Okuma Supernurbs

[Maclaw]

Hi Guys,

 

Anybody had problems/issues while using supernurbs on Okuma Genos M560R-V? I just got my machine up and running and were doing some air-tests - wanted to see its dynamic motion etc. My first experiences turned out to be : it works better... WITHOUT Supernurbs! I just had to push the supernurbs upper feed limit parameter to 20000mm/min while still having : CONTROL OFF. When I truned Supernurbs ON - the machine started jerking it's brains out...! I messed with these machine/program tolerance, filter setting, block lenghts etc. - had no visible improvement.

I programmed a part similar to the fancy X-Z movement zigzag that I saw on youtube (https://www.youtube.com/watch?v=p_vwe3kmDaE). I did it in MC X9 as a paralel surface along the X - feed was set to 10000mm/min and pumped it up to about 14000mm/min. I had a similar result as on the video - but with supernurbs OFF... Can Anyone explain this or also had issues with it?

Thanks

[jeff]

I don't have Super Nurbs, but I do have Hi-Cut Pro.

If it's anything like Hi-Cut Pro, it will jerk like crazy if your tolerances are too loose.

The tighter the tolerance, the more it will slow down at a corner/change of direction.

The looser the tolerance, the more it will try to stay at programmed feedrates at change of direction.

Do you have those parameters? If so what are they set at?

 

The max feedrate is just that. if you program your tool to cut at 20000mm/min but you set your max feedrate at 10000mm/min it won't go above 10000mm/min

[Maclaw]

I tested these parameters:

machine tolerance : 0.005mm to 1mm (!!!)

program tolerance: 0.0025mm to 0.5mm (!!!)

utilize reconst. shape : HIGH

max block length: 20

min block length: 0.05mm to 0.3 mm (0.3 was the default).

program filter : off and mode1 - the last did a little help.

Filter length : 0.02mm

filter angle : 0.5 deg

used all 3 maching modes (HQ, STAND. and HI-SPEED). the last one jerked like hell - I thought I'd lose all my sheet metal...  and stopped it after a few seconds. HQ was the slowest and jerked - but less then HS.

I really did not achieve any satisfying results with playing around with these settings - not close to the ones on the youtube video. The strange thing is - when I turned Supernurbs off - the machine started flying with high speed and almost ZERO jerking - as it was placed on cuchion pillows :-).... I Wonder if the Guy that made the video did put supernurbs on at all...? Maybe it's just marketing BS... Sorry but just dont know.

 

I put through 3 program types out of MC:

1) filter set to 0.02mm - no arc filtering - pure G1 lines

2) filter set to 0,0025 (like in the video) - no arc - pure G1

3) filter set to 0,0025 - with 50% arc filtering - the code consisted of a whole lot of arcs - almost no G1 curvature faceting. The code on this one was lik 3% of the one for 2).

 

All three programs worked well without supernurbs (comparable with the video) and not even close to the video with supernurbs on. Ther is also another parameter (i dont remember what it's called - since am not by the machine at the momemt) for supernurbs that consists of varios accel/decel axis paramters. These differ for HQ STANDARD and HI-SPEED. I suspect that maybe that's where the detail lies...? But I cant find anything in the manuals (theres like a 100 of these manuals :-). Do you have something similar for Hi-Cut PRO - another machine parameter just after the one with the tolerances?

[SlaveCam]

Sounds familiar. I used to use Super-NURBS in high-feed milling (10000+mm/min) but eventually stopped using it and just added more stock to walls to compensate for the lack of accuracy. Without Super-NURBS it may over/undercut about half a millimeter in tight arcs whereas in NURBS mode it will slow down considerably, generating more heat and wearing up the high feed inserts.

If I needed to cut an accurate 3D surface with a good surface finish, I'd turn it on. You shouldn't need to use Mastercam's smoothing with it.

[Colin Gilchrist]

This might be a dumb question, but does your code have Arc moves? Also, it isn't the Tolerance settings for the Hi-Cut Pro or SUPERNURBS that you need to worry about. It is the toolpath motion itself. No long lines, and no Arcs. You need G1, point to point motion. And short segments.

 

What toolpath are you using? What are your filter settings like? There are some Post Processor settings that can break your motion automatically.

