Sign in to follow this  
Titanium

Okuma OSP-P300LA (Looking for simple intructions on creating a master tool)

Recommended Posts

Good morning,

I'm not a fan of having to create a "Master Tool" for the LB 3000 EXII MWY. Maybe it's because I've never seen anyone explain it well. Even our trainer was stumbling through it. Does anyone have a detailed, step by step list on how to create one properly?

Thanks.

Share this post


Link to post
Share on other sites
13 minutes ago, Titanium said:

Good morning,

I'm not a fan of having to create a "Master Tool" for the LB 3000 EXII MWY. Maybe it's because I've never seen anyone explain it well. Even our trainer was stumbling through it. Does anyone have a detailed, step by step list on how to create one properly?

Thanks.

What do you mean by "Master tool"

Share this post


Link to post
Share on other sites

That is one things that always puzzled me about the way some people thought the way to use these machines. Does it have a Tool Eye? If so there shouldn't be a need for a Master Tool. Should be able to set a position relative from the Face of the Chuck to the Face of a Turret. Once you have established that then you should be able to work from those 2 places to do what ever you need with what ever tool and jaws/fixture and call it a day. Multus Machine don't require this and ask them to help you set the machine up like a Multus.

 

Share this post


Link to post
Share on other sites
28 minutes ago, YoDoug® said:

What do you mean by "Master tool"

The guy the dealer sent out said that you have to create a master tool. Basically, he wants us to take our finish turning tool and calibrate it so that the z will be zero when touched off. All tools touched off after that will reference off of that tool.

Share this post


Link to post
Share on other sites
12 minutes ago, 5th Axis CGI said:

That is one things that always puzzled me about the way some people thought the way to use these machines. Does it have a Tool Eye? If so there shouldn't be a need for a Master Tool. Should be able to set a position relative from the Face of the Chuck to the Face of a Turret. Once you have established that then you should be able to work from those 2 places to do what ever you need with what ever tool and jaws/fixture and call it a day. Multus Machine don't require this and ask them to help you set the machine up like a Multus.

 

Exactly. It's a new machine and I want to set it up so that it's fairly easy to run. The "master tool" seems weird. Yes, it has a tool eye. On the subspindle side, I can't use the tool eye because of the length of the tools.

Share this post


Link to post
Share on other sites
1 minute ago, Titanium said:

The guy the dealer sent out said that you have to create a master tool. Basically, he wants us to take our finish turning tool and calibrate it so that the z will be zero when touched off. All tools touched off after that will reference off of that tool.

Yes what I learned when running Okuma's 25 years ago. Tell them to bring in a better Application Engineer that understand modern manufacturing methods and practices.

  • Like 2

Share this post


Link to post
Share on other sites
2 minutes ago, 5th Axis CGI said:

Yes what I learned when running Okuma's 25 years ago. Tell them to bring in a better Application Engineer that understand modern manufacturing methods and practices.

I would like that but their applications guy is the only one in the area and he hasn't even used a sub spindle Okuma before.

  • Haha 1

Share this post


Link to post
Share on other sites

If set up properly you don't need to use a master tool. We have our LT3000 set up so we can use the numbers from our CAM software for offsets. We load the program and hit go. 

Essentially the machines zero is the face of the spindle. Knowing that you can calc the chucks Z position, then add you part stick out. We can measure it with a caliper if necessary, type in the number and start machining. The sub spindle machine Z is the same, from the face of the spindle. The W zero is spindle face touching spindle face. The W value you will use is the distance between spindle faces when you are at the point you want to be W=0 in your program. 

As for the Sub-spindle tools on the LB3000, those have to be touched off manually. Once you know the Z machine position of the chuck face it is pretty easy to touch tool off that. 

  • Like 1

Share this post


Link to post
Share on other sites
21 minutes ago, YoDoug® said:

If set up properly you don't need to use a master tool. We have our LT3000 set up so we can use the numbers from our CAM software for offsets. We load the program and hit go. 

Essentially the machines zero is the face of the spindle. Knowing that you can calc the chucks Z position, then add you part stick out. We can measure it with a caliper if necessary, type in the number and start machining. The sub spindle machine Z is the same, from the face of the spindle. The W zero is spindle face touching spindle face. The W value you will use is the distance between spindle faces when you are at the point you want to be W=0 in your program. 

As for the Sub-spindle tools on the LB3000, those have to be touched off manually. Once you know the Z machine position of the chuck face it is pretty easy to touch tool off that. 

I agree 100%. :)

Share this post


Link to post
Share on other sites

After thinking about this a little more, it sounds like the AE is not familiar with the use of the Mid-auto manual function. Where this comes into play is touching off for a zero offset. When you call a tool in MDI, the tool offset is active, but if you put the machine into manual/handle, it cancels the offset. Then if you try to touch of a part and CAL the Z, the tool offset is not accounted for.

Instead, after calling the the tool you want to use to touch off with in MDI, turn on Mid-Auto Manual, leaving the control in MDI. You can handle the tool into position and CAL Z with the tool offset being accounted for.  

  • Like 5

Share this post


Link to post
Share on other sites
2 minutes ago, YoDoug® said:

After thinking about this a little more, it sounds like the AE is not familiar with the use of the Mid-auto manual function. Where this comes into play is touching off for a zero offset. When you call a tool in MDI, the tool offset is active, but if you put the machine into manual/handle, it cancels the offset. Then if you try to touch of a part and CAL the Z, the tool offset is not accounted for.

Instead, after calling the the tool you want to use to touch off with in MDI, turn on Mid-Auto Manual, leaving the control in MDI. You can handle the tool into position and CAL Z with the tool offset being accounted for.  

Great advice Doug, thanks! I didn't know that Mid-Auto Manual would work for that. That will be helpful.

Share this post


Link to post
Share on other sites

Hah, I've ran across this before...  Disclaimer, I'm not a Okuma guy, so this might be a bit off base with their meaning, but where I've seen it before is as the reference for your tool height offset table.  As others mentioned, it's an old school thought process.

To describe what it's doing, think of  an old VMC machine where the spindle doesn't have enough Z to touch the table/tool setter.   In that case, you need to have a "reference tool" (master tool, etc) that is long enough that you can get down to the table/tool setter. You would set that as 0 height.

Every other tool you put into the machine has as length offset in the library that's +- that reference tool.  For example, you chose an endmill in a certain holder for your reference tool.   Then, the next tool you load is .75" shorter than that one.   When you set that tool up, the height offset value in the tool table is -.75" (The Z had to move down an additional .75" more than the reference tool). 

There are many problems with this, but the few obvious ones:  There's no way to look at your tool library and see if the H value is anywhere near correct visually, and if anything ever happens to your reference measurement (accidentally reset, machine re-levelled, etc.) you have to remeasure every tool in your library.

As mentioned above, always measure off of an immovable feature such as the spindle face.   Use a gage block to get enough height to get to the tool setter if you have to!   Then, all of the tools in your library will have a real H# from the spindle face to the tip, so you can quickly look at it and say "yep, that tool is about 7.5" long" and you can redo your reference quickly and repeatably if necessary without redoing your whole tool library.

Share this post


Link to post
Share on other sites

Back in the dim dark days of Okuma, before tool setters on the machine, this method was the standard practice. This was well before the days of PC's and Mid Auto Manual as well (I'm talking the OSP2200 control and paper tape days).

But nowadays, there is definitely no need for that, especially on a control as powerful as the P300.

  • Like 1

Share this post


Link to post
Share on other sites

Thanks a lot for the pdf! I just saw it now and it's extremely informative. I sure wish our local AE had information like that!

Much appreciated!

  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us