Okuma OSP3000L Zero Shift

[Mick]

Hi there,

 

Does anyone here have an example Okuma programme utilising the G50 Zero Shift command? I have a local customer having no success with it.

 

I used to run an old LS-N with an OSP3000L control, and I recall running this feature successfully. I thought I still had the example archived, but it appears I dont anymore :/

 

If anyone does, if possible, please email a sample to me, at [email protected]

[chris m]

No help with G50 as we don't use them on our Okumas, and the oldest control I have is 5020L.

 

Does your customer's control support any of the User Task logic functions? If it does, zero shifts are very simple.

 

C

[Tim Simmermon]

Mick,

 

I program using a G50 on one of our lathes. It is an Ikegai with Fanuc 0-T control. I'll email you a copy if it would help.

[DavidB]

Chris,

quote:

---

If it does, zero shifts are very simple.

---

I'd like to see an example Thanks

[chris m]

VZOFZ is Okuma's variable definition of Z zero [VZOFX, VZOFC, the list goes on; you get the idea] so you can shift the machine's perception of Z zero by arithmatically manipulating this.

 

We 'build' Z zero for each job by starting with a known base value [in our case the face of the turret top plate touched off on the face of the spindle] and adding things to it [thickness of the chuck, jaw height, distance from part locating surface to Z zero] to tell the machine where Z zero is located. This allows us to do a lot of things, including using the same TLO for a given tool regardless of where the part is in the machine AND shifting zero to machine multiple parts in one chucking.

 

Our 'zero set' line in the program looks like this:

 

VZOFZ=V182+V185+POCF+V1

 

Where:

V182 is the 'base' number

V185 is the height of the Kitagawa B210 chuck

POCF is a user variable which is the distance from the chuck face to Z zero

V1 is a fudge factor 'global shift' the operator can use if the stock is long / short / etc.

 

A simple Z zero shift of 1/2" would be:

 

VZOFZ=VZOFZ-.500

 

or you could go with:

 

VZOFZ=V182+V185+POCF+V1-.500

 

There are more complicated examples that I use and we can talk about those down the line if you are interested.

 

C

[RACINGCONVERTERS]

I know asking for a post is a bad deal on the forum but could any of you tell me who wrote your okuma 3000 post. I have had my reseller and a local guy look at what i need and they have never got back to me on it. Any help on editing a post would be great also.

 

thanks

matt

[chris m]

I modified the be-jeezus out of the V9 MPLOKUMA post to get what I have now. What post are you using currently? What do you need to output? If it is relatively straightforward we can work it out via email.

 

C

[DavidB]

I wish mastercam X had more than Fanuc posts on the CD

[3rdstring]

David

 

There shoud be a X post CD availabe from your reseller with a MUCH wider seledction.

[DavidB]

Should be or is there?

If there is I will ask for it.Does anyone know if there is a X post CD?

[3rdstring]

Is. I got one from my reseller when I inquired about a dynapath post for X.

[DavidB]

Was there any Okuma Lathe posts,Heid mill posts?

I'll ask for it first thing Monday morning thanks Chuck

[3rdstring]

Mill

Generic Heidenhain TNC 530 3X

Generic Heidenhain TNC ISO 4X

 

 

Lathe

Okuma OSP7000 2X

 

[Mick]

Thanks for the replies guys. It seems the old OSP3000's are a dying breed.

 

If anyone does come across a G50 work shift example, please send it to me

 

The OSP3000 doesn't have User Task, so that option isn't suitable. But thanks for responding.

[Tim Simmermon]

Mick - You have mail.

[RACINGCONVERTERS]

Chris,

 

I have been away a couple days sorry. Right now I use the MC9 Okuma post and modify the program alot. The machine is twin turret but the bottom turret has over .030 runout so i do not use it. In the program I have to recognize both turrets with G14 for the bottom and G13 for the top turret. It can not have any text. The machine needs 4 places past the decimal but can not have a decimal to recognize the deminsions. The machine has 4 gears that go from G41 to G44. I use mostly the higher gears. Any help you could give me would help. PM me if you would like.

 

Thank you very much,

Matt

[chris m]

The gear range is a G code? That's weird... If you know what the RPM range is for each gear it is simple to modify the post's lookup table to post the correct gear. The no decimal place thing is just a format statement selection, so that's easy. The two-turret thing is beyond my post editing skills, I manually paste together my twin-turret stuff, but it doesn't sound like you use the lower turret anyway [why not fix the alignment?].

