combining files, is it possible

[Bob W.]

I have been looking into the Jergens ball lock fixture system and it brought up a few questions. On the larger subplates you can use two different fixture plates at the same time.

 

Say I have two different parts (one per fixture plate) programmed in seperate MCAM files and I wanted to run them on the mill at the same time. Is it possible to combine the two MCAM files into one program that I can take to the mill if they share all of the same tools?

 

Thanks,

Bob

[Colin Gilchrist]

Bob,

 

The short answer is "sort of".

 

You can not just take two seperate Mastercam files, merge them together, and spit out code. When you merge files together, the toolpaths do not come in. You could do a Merge, then import and regenerate the toolpaths in the new file.

 

The other way you could do it would be to have both parts (parts, fixtures, ect.) programmed in one Mastercam X part file with different Machine Groups (I know that they are on the same machine, but it simplifies things if you use two machine groups in the ops manager). That way if you only wanted to post out one of the programs you could change the NC file name and post it out as a single part program. Then if you wanted the dual fixture program, change the NC file name, do a "Sort" by tool # (BE CAREFUL IF YOU DO THIS) so that each tool runs on both fixtures before being changed.

 

HTH,

 

Colin Gilchrist

The Boeing Company

MR2 and Beta test site

[Bob W.]

It is too bad that it isn't easier. It would be nice to have the ability to run parts A&B, B&C, A&C, etc... and fully utilize the fixture plate with a few quick mouse clicks. I guess it wouldn't be too difficult to cut and past the entire program (with a different work offset) but there would be a lot of redundant tool changes.

 

Thanks,

Bob

[Fig sign]

Yes you can

That`s what I did many times for exAMPLE CONVERTING

3x files into 5sx positioning

Use save/get from library option together with geometry or import NCI (obsolete ,but still working good )

Too busy now .use help for details or wait for a couple of hours for full reply with details .

~~~~~~~~~~~~~~~~

Operations libraries (*.OP9) are collections of toolpath operations that you can create by using the Save to library option in Operations Manager.

You can import these operations, with or without their geometry, into an MC9 file by using the Get from library option in Operations Manager.

You edit operations libraries using Operations Manager in the same way that you edit MC9 or DF9 files. Functions that you cannot perform on operations library are disabled. For example, you cannot import or export operations into or out of an operations library.

 

Each operation in the library can have its own origin, which is accessible through the tool parameters dialog box.

~~~~~~~~~~~~~~~

You can import an NCI file created in Mastercam version 6, 7, 8, or 9 and make a toolpath from the file. The imported NCI file does not contain geometry, tool, or toolpath parameter information and cannot be regenerated or batch processed. You can modify the toolpath using the Toolpath Editor. This function is available in Mastercam Mill and Mastercam Wire.

 

1. Choose Main Menu, Toolpaths, Next menu, Import NCI.

 

2. Select an NCI file and choose Save.

 

3. If any tools in the NCI file do not match tools in your current tool list, you are prompted to add the tools to the list. Choose OK.

 

4. Choose Main Menu, Toolpaths, Operations to open the Operations Manager. A merged NCI toolpath displays in the operation list area.

 

Note: You can also choose Toolpaths, Import NCI from the right-click menu of the Operations Manager.

 

~~~~~~~~~~~~~~~~