NURBS--Anyone using this Machine option???

[DrewG]

I have been going crazy with Makino and Fanuc trying to get this option to work on our new A66E Horizontal Machining Center. Each manufacturer states it's something wrong on each others end (Fanuc states Makino's got something wrong in their parameters, and Makino states Fanuc has a hardware problem). The major problem is trying to get a person either at Makino or Fanuc who even knows what a NURB curve is. The service guys who came from both companies had absolutely NO experience with NURBS, and just read from the book trying to get something to work to no avail.

 

Makino installed their optional SGI.3 high speed control option, Buffer Mode, Data Server and parameter changes, and Fanuc turned on their "NURBS Interpolation" option. However, when the program gets to a NURB call out the control alarms out with "Illegal G-Code". The following is a sample of the code were using:

 

%

O0001

( PROGRAM CC400-OP.1-1 PART )

( MON NOV 21 21H31M17S 2005 )

 

(TOOL T45005000 DIA 0.5000 .500 BULL MILL )

 

G20

G00 G90 G80 G40 G17 G49 G94

G91 G30 Z0

G90

(CALL OFFSET FILE)

M98 P7998

M01

 

T45005000 M06

S18000 M03

M253 (SUPER SGI.3 ON)

G05 P10000

M42 (150 PERCENT ALLOWABLE AMP LOAD-MAKINO SPINDLE MONITORING)

 

(12 FREEFORM FINISH ID RADIUS WALL)

G90 G00 G54.1 P1

M11

B0

M10

M08

X2.9264 Y2.9947

G43 Z.05 H1

Z-1.05

G01 Z-2.55 F340.

G06.2 P4 K0 X-1.0736 Y2.9947 Z8.58 R0 F400.

K0 X-1.0365 Y2.8368 Z8.58

K0 X-.9718 Y2.6644 Z8.58

K0 X-.864 Y2.4689 Z8.58

K.044 X-.5538 Y1.9615 Z8.58

K.0495 X.065 Y1.5812 Z8.58

K.0606 X.8816 Y1.5141 Z8.58

K.2057 X1.2589 Y1.568 Z8.58

K.2169 X1.5985 Y1.7134 Z8.58

K.2835 X1.8875 Y1.8714 Z8.58

K.3058 X2.1139 Y2.0609 Z8.58

K.317 X2.3077 Y2.3015 Z8.58

K.3729 X2.4008 Y2.4386 Z8.58

K.3841 X2.5292 Y2.6741 Z8.58

K.401 X2.632 Y2.9684 Z8.58

K.4178 X2.6754 Y3.2747 Z8.58

K.4569 X2.6787 Y3.5604 Z8.58

K.4848 X2.6488 Y3.7834 Z8.58

K.5014 X2.586 Y4.0184 Z8.58

K.5344 X2.529 Y4.1712 Z8.58

K.5454 X2.4221 Y4.3906 Z8.58

K.5675 X2.3092 Y4.5621 Z8.58

K.5785 X2.1496 Y4.7474 Z8.58

K.6117 X2.0311 Y4.8607 Z8.58

K.6228 X1.8704 Y4.9871 Z8.58

K.6449 X1.5945 Y5.1638 Z8.58

K.656 X1.1625 Y5.3183 Z8.58

K.6782 X.7488 Y5.3391 Z8.58

K.7337 X.5039 Y5.3118 Z8.58

K.7782 X.3822 Y5.2901 Z8.58

K.7894 X.1821 Y5.2409 Z8.58

K.8006 X-.5077 Y4.9722 Z8.58

K.8118 X-.9778 Y4.3824 Z8.58

K.8453 X-1.0947 Y3.7626 Z8.58

K1. X-1.0947 Y3.7626 Z8.58

K2.

K2.

K2.

K2.

X2.9053 Z-2.55

X2.9045 Y3.7551 Z-2.5391

X2.9049 Y3.7484 Z-2.5398

X2.9065 Y3.7426 Z-2.5406

X2.909 Y3.7377 Z-2.5414

X2.9125 Y3.7336 Z-2.5421

X2.9167 Y3.7304 Z-2.5428

X2.9215 Y3.7281 Z-2.5435

G06.2 P4 K0 X-1.0785 Y3.7281 Z8.5865 R0 F400.

