Okuma Hi2NC/Hi Nurbs

[Mick]

Does anyone here use the Hi2NC/Hi Nurbs option for surface machining on their Okuma verticals? I'm interested in what settings you use, as we haven't had a lot of success with it, and our local agent isn't very helpful.

 

When running large 3 axis surface toolpaths, the machine motion seems to be very slow, even with a programmed high feedrate. I'm interested to hear from any other Okuma users utilising this option, and what settings are being used.

 

Cheers

[gcode]

Mick,

Don't you have to use nurbs toolpaths to take advantage of this option?

Mastercam can't output nurbs so I don't think

you'd gain anything running an MC generated toolpath with nurbs activated.

[Psychomill]

I agree with gcode here. If this option is similar to Nurbs of other machines/controls, you need the positions of the control points for this to function properly. I'm guessing that you cut a spline, posted it, and trying to run that code. The increments are tiny that way. And although the toolpaths may appear "correct", this is what is causing the slow feeds because the control is calculating the spline based upon the points in the program.

 

If you don't know the points, or you're generating from an existing file, then MC can create the points for you. First determine if the spline is parametric or nurbs. If nurbs, just go " create > points > Cpts Nurbs " and select the spline. If its parametric, then you'll have to convert first. Go " modify > x to nurbs " and select the spline. Now create the control points for a nurb spline.

 

MC will program a nurb spline if you have the control points. You can program by selecting the control points using "Contour" toolpath. Then for the selection use the "Point" method. You have to select "point" each time for each point though. Otherwise you end up going point then accidently selecting some other type of chain.

 

 

 

PS: if you knew this already, then just ignore me

[Mick]

Thanks for the replies

 

I apologise, I used the wrong description. Its the Hi2NC function I want to know about. Its the high speed "look ahead" function for contouring/surface toolpaths. My experience with it so far, is that the machine motion is smooth sometimes, and other times it pauses, or shudders. We're using the DNC/DT transmission option (ethernet) so it isn't a data flow issue.

[Guest CNC Apps Guy 1]

You are going to NEED MetaCut Pro to get NURBS code from MC. It is an outstanding Product. I used it quite a bit while I was an AE at Mori Seiki for HSM Demos.

[35K chipper]

is this an OSP-U100M control? if it is are you using g130/g131 (off/on).

[Mick]

35K Chipper,

 

We have two machines, a U100M, and a E100M. According to the machine manuals, the Hi2NC can be switched on at the control, or using G130/G131. We cant get it to work with G130/G131 (neither can another couple of companies locally using the same machine). When it is functioning (we have it switched on at the control), it shows it on the control, flashing a display (I cant remember the actual text it displays).

 

My question is, what settings do you use? when I was running a Matsuura with a Yasnac i80M, and HON/HOF high speed machining, we just switched it on, and we naver had a problem. With the Okuma, it seems to work some of the time. Since there are several settings on the parameter page, I'm curious to see what other users are using for settings, when machining 3D surfaces.

 

I'll check our settings at work tomorrow and post them here

[Greg Williams]

Mick,

 

Something like this in your post should do the trick

 

if mi8 = one, n,"G131 J0 E0.001 D0.0005 I0", *feed, "(SUPER NURBS ACCURACY SETTINGS)", e

 

if mi7 = one, n,"G131 J0 E0.005 D0.001 I0", *feed, "(SUPER NURBS HIGH SPEED SETTINGS)", e

 

So the Gcode is

 

Blah

Blah

G131 J0 E0.01 D0.001 I0 F8000

Blah

Blah

 

Works fine in my old companies Okuma

[35K chipper]

Mick,

there are two prameter pages in the control that need to be set.

the first page is what i call the fall back mode or G130 mode. this

is how your machine will respond if you do not call G131 in your or

G130 in your program. the values in my machine are as follows:

execution mode = 1

feedrate upper limit = 400 -IPM-

machine mode = 0

machining tolerance value = 0.0002

program tolerance value = 0.0001

utilization level of reconstructed shepe = 3

this fall back mode is the slowest and most precice.

