okuma hem/hsm not keeping up with called feed

lowCountryCamo

Stainless

Joined

Jan 1, 2012

Location

Savannah, Georgia, USA

• Aug 24, 2019

• #1

I program for six different Okuma mills with osp200 and osp300 controls. When running high efficient milling paths the machines cannot keep up with a constant say 100 ipm feed. It will achieve those speeds in the field but slows when converting from reposition feed to cut feed. Also when the circles get tight say .5" - .25" rad it slows here also to say 40 ipm. It was worse until I learned about g131 j2 hi pro or nurbs. That did help but still not what a modern machine should do in my opinion. I understand acceleration from stop to go but this seems different to me. I saw this vid on youtube of similar machine keeping high feeds even in tight rads so there must be something I am not doing correctly. I program with Mastercam 2020 and post g01 g02/g03 code. Would only g01 improve?

YouTube

Thanks

Steve Austin

 

B

boosted

Stainless

Joined

Jan 4, 2014

Location

Portland, OR

• Aug 24, 2019

• #2

Are you dealing with hi-cut or supernurbs? Are you setting it appropriately, or just turning it on? Which machine platforms are you dealing with?

I suspect you aren't using the look ahead / shape comp correctly, because my M560V with just the hi-cut does a pretty impressive job until you crank the tolerance way down, or start asking it to move in 3 axis simultaneously.

Once you are certain look ahead is set right, then you can move on to other "tricks" like making sure sharp corners are posted with a fillet, etc... In your demo video, I can pretty much guarantee everything is running with huge tolerance settings. Ever try bumping the E value up to .010 inch? It helps a bunch.

 

D Nelson

Stainless

Joined

Jan 7, 2015

Location

Missouri Ida

• Aug 24, 2019

• #3

Make sure in mastercam you are converting lines to arcs in your tolerance page. When it’s running and studdering do you see any I or j codes or lots of tiny line moves?
Don


Sent from my iPhone using Tapatalk Pro

 

lowCountryCamo

Stainless

Joined

Jan 1, 2012

Location

Savannah, Georgia, USA

• Aug 25, 2019

• #4

I think the tolerance could be set too tight. One machine has the supernurbs option and the others have hicutpro. One machine is a mu6300 ac trunnion. 3 are mu4000 bc trunnions. The other 2 are ma600H HMC. I am converting lines to arcs. Mastercam has micro lift of .01" in z when repositioning. So that would be 3 axis interpolation. Could that cause the slow down? I could change that if needed. Thanks for your help.

 

Nerdlinger

Stainless

Joined

Aug 10, 2013

Location

Chicago, IL

• Aug 25, 2019

• #5

The first time this happened to me it was the arc tolerance set too tight. I bet that’s your scum bag. Good luck!

 

X

XD341

Hot Rolled

Joined

Mar 23, 2011

Location

NY USA

• Aug 25, 2019

• #6

OSP300 is one of the faster controls out there...it's not a volume of code problem, the control is slowing things down on purpose. I suspect tolerance is too tight in the high cut settings.

 

R

rickyt

Aluminum

Joined

Apr 30, 2006

Location

Ga.

• Aug 26, 2019

• #7

Try using G131, it goes like this.

G20
G90 G80 G40 G0
M6 T1
(T1 - 1/4 FLAT ENDMILL - TOOL DIA. - .25)
G15 H1
M11
G131 E.01 F750. (E IS THE PRECSION SETTING, F IS THE MAX FEED RATE)
(THE SMALLER THE E VALUE IS THE TIGHTER THE TOLERANCE BUT SLOW FEED)
G0 G90 X-1.3125 Y.0375 A0.
S6500 M3
G56 H1 Z1. M8
Z.05
G1 Z-1. F50.
G41 D1 X-1.3375 F30.
G3 X-1.375 Y0. I0. J-.0375
X0. Y-1.375 I1.375 J0.
X1.375 Y0. I0. J1.375
X0. Y1.375 I-1.375 J0.
X-1.375 Y0. I0. J-1.375
G1 Y-.01
G3 X-1.3375 Y-.0472 I.0375 J.0003
G1 X-1.3372
G40 X-1.3122 Y-.047
G0 Z1. M9
G130 (CANCELL'S THE HSM MODE)
(MAKE SURE TO CANCELL IT AFTER EACH MILLING OP)
M5
Z30
M30

Hope this helps.

 

Mtndew

Diamond

Joined

Jun 7, 2012

Location

Michigan

• Aug 26, 2019

• #8

What control?
The older Okuma mills have the old school Hi Cut, and it's AWFUL.
The Hi-Cut Pro is insane how good it is.

 

Mtndew

Diamond

Joined

Jun 7, 2012

Location

Michigan

• Aug 26, 2019

• #9

rickyt said:

G130 (CANCELL'S THE HSM MODE)
(MAKE SURE TO CANCELL IT AFTER EACH MILLING OP)
M5
Z30
M30

Hope this helps.

Click to expand...

No need to cancel Hi Cut. Ours is on constantly.

 

B

boosted

Stainless

Joined

Jan 4, 2014

Location

Portland, OR

• Aug 26, 2019

• #10

I think you still need to confirm what the "E" setting is on your code. It's not one-size-fits-all. A value that will give good accuracy while finishing is going to slow it to a crawl when you are roughing.

The microlift probably isn't hurting much. I also run volumill roughing, and don't notice significant slowdown on the lift during repositioning.

 

Mike1974

Diamond

Joined

Nov 5, 2014

Location

Tampa area

• Aug 26, 2019

• #11

lowCountryCamo said:

I think the tolerance could be set too tight. One machine has the supernurbs option and the others have hicutpro. One machine is a mu6300 ac trunnion. 3 are mu4000 bc trunnions. The other 2 are ma600H HMC. I am converting lines to arcs. Mastercam has micro lift of .01" in z when repositioning. So that would be 3 axis interpolation. Could that cause the slow down? I could change that if needed. Thanks for your help.

Click to expand...

Not sure about the newer version on MCX, but in the same place as the microlift is a back feedrate. Make sure that is not defaulted to something slow. I usually set mine to 200-300 IPM, doesn't get near that in the little space I am programming, but it is noticeably faster than the 60-100ipm it is programmed at for cutting. Sorry not Okuma specific, but worth checking your settings in MCX.