okuma osp200m hi-cut feature

[sarver1]

Hey guys new to the forum hear, been a machinist for close to five years now and worked in a job shop that is dominately okuma mills and lathes.

 

Were located in southern Illinois and use master and conversational for our programming, we have been getting alot of work of profiling nest and numerous other parts that are made out of delrin. Im trying to wrap my head around this hi-cut codes (nobody here really goes outside of the box when machining) and im just curious on how exactly it works.

 

I understand it anticipates corners straights and what not to hold tolerance but for roughing i would like to turn it off and have it on for finishing,

 

If someone could explain this to me like im a dummy that would be perfect.

 

 

We have custom post for our Okuma mills, but i didn't really seen any true options for the hi-cut, is this something you have to manually enter into the program or what?

 

I have alot of questions about this and would definately appreciate any help I could get from you masters on here!

 

Thanks again,

Cody

[Mr. M]

We have our post set to use "misc integers" for the high cut settings and don't need to hand edit them. Once I get on a computer I can type up how it all works for ya

[sarver1]

awesome thanks!

[Greg Williams]

This may be a little over the top but hey it works for me

 

1st Define the strings

hsmset :1 #High speed cutting 0=off 1=Hicut pro G131 2=Supernurbs G131 3=HiCut G187

 

hsmon : 0 # G131 flag

 

Then in the tool change blocks

if opcode$ = three | opcode$ = 16, e$ #GHW

else,

[

if hsmset = 1, #High-cut pro

[

if mi8$ = one & mi7$ = one, result = mprint(shspmill)

if mi7$ | mi8$ > 0 & cas_off, n$, "M510", e$

if mi7$ = one, n$, "G131", "J2", [if mr1$ <> 0, *mr1$, else, "E0.025"], "F20000", "(HICUT PRO ROUGHING)", e$

if mi8$ = one, n$, "G131", "J1", "E0.01", "F20000", "(HICUT PRO FINISHING)", e$

if mi7$ | mi8$, hsmon = 1

]

if hsmset = 2, #Super Nurbs

[

if mi8$ = one & mi7$ = one, result = mprint(shspmill)

if mi7$ | mi8$ > 0 & cas_off, n$, "M510", e$

if mi7$ = one, n$,"G131", "J0", [if mr1$ <> 0, *mr1$, else, "E0.025"], "D0.010", "I0", "F20000", "(SUPERNURBS ROUGHING)", e$

if mi8$ = one, n$,"G131 J0 E0.01 D0.005 I0 F20000", "(SUPERNURBS FINISHING)", e$

if mi7$ | mi8$, hsmon = 1

]

if hsmset = 3, #High-Cut

[

if mi8$ = one & mi7$ = one, result = mprint(shspmill)

if mi7$ | mi8$ > 0 & cas_off, n$, "M510", e$

if mi7$ = one, n$,"G187", [if mr1$ <> 0, *mr1$, else, "E0.025"], "F20000", "(HICUT ROUGHING)", e$

if mi8$ = one, n$,"G187 E0.01 F20000", "(HICUT FINISHING)", e$

if mi7$ | mi8$, hsmon = 1

]

]

 

 

And then in the retract blocks

if hsmon = 1,

[

if hsmset = 3, n$, "G186 (HICUT OFF)", e$

else, n$, "G130 (SUPER NURBS OFF)", e$

if cas_off, n$, "M511", e$

hsmon = 0

]

 

 

also in the error messages

shspmill : "ERROR-CHECK HIGH SPEED MILLING PARAMETERS"

 

add this to the MI numbers

 

7. "Super Nurbs High Speed [1 = ON]"//1

8. "Super Nurbs Ultra high Accuracy [1 = ON]"

 

Hope this helps

[Mr. M]

Here shows how our posts are setup, Gregs actually show ya something useful (like how to setup your post )

 

How Hi-Cut work is it keeps the feed-rate as high is it can based on the geometry and while keeping within the tolerance setting.

[sarver1]

so the post needs to be edited to be able to control the hi-cut then?

 

i dont fully comprehend the misc integers and reels as nobody here has ever touched them so when being trained i was never explained to how they work.

 

sorry like i said im basically clueless when it comes to this haha

[sarver1]

ill take a screenshot to show you guys what i see in this tab

 

(well i hope this works, first attempt of uploading a picture here)

 

http://i1294.photobucket.com/albums/b611/Cody_Sarver/Untitled_zps3ce6aeff.png

[Colin Gilchrist]

Hello Sarver,

 

I'd recommend talking with your Reseller to inquire about the OSP_P200M post. There is a post available from CNC Software to your Reseller (They have the option to charge for the post, so it might not be "free"). This post is included in the "Mastercam X7 Post Installation" program.

 

The OSP_P200M post is already configured to output code for either Hi-Cut Pro, or Super NURBS (set by a switch in the post).

 

Hope that helps,

 

Colin

[sarver1]

does anyone know how to stream live video feed to my okuma. im really excited about britians soccer game and my mom wont let me watch

[Mr. M]

While that can be done, I don't recommend it. There are reasons your mother doesn't want you watching Britain play soccer.

[sarver1]

haha sorry i obviously left this open and some people here cant help but write stupid xxxx.

 

I will look into who our reseller is and see if we can come up with this post

[Mr. M]

[sarver1]

..

[sarver1]

well i did notice today our custom post, does turn super nuerbs on and off when profiling it still seems like these machines could be running muchharder while roughing during profiling.

 

Is there a way to see true feed rate on the machine and not just whatever is called out in the program?

 

thanks

[Mr. M]

The "Feed Axis Data" page will show you all of that. Also one of the things with the Okuma open API on the THINC controls is you can make your own custom interfaces. I built this one the other day for a HMC that had all the desired data collected on that page

[jeff]

I just use Manual Entry for my Hi-Cut

 

G187E.003F1000.

 

And when I want to turn it off

 

G186

[Mick]

That is really cool. I would really like to be able to do that sort of thing myself.

 

Got to dig Okuma controls

 

The "Feed Axis Data" page will show you all of that. Also one of the things with the Okuma open API on the THINC controls is you can make your own custom interfaces. I built this one the other day for a HMC that had all the desired data collected on that page

[Mr. M]

We have been doing more and more of it! Once we got the first few applications built it got easier to do. Debugging the apps seems like it takes the longest.

[Mick]

We have been doing more and more of it! Once we got the first few applications built it got easier to do. Debugging the apps seems like it takes the longest.

 

So are you at Hegmans?

 

I was in Charlotte at the Thinc facility about two months ago. What a great place. I had a blast, and learnt a lot. I definitely want to head back there some time!

[Mr. M]

Yes I am, and it is a great facility down there! You can check out all kinds of things in one place

[Mick]

Ah, so you're working with Doug.

 

Yes, I enjoyed being there. Learnt a lot. Oh, and the wings and fried pickle (plus the sweet tea) were great too

[Mr. M]

Well, I work. Doug is there.

 

[YoDoug®]

Well, I work. Doug is there.

 

LOL, That's because I'm "King Nerd". I have minions to do my bidding.

[Mick]

LOL, That's because I'm "King Nerd". I have minions to do my bidding.

 

Note to self. Never become Dougs minion...

 

I've been used enough already... LOL

[mig]

What is M510 /M511 Collision avoidance off/on ?

Thank you