 

the second prameter page has three colloms this is the G131 modes.

the values in my machine are as follows:

 

High Quality Standard High Speed

machining tolerance 0.0002 0.0003 0.0006

program tolerance 0.0001 0.0002 0.0004

utilize reconst. shape 3 1 0

max block length 0.400 0.600 0.800

min block length 0.005 0.010 0.020

program filter mode 0 0 0

filter value: length 0.0003 0.0005 0.0012

filter value: angle 5 7 10

 

 

now is the fun part. the snips from one of my Okuma posts shows 24 different

modes that are selectable from mi8. this allows you to change HiNC modes for any

operation -ex can cycles or rapids- to the mode that best fits this operation.

the modes 1-12 are from the 3 machining modes 0,1,2 and the 4 shape reconstruction

levels 0,1,2,3. the modes 13-24 are the same as 1-12 with the filter values turned on.

 

machining mode = J

shape reconstruction = I

finter mode = K

 

____________________________________________________________

 

 

"SUPER Hi-NC"

 

[misc reals]

1. "'X' STEP AMOUNT [ + - 0.0000 ]" -mr1-? 0.0

2. "'Y' STEP AMOUNT [ + - 0.0000 ]" -mr2-? 0.0

3. ""

4. ""

5. ""

6. ""

7. ""

8. "Stock, Blank, or Part Thickness"

9. "Stock, Blank, or Part Width"

10. "Stock, Blank, or Part Length"

 

[misc integers]

1. "Starting WCS [1= G15H1 40= G15H40,etc.]" -mi1-? 1

2. "Sub Reps for all tools [0 - 40 Reps Max]" -mi2-? 0

3. "Sub Rep from each tool = 1 All tools = 0" -mi3-? 0

4. "Stage tools for OK 7 or 8 = 1 No Stage = 0" -mi4-? 0

5. "Merge an EXT file [1= Merge 0= No Merge]" -mi5-? 0

6. "Work shift in X = 0 , Work shift in Y = 1" -mi6-? 0

7. "Total number of work shifts for this part" -mi7-? 0

8. "Super Hi-NC OK8 only [0= off 1-24 on]"

9. "Spindle face air blast [OK8 only 1= ON]"

10. "Part Type Selector [0 - 20]"

 

-----------------------------------------------------------

 

 

phincoff # Super Hi-NC off selector

if mi8 = 0, "", e

if mi8 = 1, "G130", e

if mi8 = 2, "G130", e

if mi8 = 3, "G130", e

if mi8 = 4, "G130", e

if mi8 = 5, "G130", e

if mi8 = 6, "G130", e

if mi8 = 7, "G130", e

if mi8 = 8, "G130", e

if mi8 = 9, "G130", e

if mi8 = 10, "G130", e

if mi8 = 11, "G130", e

if mi8 = 12, "G130", e

if mi8 = 13, "G130", e

if mi8 = 14, "G130", e

if mi8 = 15, "G130", e

if mi8 = 16, "G130", e

if mi8 = 17, "G130", e

if mi8 = 18, "G130", e

if mi8 = 19, "G130", e

if mi8 = 20, "G130", e

if mi8 = 21, "G130", e

if mi8 = 22, "G130", e

if mi8 = 23, "G130", e

if mi8 = 24, "G130", e

if mi8 - 24, "", e

 

 

phinc # Super Hi-NC output selector

if mi8 = 0, "", e

if mi8 - 0 & mi8 < 25, phinca, e

if mi8 - 24, "", e

 

phinca # Super Hi-NC Control Selector

if mi8 = 1, "G131J0I0", e

if mi8 = 2, "G131J1I0", e

if mi8 = 3, "G131J2I0", e

if mi8 = 4, "G131J0I1", e

if mi8 = 5, "G131J1I1", e

if mi8 = 6, "G131J2I1", e

if mi8 = 7, "G131J0I2", e

if mi8 = 8, "G131J1I2", e

if mi8 = 9, "G131J2I2", e

if mi8 = 10, "G131J0I3", e

if mi8 = 11, "G131J1I3", e

if mi8 = 12, "G131J2I3", e

if mi8 = 13, "G131J0I0K1", e

if mi8 = 14, "G131J1I0K1", e

if mi8 = 15, "G131J2I0K1", e

if mi8 = 16, "G131J0I1K1", e

if mi8 = 17, "G131J1I1K1", e

if mi8 = 18, "G131J2I1K1", e

if mi8 = 19, "G131J0I2K1", e

if mi8 = 20, "G131J1I2K1", e

if mi8 = 21, "G131J2I2K1", e

if mi8 = 22, "G131J0I3K1", e

if mi8 = 23, "G131J1I3K1", e

if mi8 = 24, "G131J2I3K1", e

 

