Save As Part Replace in Assembly

[tcarson]

I have a designer working on some concepts, he is working file based not though PDM (smarteam). Here is an example of our problem... We have an assembly open with 3 parts. I have the assembly and all the parts open. I want to make a change in part 2 and save as a new part. I go to part 2 and do a save as and rename to part 4, make my changes and save. The part 2 in the assembly has changed to part 4. I want it to stay as part 2. How do I make a new part and leave the original part as is and not replace any used in assemblies.

thanks

 

[solid7]

A good way to do this, is to do File -> "make new from," and save the resultant file immediately in a new directory. (or the same directory, if it doesn't use the same file name)

Be advised - the parts that you want to "make new from" cannot be open in a current session. You must close all detail parts, and the assembly in order to make the new file. (at least in R15 - I thought that it worked earlier, but I might be mistaken)

This will avoid any replacements.





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[tcarson]

thanks for the help, I have File -> New From, I tried this and it does work if I do not have the part or the assembly using it open. But so does opening it and using save as, if I don't have any instances open. I was hoping to find a way that I didn't have to close all my windows and then save and then reopen all my windows. I have several subs and large assemblies and it takes more time to back out and then reopen every time I need to save a new instance.

Again thanks for the help.

 

[catiajim]

Another method is to Copy the first part, Paste Special back into the assembly, and chose Break Link. This will create a new version of the part (same as New From) in your assembly. You can then make the changes that you want, and save it (use Save Management and Save As). If you don't want it in your assembly any more, just delete it from the Product, or don't save the Product.

 

[Akesson]

To avoid the part to be replaced in the assembly it's used if (the assembly is opened) check the "Save as new document" box in the "Save As" dialog window.

By using this option you get the same result (an independent copy of a part) as "New From" without having to close the part/assembly first.

/Akesson

 

[Akesson]

"Save As" can be dangerous to use.
Catia V5 recognize a part by its name and identifier (UUID).
With "Save As" the new part only gets a new name and the UUID remains the same. This means that following case/problem can happen.

You have an assembly A which contains Part 1. You make a copy of Part 1 using "Save As" (without checking "Save as new document") and rename it to Part 2. Part 2 is assembled in to assembly A. In the context of the assembly which already contains Part 1, Part 2 with the same UUID as Part 1 could be read by Catia as Part 1. This gives you an assembly with two Part 1. So be careful with "Save As". I see "Save As" as a "Rename" (compare other windows programs) not a copy function. Use "New from", "Send To/Directory" or "Save As new document" to create independent parts/products.

Anyone else with more information about this issue?

/Akesson

 

[tcarson]

thanks for the help, I do not have a "Save as new document" checkbox. It is just the standard windows save setup. I am on V5 R13.

Catiajim, your method did work on a quick trial. Thanks again for the help.

 

[Akesson]

I have seen users with the same problem as you that the checkbox is disabled. I don't know why.
Maybe someone out there does?

But try this...

In tools options /General/Document/Linked Document Localization Deactivate all except "Folder of the pointing documnet" and "Relative folder" and sort them in the same order.