 

'brklinestype$ = 11' will break all lines. Use 'brklineslen$' to set your segment length. And turning on 'linarc$' will linearize your Arcs. (Arcs get broken based on the value of 'chord_tol$'.)

[Maclaw]

Thanks for your posts Guys.

Colin, I used the old Surface finisz paralel toolpath. The toolpath at first didn't consist of any arc moves since I turned the arc filter off - so MC didn't generate G2 G3 moves. But... it did have quite long line moves in the toolpath - about 12-16mm. You're right - this might of caused the machine to go hi-speed on the long lines and then suddenly slow down on the linearized arc moves which were G1 moves of about 0.1 - 0.2mm - hence causing the jerking (you guys buy that explanation... :-) ). I will try breaking the NC code into small line moves and let You guys know how it worked.

 

Besides - do you Guys think messing with the OTHER Supernurbs parameter which containes Accel/Decel etc. for all 3 modes (HQ, STNADARD and HIGH SPEED) might be the solution? The parameter I'm talking about is also called Supernurbs.... and in my machine it lies just after the parameter where you pick the tolerances etc. I have no acces to my machine now (am staying sick at home...) but will post a screenshot right after I get better and You'll see what I mean.

[jeff]

Thanks for your posts Guys.

Colin, I used the old Surface finisz paralel toolpath. The toolpath at first didn't consist of any arc moves since I turned the arc filter off - so MC didn't generate G2 G3 moves. But... it did have quite long line moves in the toolpath - about 12-16mm. You're right - this might of caused the machine to go hi-speed on the long lines and then suddenly slow down on the linearized arc moves which were G1 moves of about 0.1 - 0.2mm - hence causing the jerking (you guys buy that explanation... :-) ). I will try breaking the NC code into small line moves and let You guys know how it worked.

 

Besides - do you Guys think messing with the OTHER Supernurbs parameter which containes Accel/Decel etc. for all 3 modes (HQ, STNADARD and HIGH SPEED) might be the solution? The parameter I'm talking about is also called Supernurbs.... and in my machine it lies just after the parameter where you pick the tolerances etc. I have no acces to my machine now (am staying sick at home...) but will post a screenshot right after I get better and You'll see what I mean.

Who's your distributor down in your area? It's Gosiger up here, and they are pretty good to work with over the phone. Maybe try calling them for help, or have them come out for a 1/2 day to show you the correct way to use it?

[Maclaw]

Yeah - thanks Jeff. Will try that.

I'm based in Warsaw, Poland. The Okuma Distributer here is HTM in Gliwice. Will have a word with them regarding the subject.

I will let You all know if I get any concise remedy regarding the subject.

In the meantime I wish You all a Merry Christmas with lots of joy and great time spent among Your Families :-)

[jeff]

 

I'm based in Warsaw, Poland. 

 

I'm an idiot, I looked quickly at your location and thought it said FL meaning Florida. 

[Maclaw]

not to worry my Friend, not to worry

just a few miles further to the east...

[Mick]

Okuma Europe should be able to help you out. All feedback I've heard about them has been very very good.

[Greg Williams]

I normally use these values for roughing in Metric

 

G131 F20000 J2 E0.05 D0.01 I0 L20 R0.3 K0 P0.01 Q5

[huskermcdoogle]

Maclaw  Have you looked at the smoothness of the toolpath itself?  Is the programmed motion perfectly smooth, or does it make a bunch of small sharp turns.  If this is the case, maybe you need to play with tolerances and smoothing in mastercam.  If that doesn't work, you possibly would need to filter the path itself.  Which shouldn't be needed as that is essentially what Super Nurbs does.  I am thinking that your settings in Super Nurbs are not quite compatable with your code.  Meaning either you are giving it too much data (highly unlikely) or not a fine enough point to point density and you are aren't achieving any gain by running super nurbs as a result.   I find with smoothing on a fanuc, that sometimes I need to filter the code heavily to remove sharp turns, as no matter what they end up gouging the part worse than the potential out of tolerance move... I have written some NCI filters that do pretty good work on a point to point basis, both 3ax and 5ax capability.  Post out and shoot me your NCI if you want me to take a look at the point to point data and filter it.

 

Husker

[ls1wot]

Maclaw did you ever get this figured out? I seem to be having the same issues with it, I just haven't had time to mess with it more. Curious how much tuning of the parameters is needed. Thanks

[Maclaw]

Hi Is1wot,

No - I still havent figured it out... Liearizing arcs did not change much.