[chris m]

Format statements are here:

 

# --------------------------------------------------------------------------

# Format statements - n=nonmodal, l=leading, t=trailing, i=inc, d=delta

# --------------------------------------------------------------------------

#Default english/metric position format statements

fs2 1 0.7 0.6 #Decimal, absolute, 7 place, default for initialize ( )

fs2 2 0.4 0.3 #Decimal, absolute, 4/3 place

fs2 3 0.4 0.3d #Decimal, delta, 4/3 place

#Common format statements

fs2 4 1 0 1 0 #Integer, not leading

fs2 5 2 0 2 0l #Integer, force two leading

fs2 6 3 0 3 0l #Integer, force three leading

fs2 7 4 0 4 0l #Integer, force four leading

fs2 9 0.1 0.1 #Decimal, absolute, 1 place

fs2 10 0.2 0.2 #Decimal, absolute, 2 place

fs2 11 0.3 0.3 #Decimal, absolute, 3 place

fs2 12 0.4 0.4 #Decimal, absolute, 4 place

fs2 13 0.5 0.5 #Decimal, absolute, 5 place

fs2 14 0.3 0.3d #Decimal, delta, 3 place

fs2 15 0.2 0.1 #Decimal, absolute, 2/1 place

fs2 16 0 4 0 4t #No decimal, absolute, 4 trailing

#Default english/metric feed format statements

fs2 17 0.2 0.1 #Decimal, absolute, 2/1 place

fs2 18 0.4 0.3 #Decimal, absolute, 4/3 place

fs2 19 0.5 0.4 #Decimal, absolute, 5/4 place

fs2 20 1 0 1 0n #Integer, forced output

fs2 21 6 0 6 0l #Integer, six four leading

 

 

It sounds like you want 16 [no decimal, abs, 4 trailing] for your X,Y,Z,U,V,W values; you might need to screw around a little with I,J,K,F, etc to get what you want. Those values are set here:

 

 

# --------------------------------------------------------------------------

# Toolchange / NC output Variable Formats

# --------------------------------------------------------------------------

fmt T 7 toolno #Tool number

fmt G 4 g_wcs #WCS G address

fmt P 4 p_wcs #WCS P address

fmt S 4 speed #Spindle Speed

fmt M 4 gear #Gear range

fmt S 4 maxss #RPM spindle speed

# --------------------------------------------------------------------------

fmt N 4 n #Sequence number

fmt X 2 x0 #X ZERO position output

fmt X 2 y0 #Y ZERO position output

fmt X 2 z0s #Z ZERO position output

fmt X 2 xabs #X position output

fmt Y 2 yabs #Y position output

fmt Z 2 zabs #Z position output

fmt U 3 xinc #X position output

fmt V 3 yinc #Y position output

fmt W 3 zinc #Z position output

fmt I 3 iout #Arc center description in X

fmt J 3 jout #Arc center description in Y

fmt K 3 kout #Arc center description in Z

fmt L 2 arcrad #Arc Radius

fmt F 18 feed #Feedrate

fmt F 10 dwell #Dwell

fmt M 5 cantext #Default cantext

[chris m]

For the gear range selection you'll need to change this:

 

# --------------------------------------------------------------------------

# Define the gear selection code

flktbl 1 3 #Lookup table definition - table no. - no. entries

40 0 #Low gear range

41 400 #Med gear range

42 2250 #Hi gear range

 

 

to this:

 

 

# --------------------------------------------------------------------------

# Define the gear selection code

flktbl 1 4 #Lookup table definition - table no. - no. entries

41 0 #1st gear range

42 500 #2nd gear range

43 1000 #3rd gear range

44 1500 #4th gear range

 

The RPM stated is where the machine will shift ranges [the bottom of the range for each gear]. Be sure you change the 'number of entries' for the table from 3 to 4 [as I have done in my example] or you'll never get hi gear.

 

You will also need to change the format statement for gear range to post G instead of M, here:

 

fmt M 4 gear #Gear range

 

AND you will need to switch 'usegear' on

[chris m]

**BUMP**

[RACINGCONVERTERS]

Chris,

 

I have made some of the changes, But I have had keep my machines running also so have not got them all done. Thanks for the help. And your right on the gear change being a M I do not know what I was thinking. Sunday I like to take the day off.

 

Thanks,

Matt

[chris m]

Just let me know how you make out. My email address is in my profile so just fire me an email if you get stuck.

 

C

[Mick]

Er, I think that is a typo. The gear ranges on those lathes are M41, M42, M43 and M44.

 

They'd conflict with G41 and G42 if they were G codes.

[chris m]

Mick

 

Matt realized that; he should be all set there

[Mick]

Hehehe... cheers... Its 11:30pm here, and I am real tired... Just spent three days flying the Mastercam flag at a Trade Show.