 

 

pblow # Spindle nose blow

if mi9 = 1, "M121", e

 

pblowoff # Spindle nose blow off

if mi9 = 1, "M9", e

 

 

--------------------------------------------

 

 

pheader # File header

spaces_sav=spaces

sextnc = ucase-sextnc-

spathnc = ucase-spathnc-

if mi5 = 1 & mi2 <- 0, q1

"$", progname, ".", sextnc, "%"

"-PROGRAM FILE NAME - ", progname, ".", sextnc, "-"

"-OPERATION - ", *progno, "-", e

spaces=0

"-PROGRAMMER - MIKE JONES-"

"-POST NAME - ", snamepst, "-"

"-DATE - ", *smonth, "-", *day, "-", "20", *year, " TIME - ", *time, "-"

spaces=spaces_sav

 

 

 

psof0 # Start of file for tool zero

psof

 

psof # Start of file for non-zero tool number

if tplnout = one, ttplane = wbuf-one,wc1-

ptravel

pwritbuf5

pinit

if metric = 1, pmetric

tooltotal = rbuf-4,0- #Reads total tools used #Index!

if toolcountn <= tooltotal, nexttool = rbuf-4,toolcountn-

else, nexttool = first_tool

 

 

if mi5 = 0 & mi2 <- 0 & mi7 <- 0, pprtoff, e

pparts

 

spaces=0

if output_z = yes, "-PGM Z MAX ", *z_tmax, "-"

if output_z = yes, "-PGM Z MIN ", *z_tmin, "-"

 

spaces=spaces_sav

 

subprg = yes # Open subprogram file? yes/no

subprogno = progno

tlnxt = mi4

dumsub = mi3

if dumsub = 0, numsub = mi2

if dumsub-0, numsub = mi2 # Store number of subprograms

mi1org = mi1 # Original mi1 value

mergeext

*sg00, *sgabsinc, "G80", "G40", "G17", "G94", e

 

 

prv_absinc = c9k

 

 

"N", *t, e

"IF [VATOL EQ ", *t, "] N", *next_tool, nna, e

pblow, e

 

"T", *t, "M6", e

pblowoff, e

"N", *next_tool, nna, e

ptoolcomm, e #Tool!

comment, e

 

 

spaces=0

if output_z = 1, preadbuf5

if output_z = 1, "-", "MAX ", *max_depth, "-"

if output_z = 1, "-", "MIN ", *min_depth, "-"

if tlnxt = 1 & next_tool <- 1, "/T", *next_tool, " -IS THE NEXT TOOL-"

 

 

spaces=spaces_sav

 

if tplnout = one, ptplane

 

startflg = one

nobrk_sav = nobrk

nobrk = one

 

pstock #Stock!

pindex #Index!

last_op_id = op_id

 

ptoolend # End for current tool

!coolant, !opcode

 

ptlchg0 # Null tool change

toolcount = toolcount + 1 #Index!

prvtp = rbuf-3,toolcountp- #Index!

if toolcountn <= tooltotal, nexttool = rbuf-4,toolcountn-

else, nexttool = first_tool

 

if tlplnno <- prvtp, "G0G30P1"

 

if tlplnno <- prvtp, pindex #Index!

 

if opcode = three, ptlchg0drl

 

 

spaces=0

comment

spaces=spaces_sav

 

if op_id<-last_op_id, pstock #Stock!

