Help with creating new parts from existing assembly components... 1

[closer9]

Sorry, but I'm just getting frustrated here...

I have an assembly (product) we'll just call Assembly. This assembly is made of components 1, 2 & 3. Now, I want to create a new part called 4, (slightly modified version of 3)and bring it into the assembly. So, I open Save Management and use "Save As" to save part number 3 as part number 4 (so that I keep my link to the drawing). Now, I have both part number 3 and 4 in the correct folder, but all instances of part number 3 have now been changed to part number 4.

How, do I "Save As" without changing existing assembly components, or losing links to the drawing?

thanks!

 

[MarkAF]

The best thing to do is a different function called "New From." This can create new copies of files, including whole structures of parts, assemblies, and drawings.

-Side note: "New From" won't operate on files that are already open in session-

With the Assembly closed, and say part 3 closed, go to File > New From. In the dialog box, browse to the drawing file. When you select the drawing, Catia will present you with a window that gives the option to create both part and drawing and give them new file names. When you've done this, you will have a new pair of part and drawing that are correctly linked.

At this time, all the internal information of the new part 4 will be identical to part 3, so be sure to update the part number field before inserting part 4 into your assembly.

Beyond that, check the help docs for that function.

Cheers,
Mark

 

[jackk]

I like Mark's suggestion.

But I was thinking about another way to resolve your problem. When you used SAVE MANAGEMENT, you saved and renamed Part3 as Part4. The assembly now shows the new name Part4.

All you have to do is insert the old Part3 back into the assembly. (ending up with components 1, 2, 4, and 3)

Unfortunatly, Drawing3 is now linked to Part4. Mark's method is the best method.

 

[closer9]

I will give that a try Mark. I just think it sucks that I have to close everything I'm working on to save as. That's similar to what a co-worker suggested, though. He said to just close everything, open part 3 and drawing, and save as through save management. Then re-open my assembly and bring 4 in once modified.

Jack, I've been using your method. Save part 4 then replace the "old" instance of 4 with 3. Not a terrible way of doing it, especially since I don't have to get out of my assembly, but when I have several instances of 3 already in the model, it is bothersome.

thanks guys...

 

[ferdo]

I saw this thread before but I didn't realize that there is also another way to do it with all parts loaded in CATIA...

You can use Save As but with the option Save As New Document checked (in the lower side of the SAve As Window, hope I remember correctly because I don't have CATIA in front of me). This is equivalent to New From, is creating a new UUID for the new part.

I've done also in the past a macro to change directly in the new CATPart Properties the number of the part (for us is compulsory to have the CATPart number equal to file name), so when you will insert the new CATPart there will be no conflict between CATParts instance names.

In this way, your initial parts instances will not be modified.

Of course, linking to the drawings is another story...

Regards
Fernando