Like SlaveCam wrote a few lines up in this post - I simply dont use SUPERNURBS when roughing (thanks SlaveCam for Your post) - just use it to finish. Be aware that when NOT in SUPERNURBS the speeds are very nice and dynamics is brilliant - the machine "flies" fast and doesn't jerk at all - however You get quite significant machining erros - especially watch your outside sharp corners (especially greater than or equal to 90 DEG) - they can be rounded off by even 1mm (R = 1mm)!!!

If I come up with something I will liet You know. Right now I a am pounded with loads of orders and work and don't have the time to experiment... :-( But it all is in the back of my head and waits to be remedied :-)

[Brad Lisle]

OK, Super-NURBS & Hi-Cut Pro in a nutshell...

First off, please note that Super-NURBS and Hi-Cut Pro will not speed up your program! In fact it will do quite the opposite and slow it down.

Here is the best way that I can describe Super-NURBS and Hi-CUT Pro: With either function turned OFF the machine will try to maintain programmed feed as much as possible. With either function turned ON the control will override the feed (acc/dec values) to maintain machine accuracies. Imagine trying to drive you car at 100mph and a sharp 90 degree corner is ahead. Do you smash the breaks just before the corner to navigate in you lane then throttle on as you come out of the corner, if so then Super-Nurbs or Hi-Cut Pro is engaged. Or do you stay on the throttle the entire time and keep the speed at 100mph, cutting the corner then swinging wide taking up the entire road and then some? This would be the results of Super-Nurbs or Hi-Cut Pro being turned off.

With that said lets look at some settings; First your toolpath must be CLEAN! I cannot stress this enough. Just because you generated a toolpath DO NOT assume it is good. Actually look at it with a fine tooth comb. Typically when you get jerking the toolpath is to blame. If you zoom in on it and when you think you zoomed in enough keep zooming in, you will see the toolpath jumping around in crazy directions. To help eliminate this I recommend running the filter as tight as possible (I typically run at .0002" or less) and linearize everything. This will cause long regen times and crazy long programs, but who cares the Okuma OSP loves it!

For the Super-Nurbs settings (G131 D_ J_ E_ F_ I_ L_ R_ K_ P_ Q_) or For the Hi-Cut Pro settings (G131  J_ E_ F_):

G131=ON   G130=OFF

D= Program tolerance; have this match the filter tolerance in MCAM

J= Machining mode; 0=High quality (Super-Nurbs only), 1=Standard, 2=High speed; 0 for fine finishing, 1 for finishing and general roughing, 2 for 3D surface toolpath roughing

E= Machining tolerance; this is the allowable error from point-to-point that you can cut the corner (drive across the grass in the example above). Typically I run .002"-.004" when roughing / Semi-Finishing and .0002"-.0004" when finishing

F= Feedrate upper limit; This will not increase the programmed federate! it will only limit the max, similar to a G50 S___ on a lathe. If the operator turns the federate override to 200% that could cause damage to tool/part/machine. By setting this value you can limit the allowable override. I typically always set this at 1240. since that is the fastest I have ran a tool in material to date.

I= Utilize Reconstruct Shape; 0=Low, 1= Medium, 2= High, 3= Full; Since I typically set my program filter tolerance very low (0.0002") and linearize everything I do not need the OSP control to reconstruct the point as much as I would need if there were spline segments. So I typically have this set to 0 (Low), if there are any splines I would either re-create geometry to select from or set this to 2 (High) or 3 (Full).

L= Max block length; Default (20.0mm or 0.7874")

R= Min. block length; Default (0.3mm or 0.0118")

K= Program filter mode; Default (Off); 0= Off, 1= Mode 1 on, 2= Mode 2 on, 3= Mode 1 & 2 on; If you toolpath is clean, you should not need this enabled. However, if you still have toolpath that jumps around you may need to enable this function.

P= Filter value length; Default (0.01mm or 0.0004)

Q= Filter value angle; Default (5°)

 

I hope this helps, also please refer to the manual for additional information.

 

Super Nurbs.doc

[jeff]

Thank you for that detailed explanation Brad!!

Very helpful!

[Brad Lisle]

No problem, hope it helps