 

speed

smcool

if tplnout = one, ptplane

last_op_id = op_id

 

ptlchg # Tool change

if numsub-0, phincoff, e

if numsub-0, "RTS"

if numsub-0, " "

if numsub-0, " "

 

subout = 0

mi1 = mi1

if dumsub-0, numsub = mi2 # Store number of subprograms

toolcount = toolcount + 1 #Index!

if toolcountn <= tooltotal, nexttool = rbuf-4,toolcountn-

else, nexttool = first_tool

 

if numsub-0, n = nsav

 

pcooloff, e

"G0G30P1M5", e

phincoff, e

 

"M1"

" "

 

 

pinit

if numsub-0, " "

"N", t, e

"IF [VATOL EQ ", *t, "] N", *t, *next_tool, nna, e

pblow, e

"T", *t, "M6", e

pblowoff, e

"N", *t, *next_tool, nna, e

ptoolcomm #Tool!

comment, e

spaces=0

if output_z = 1, preadbuf5

if output_z = 1, "-MAX ", *max_depth, "-"

if output_z = 1, "-MIN ", *min_depth, "-"

if tlnxt = 1 & toolcount <- 1, "/T", *next_tool, " -IS THE NEXT TOOL-"

 

 

spaces=spaces_sav

 

if tplnout = one, ptplane

 

startflg = one

nobrk_sav = nobrk

nobrk = one

 

pstock #Stock!

pindex #Index!

last_op_id = op_id

 

peof0 # End of file for tool zero

peof

 

peof # End of file for non-zero tool

if numsub-0, phincoff, e

if numsub-0, "RTS"

if numsub-0, "%"

subout = 0

 

if numsub-0, n = nsav

 

pcooloff, e

"G0G30P1M5"

phincoff, e

pblow, e

if tlnxt = 1 & toolcount <- 1, "/M6"

if tlnxt = 0 & toolcount <- 1, "T", *first_tool, "M6"

"G0Y9.0"

pblowoff, e

 

mi1 = mi1org

*sgwcs

 

"M2"

if numsub=0, "%"

if numsub-0, " "

if numsub-0, " "

 

mergesub

clearsub

 

-----------------------------------------------------------------------

 

Mick hope this is some help to you.

 

ps.

 

i plan to use mr4-10 to allow you to plugin other values ie F,E,D,L,R,P,Q

no time now with multi seates of X to get up and running.

 

35K Chipper

[Mick]

Thanks for your replies!

 

I need to investigate this further. From what I can tell, our control doesn't recognised the G130/G131, but the Hi2NC is engaged in, as you describe, "fallback mode". The trouble is, it seems to me, that it needs to set for wach machining operation, ie: I might be doing a suface finish contour toolpath, and the settings that work well for that, may not work for a surface finish scallop toolpath, using a different tool/parameters.

I take it there is no "generic" setting that works well for all contouring code (ie no rapids or cycles). If not, it looks like I need to experiement a bit

 

Thanks again for your help. I'll let you know how I get on

[35K chipper]

mick,

the setings for mi8 i use most are as follows:

3 for high speed

7 for general

10 for precision

 

35k chipper

[david]

mick,

 

we have a vertical and horizontal with the U100 control

 

try this in your program

 

G187 F600 E.003

 

this sets max. feed at 600ipm and cut tolerance at .003

 

G186

 

this cancels a G187 command and returns to parameter settings in control

 

 

when I run 3d I manually type this in my program to speed up movements and am still able to hold tolerances. if you go to parameters and set work tolerance from .0001 to .003 you will notice some difference when you interpolate dowel holes.

 

cant explain what super hi-cut option is or does but these commands work for us.

 

good luck,

david

[35K chipper]

mick,

you need to find ought what you have in your control. Hi2-NC G187/G186 or Super Hi-NC G131/G130.

i don't think you can have both in the same control . also do you have linear encoders on these machines? call Okuma with the serial number they can tell you what you have. they are very good with keeping track of what was purchased or what was added.

 

35k chipper

[beej]

Mick,

I have an Okuma with Super Hi NC with dnc-dt and it works great for us. I don't know a lot about it because our Okuma service department set it all up and I haven't had to do a thing to it. I do know that there are 3 settings in the parameters. one for less quality- more speed, one for more quality less speed, and another in between. You might want to consider calling my Okuma guys they are top notch. Hartwig inc in St Louis Mo 314-426-5300 ask for Roger, he's head of service.