K0 X-1.073 Y3.7261 Z8.5857

K0 X-1.0669 Y3.7256 Z8.5857

K0 X-1.0612 Y3.7261 Z8.5844

K1. X-1.0612 Y3.7261 Z8.5844

K2.

K2.

K2.

K2.

G06.2 P4 K0 X-1.0612 Y3.7261 Z8.5844 R0 F400.

K0 X-1.057 Y3.7264 Z8.5845

K0 X-1.0506 Y3.7278 Z8.5845

K0 X-1.0425 Y3.7312 Z8.5844

K.1813 X-1.0365 Y3.7344 Z8.5843

K.2758 X-1.0308 Y3.7385 Z8.584

K.3724 X-1.0256 Y3.7433 Z8.5837

K.4708 X-1.0209 Y3.7488 Z8.5833

K.5711 X-1.0156 Y3.7574 Z8.5827

K.6734 X-1.0129 Y3.7646 Z8.5821

K.7783 X-1.0118 Y3.7697 Z8.5816

K1. X-1.0118 Y3.7697 Z8.5816

 

etc.....................

 

Is anyone using NURBS on either a Makino or any other machine? If so, do you have a sample of the code your using so I could give it a try and see if I get anything different. We tried using a sample code direct from the Fanuc manual and still had no luck. Any ideas?????

Thanks in advance for any posts!!!

[Greg Williams]

Hi Drew,

 

Just out of Interest, Why do you want to use this option?

 

My experience and tests with SGI show no real advantage with Nurbs on certain parts.

 

SGI mode cannot be used with B axis Rotation

[Guest CNC Apps Guy 1]

I have a fair bit of NURBS experience. What are you using to get your NURBS Code???

[DrewG]

Greg,

We won't use it on every part, only certain parts that can benefit from it. From what I've read, NURB curves are more accurate, although that's not a major problem. With NURBS the program can be significantly shorter, and the machine can process the code significantly faster and more accurate. I really want to run some test's to see how much faster we can machine on some of the parts I believe can benefit.

 

James: I believe the code is either from Esprit or UG NX3. I'm not at work anymore to be able to look up the part to confirm. I can give you a firm answer on Tuesday. The Fanuc rep. tried using a test program from Fanuc and got the same results. Do you have a suggestion, something to try, or something to look for? Thanks!!!

[DrewG]

JAMES--This particular part was programmed and posted in Esprit 2005. Thanks!!

[Guest]

Could always try the Esprit forum.

 

[specv]

DREWG

I am looking in my Makino prgramming manual for our A66 an it shows using G6.1 NOT G6.2 just a thought.

[gcode]

quote:

---

Could always try the Esprit forum

---

Do they have an Espirt fourm??

[CAM-mando]

quote:

---

Could always try the Esprit forum

---

LOL @ John

[DrewG]

specv--Thanks, I will double check that.

 

Guy's, yes Esprit does have a forum, and a pretty good one at that. I would not say it has anywhere near the amount of users as this one though, and my question isn't an Esprit question, but a question relating to NURBS.

 

I don't believe(but I could be wrong), that it's a post issue as this same code ran on another Makino. I also have tried code direct from Fanuc and UG as well to na avail. If Mastercam was able to post NURBS, I would give that a try too.

 

I was looking to see if anyone had a sample code (Fanuc control) that they know runs on their machine and uses NURBS so I could run another test.

[Guest CNC Apps Guy 1]

I''ve got a few programs. Looking for one I can part with and not get into trouble for doing it.

 

In the mean time here's some info about NURBS;

 

A sample snippet would look something like the following;

 

%

O9999(NURBS DATA)

G00Z2.54

G05P10000

X11.9456Y1.0389

G1Z-1.9257

G1X11.8986Y1.7906Z-1.9404

G6.2P4K0.X11.8986Y1.7906Z-1.9404R1.0

K0.X11.8809Y1.7246Z-1.958

K0.X11.8544Y1.6254Z-1.9844

*

*

*

K9427.5X11.4913Y.2705Z-2.3331

K9427.5X11.4736Y.2044Z-2.3496

K10000.

