I have assemblies that include assembly created parts. Every part contains links to the asembly I need to maintain.
How do I copy the assembly (and rename it) while maintaining the links?
Revision manager: Breaks links
Save file as (inside ST6): Breaks links
Best solution so far: Copy the Assembly and Parts from one directory to another using windows. Links are maintained until the assembly file is renamed....that kills the links. Because of this, I must assume that the assembly created part files point to the assembly file name and search starting with the same directory. If this is as good as it gets, then I will end up with 100's of files that have the same name and forces me to track files with directory names.
Have any figured out how to copy and rename an assembly that maintains links?
Solved! Go to Solution.
I generally use resision manager to copy and rename assemblies with links, usually with reasonable success. What is it you are trying to achieve? for example, do you want the new assembly model to use the existing parts that were created in place with links staying with existing assembly from which they were created. Or have a new assembly with new parts all linked only to the new assembly.
Let me know what you are trying to achieve and I will see it that works with my workflow.
My goal is:
To make a copy of a design so that it may be modified seporatly from the origional.
The design is a collection of files
The drafting file
The assembly file
The assembly driven parts of the assembly
If this were AutoCAD, it would be as simple as "Save as"
But since there are multiple files and links between the assembly and parts. The "copy" process is not intuitive.
Also the copied part files don't change name. But the assembly and Drafting file do change names.
The best way to do this is to Open the DRAFT file that contains all the Assemblies and parts in Revision Manager. Then use Copy and save them ALL to a new Folder (path).
This of course only works if you have 1 Draft file (even with multiple pages) for an Assembly. But it will capture all the Part and Assembly Files files shown in the Draft on all pages.
As discussed in another thread, many folks have numerous pages in their Draft files representing a complete project. While other's need to use a "one single Draft page per part" strategy due to using the same part(s) in multiple assemblies, so this probably wouldn't work.
That's what I needed to know. "Only open the last file in the chain with revision manager". Then all the links can come along for the ride, the files stay associated with each other, and break ties to the origional files.
I'm running about 20 to 50 pages of 2D PDF per drafting file
I only have two catagories of files/parts:
Standard parts----used by everything that never move or change, referanced by every assembly
Assembly created parts----sheet metal that is controlled by an assembly. Only belongs to a single assembly.
So a typical Revision Manager process for moving/renaming or copying complete structures would be:
Thank you. Respectfully, I disagree.
In general, I want to copy files, verify links, rename file, and verify seperation from origional files before I ever start modifying anything.
Also, I need to copy all file starting with the drafting file to maintain links between the drafting, assembly and parts all together.
I'm running about 50 links from parts to assembly, and another 50 from assembly to drafting.
It takes me about a day to create a set of parts, assembly and drafting files.
Im just about to add about another 50 spreadsheet links to all these file to overcome the shortcommings of the packaged "bend tables"
I need to ask something. When you say "where used" What command are you talking about?
Is this something in the revision manager or the graphic editing/modeling window or the part tree?
"Where used" is part of revision manager, found under the "tools" tab.
I have found that on large assemblies with many links it is usefull to open the high level assembly and use "Inter-Part Manager" to check for issues with links, image attached.