[CNC-Hammer]

Hi guys,

can the tool shape definitions be output to a program so that they are loaded with the program everytime?

MB56-VA OSP E10M & OSP P200M

[Superman]

can the tool shape definitions be output to a program so that they are loaded with the program everytime?

When you say output, do you mean from IGF ?

If yes, then after running the IGF graphics when "posting" it to get code, when it asks for a filename, add to the end ;U to have it insert the graphic info ( stock and tool data ) into the NC-file

[broby]

However... when outputting the "Toolshape" using the ;U option, IGF will write the shape of the tool to the tool "Number" used when programming.
So... if you change the tool number later, you need to update the relevant code in the shape definition.
Brian.

[CNC-Hammer]

When you say output, do you mean from IGF ?

I was actually referring to what is in the tool page about four items down. But this is good to know.

[CNC-Hammer]

However... when outputting the "Toolshape" using the ;U option, IGF will write the shape of the tool to the tool "Number" used when programming.
So... if you change the tool number later, you need to update the relevant code in the shape definition.
Brian.

Thanks Broby, but thankfully we tend not to change tool positions too often.

[Superman]

I'm assuming you have the PDF manuals for the OSP P200-M

go to the "Special Functions Manual #1"

Section 1-5 is about tool shape in the machine
Section 1-6 is about having the shape ( stock and tool ) in the program

section 1-6-13 is specifically about the tool
each tool would have these 4 lines in the NC-code after your header before the program proper to enable the graphics
VTLTD [I] Tool diameter 0.000 ≤ * ≤ 9999.999
VTLNA [I] Tool nose angle 0.000 ≤ * ≤ 180.000
VTLND [I] Tool edge diameter 0.000 ≤ * ≤ 9999.999
VTLIN [I] Tool classification code number 1 ≤ * ≤ 7

ie T12= 10mm ENDMILL
VTLTD[12]=10.0
VTLNA[12]=180.0
VTLND[12]=0.0
VTLIN[12]=6

I am not aware of any method of saving the tool graphics data to a file

Steve

PS looks like a "down-under" only thread

[CNC-Hammer]

Funnily enough I ran a program today with all the information at the beginning and I just knew that was the tooling data we have been discussing.

Thanks guys!

[broby]

I was actually referring to what is in the tool page about four items down. But this is good to know.

Rather difficult to read the screen on a machine that you do not have...
or a controller that you do not have...
so a description of "four items down" is rather lacking to say the least!

Oh I forgot... have you seen my dog? it went missing last week...
It is about this high, hold hand above floor to correct height
is black and white, with a patch over one eye.
Missing one leg etc...
goes by the name of "Lucky"
LOL
Know what I mean?

Cheers (and don't forget this was said with tongue firmly planted in cheek!)
Brian.

[Superman]

Hey Brian,
You need to water that cordial down a little more.

Or

Go back to the doctor, he needs to increase the dosage levels on your medication

LOL(chair)

[broby]

Whaaat?
Nothing wrong with Raspberry cordial full strength is there?
yeeeeeee haaaaaa!

PS Dog still missing

[Shotout]

Does anyone know if it would be possible to get a cam program, MasterCam specifically, to output the animation data for an OSP200 control? I remember vericut use to do this as an add on for their software and was wondering if the same was possible for OSP.

[Superman]

Here we are, a wanna-be Aussie :cheers:

Yes it can be done, they already do it for "Predator" and "Metacut", so why not for IGF
It would not be that hard to output those variables after a header and combining it with the tool list

[OkumaWiz]

Yes you can get your cam system to output the shape to your programs. I currently have GibbsCam calculate the stock size and output both the stock and the check shape correctly for me on our lathes. The tool data is possible too if your cam system can handle it. There is a whole section on system variables that can prove pretty useful.

I personally like to save all of the fixture offsets to the program as well. (VZOFX[1]=1.237 VZOFY[1]=0 VZOFZ[1]=3.57) You can put multiple parameters on one line as long as there is a space between them.

By the way, if you use the Data PIP function, you can save the tool information to a file that is separate from your program as well. The nice thing about that is that it can save all of the parameters as well so a complete setup can be saved easily.

Welcome to variable heaven...

[CNC-Hammer]

Cheers (and don't forget this was said with tongue firmly planted in cheek!)Brian.

Dude, it's easy to forget that other members don't have the same machine/contol.

I was spewing when I read your post!

[CNC-Hammer]

By the way, if you use the Data PIP function, you can save the tool information to a file that is separate from your program as well. The nice thing about that is that it can save all of the parameters as well so a complete setup can be saved easily.

Welcome to variable heaven...

Is the Data PIP a function of Gibbs or Okuma?

[broby]

Is the Data PIP a function of Gibbs or Okuma?

Data PIP on the Machine!

[broby]

Dude, it's easy to forget that other members don't have the same machine/contol.

I was spewing when I read your post!

LOL, do not stress about that! I would imagine that we have all done that at some stage or other.

Cheers
Brian.

[CNC-Hammer]

Can you elaborate please Broby, I'm relatively new to Okuma.

[Shotout]

@ Superman, by far not the worst thing a man could be called

@Whiz
I assumed Gibbs would do it considering their partnership with Thinc but wasn't sure about other packages. Our ME Lead was going to play around with a post to get Master Cam to output the variables for the stock, useful with extrusions more so than billet stock which is a simple format. I can't figure out how to do it myself though. We had talked over defining the tombstones and vises with an odd offset that wouldn't be used for the new horizontal. Something we can cut a paste into our posted code. It seems to be easier to get a setup machinist to do a dry run on a program when they have pretty graphics to look at plus a safety factor as well. As to tool data isn't that a pretty big set of commands for every tool? Lots of block data to define them etc?

On a HMC the variables to set work offsets are pretty nice. Learned them on the first OSP control I used running castings, all programs ran as subs and a main defined work offsets and took care of pallet swapping etc. Be handy on a VMC if every thing was mounted to a sub plate with set positions too.

[Superman]

Been thinking of how to incorporate it in Mastercam

Stock would have to be analysed and only output if round or rectangular, Solids, holes etc would have to be ignored or converted to min/max values or along those lines

Tool Data would be output with the tool list at the header
I have modified a post to output actual tool sizes into the list to give better, more informed info and eliminate typing errors. But have yet to add the Okuma data ( it is planned )

ie

(*** Tool List ***)
()
(T1=8mm HSS Spotdrill_Point Dia=1.0_ blah,Tool Angle=90_Tool Out=35 )
( Build=HSK100_ER32....)
( Tool Spec=...) 
VTLTD[1]=8.0 VTLNA[1]=90.0 VTLND[1]=1.0 VTLIN[1]=2 ( 2 may be wrong )
()
(T12=10mm CBD Endmill, blah, blah , blah, blah_Tool Out=30 )
( Build=HSK100_SRKIN 10 * 110 )
( Tool Spec=...) 
VTLTD[12]=10.0 VTLNA[12]=180.0 VTLND[12]=0.0 VTLIN[12]=6
()