To okuma gurus

[mig]

Hi ,

We running Okuma VMC MC –v4020 . Control OSP –e100l

Super HI-NC control .

Machining mode – Standard.

If geometry spline instead of arc surface finish look like kind of “diamond “.

I guess this is wrong set up of ” reconstr shape” and filters .

Somebody has this problem? How it was solved?

 

Thank you in advance

[kinglouie V]

splines suck. Try edit/simplify

 

are you using "long word" format for your programs?

[Colin Gilchrist]

mig,

 

Are you Contouring the spline and creating g-code, then the g-code give you facets? Or are you creating/importing the spline into the control and programming it in there?

 

If you are creating toolpaths, you need to watch your linerization tolerance, and use your filter settings to generate arcs.

 

When Mastercam contours a spline with no filter enabled, it will always linerize the spline and create point-to-point output.

 

On some controls, when you generate a toolpath, the control actually prefers lots of very small point-to-point moves and because the controller can apply its own acceleration and deceleration parameters to the calculated path...

 

For this to happen you would need to set your linerization tolerance to .0001 or smaller.

 

What is your control's resolution? is it .0001, or does it go smaller. Some controllers these days have encoders that go down to the millionths... .000001

 

Your fix might be as simple as turning on the toolpath filter, set the tolerance to .001, and turn on "create arcs in X,Y".

 

HTH,

[Greg Williams]

Mig,

 

I think you need some different settings below are metric

 

G131 J0 E=0.03 D=0.01 I0 F10000. (SUPER NURBS ON)

[mig]

Hi everybody ,

Thank you for response

In ver 9 was two ways to convert spline to arc :

"CONV to ARC" and :Break "spl to arc" .If one not working other does . In X "simplify" not always help.

I used filter in Mastercam , not always help to .

Also when i machine surfaces which represent arc with relatively big dia i have same (facets)diamond effect .

I guess setting in control an issue . Now it reconstruct shape to precisely or so .

[mchin-pilot]

Hello,

 

Your Nurbs setting in Okuma entirely depend upon the distribution of points in your CAM system. You first decide what the shape of part is that you are machining.( is it gently curved or jerky conners or mix).

 

Having filters on is not a solution, you need to output points. Before you post your TP , watch the min/max distance among the points in that particular TP and set you Min Max Block length ( L , R) in nurbs control accordingly. and have the shape reconsctruction mode to High ( I 2) for gently curved surfaces and Low (I 0) on Jerky surfaces.

 

If what you said you are machining some diamond type surfaces keep machining mode to High Quality(J 0)

 

If its patchy mold work, then the nurbs filter come in play (K,P,Q)Otherwise keep it off.

 

You'll figure out.

 

Play!