K10000.

K10000.

K10000.

G00Z2.54

G05P0

M99

%

 

 

The G6.2 is obviously the G Code to put the control into NURBS mode. The "P" is the Spline Order, the "K" is the Knot Vector, and the X, Y, and Z coordinate is the Control Point location and the "R" is the Knot Weight.

 

I have successfully run programs that were generated in UG so I would trust their Post Processor. I've also used point to point programs run through Metacut Pro and had good success with their NURBS Translator.

[Guest CNC Apps Guy 1]

Found one.

 

I PERSONALLY ran this code and it was successful.

 

It's metric and was run on a Mori Seiki SV-500.

 

HTH

 

code:

---

% 

O7102(MAIN/NURBS)

G90G54G0X0Y0S50000M3

G43Z100.H12

F2000

M8

G05P10000

M98P7011(SUB-TOLERANCE)L50

G90G0Z100.

G05P0

M9

G91G28Z0M5

M30

 

O7011(TOLERANCE 0.02)

G00X0.01

Z62.

G91G1Y0.1(PITCH)

G90

G01Z47.

X7.843

G06.2P3K0.X7.843Z47.R1.

K0.X7.9336Z47.9424R.9999

K0.X7.998Z48.887R1.

K1.X8.1085Z50.1196R.8497

K1.X9.262Z50.568R1.

K2.X9.9145Z50.86R1.

K2.X10.567Z51.152R1.

K3.X11.304Z51.4255R1.

K3.X12.041Z51.699R1.

K4.X12.7935Z51.926R1.

K4.X13.546Z52.153R1.

K5.X14.3115Z52.332R1.

K5.X15.077Z52.511R1.

K6.X15.8525Z52.6415R1.

K6.X16.628Z52.772R1.

K7.X17.41Z52.8535R1.

K7.X18.192Z52.935R1.

K8.X18.9775Z52.967R1.

K8.X19.763Z52.999R1.

K9.X20.5485Z52.9815R1.

K9.X21.334Z52.964R1.

K10.X22.1175Z52.8975R1.

K10.X22.901Z52.831R1.

K11.X23.6785Z52.7155R1.

K11.X24.456Z52.6R1.

K12.X25.225Z52.4355R1.

K12.X25.994Z52.271R1.

K13.X26.7505Z52.0585R1.

K13.X27.507Z51.846R1.

K14.X28.249Z51.5865R1.

K14.X28.991Z51.327R1.

K15.X29.7155Z51.0215R1.

K15.X30.44Z50.716R1.

K16.X31.1435Z50.3655R1.

K16.X31.847Z50.015R1.

K17.X33.0033Z49.354R.9999

K17.X34.145Z48.668R1.

K18.X41.5275Z44.4677R.9571

K18.X50.Z45.067R1.

K19.X51.9868Z45.0538R.7136

K19.X52.01Z43.067R1.

K20.Z42.5335R1.

K20.Z42.R1.

K21.

K21.

K21.

G01X70.

G00Z62.

X0.01

M99

%

---

[DrewG]

Thanks James!!!! That's exactly what I was hoping to find, something that has been proven on another Fanuc control. I will try feeding the Makino the code on Friday (I'm probably one of the rare few at work after Thansgiving Thursday).

 

I will post back to you than. Thankyou for taking YOUR time to both find that, and post it. Thanks again!!

[Guest CNC Apps Guy 1]

Glad I could help.

[Carl Hessig]

Drew are you trying to run from the dataserver.

You can't make M98 subprogram calls from there.

 

Carl

[DrewG]

Carl, I was also having problems with trying to get the data server to work. This Makino is part of a cell with a Cell Controller. I will have to see how Makino handles this. The M98 sub program is set up the way Makino calls for it in their Cell Controller example. Thanks!!!

[Guest CNC Apps Guy 1]

So, what's the word???

[DrewG]

James, I haven't had the opportunity to try it yet. I'm sorry. I have been awaiting a call back from Jeff Wallace at Makino to see if he can answer some of my questions. It seems he is always on the road, so I may not wait any longer. I'll try it this week at some point, whether I hear from him or not. I promise to post once I figure it out in the hopes it may help someone out in the future. Thanks!!