change the G187 mode from P1 to P3.

The settings in the machine is set a G187 P2. thats for the corner smoothing. If I set it at P3 in the Misc ops I see the machine slowing down in the corners and speeding up when it leaves the corners.

I have never used G103, except for Macros. I set it at P1 in a macro. That sets the look ahead to 1 block. When the macro is done its set pack to G103 P0.

That sets the machine to its default, which is 80 blocks with the high feed option turned on.

Now a a example, I ran a Toolroom mill without the high feed option turned on and did a surface path with a lot of free flowing curves. the machine movement just shook the machine at 80 ipm. turned the feed down to 25 ipm and the machine still jerked but it was a lot less noticeable.

Next i turned the trial option on for the high feed option. Ran the same path at 80 ipm. The machine ran smooth as silk up to 120 ipm. I was way out of range for only 4000 RPM but i saw a big difference.

 

Does this help?

 

Machineguy

 

THe High feed option was a option about year 2000. I did have a 1998 VF-3 updated to add the feature but that was a 3 board change in the controller to get everything working.(floopy disk was the main problem) I dont think it can be done now.

[Matthew Hajicek - Singularity]

Does any one know if Kitamura 3xi has a high speed G-code

 

We have four Kitamura horizontals of different ages and sizes, and they use AICC / AI APC. The oldest is just G5.1Q1 to turn it on and G5.1Q0 to turn it off. For the rest when you turn it on you add a P#, P1 through P10, P1 being smoothest and P10 being most accurate. So for a finish path I do G5.1Q1P10. You also need to have a G49 before the turn on call, otherwise it gets confused.

[workmantm]

I've noticed an improvement on both of our '96-'99 generation Mills using G103. It dramatically improved what I was getting since I was watching the machine move slowly around corners. That pretty much made dynamic paths worth very little. I also noticed that with a new 2013 generation VF2SS that I would get some improvement with the G187 and G103 running together. I just consult and tune for the VF2SS, so I do not have long term cycle improvement feedback other than what the owner gives me when I stop in to see him. I check his cycle times and make sure his tool are living up to the expected life I said they should be getting. We saw reduction in cycle times when we applied the G103 P15 to his roughing code.

 

We do not have the high speed options on these machines. VF2SS does have the option. I have both set to .001 on setting 85. That may also be a big reason that I am seeing such a difference. We keep it that tight to ensure interpolation of .001 tolerance holes stay where we want them in the end.

 

It has come down to tuning my code to the individual machine as far as using the G187 and the G103 codes. I can't say that everyone will have the same results or that there is something that is unique to how the code is output by MC either. I can only say that those are the two things I look at when I need to wring every last little bit of time out of the programs that we are running here. YMMV. I hope that helps people tune for their specific machines in the end.

[SGoertz]

Apparently with prior New Gen controls, you cannot use Tool Radius Compensation with G103 P## anything other than 0.

[crazy^millman]

2 hours ago, SGoertz said:

Apparently with prior New Gen controls, you cannot use Tool Radius Compensation with G103 P## anything other than 0.

Thank you after 6 of waiting I was wondering if anyone was going to help them out. Appreciate your willingness to help someone that was sitting around for 6 years waiting on your to bring this back up and help them. 

Sorry, I appreciate anyone who can read old topics and be helped, but what purpose does it serve for people to do the drive by answers from old topics? 

[Ewood42]

22 hours ago, 5th Axis CGI said:

...but what purpose does it serve for people to do the drive by answers from old topics? 

It gets people to re-read an old very helpful post from Rizzo, then be depressed that he's gone. 

[crazy^millman]

1 hour ago, Ewood42 said:

It gets people to re-read an old very helpful post from Rizzo, then be depressed that he's gone. 

Yes like he like others are missed.