Compiling Files

[Gherkinman]

The team 116 CAD is nearing completion and we are going to need all our files in one place so we can upload. Naturally we've been managing our data throughout the season, so we have very little work to do.
However, we have use bolted connections in our assembly with the Design Accelerator tool; the nuts and bolts are a part of the ANSI library file installed with inventor 2008 and as such, are not located in our main directroy. I know the most copies of Inventor 2008 will have the ANSI library installed by default, but the file pathnames won't match up and inventor will generat those annoying missing part errors. So is there a way to compile all the parts in one neat little package like with power point presentations? Or do I not need to worry about this at all since they are library files?

[Dan Zollman]

When you use a part from the Content Center, it automatically saves that part--unless you change the defaults--in a special Content Center folder. This way, when you open the assembly, Inventor can open and display that part file quickly instead of going through the Content Center/Design Accelerator every time. This means that if you move your project folder to a different computer, Inventor will not be able to find those parts (because it doesn't have that Content Center folder) and it'll give you those errors. What you need to do is find that Content Center folder and move those files to some place within your project folder.

This folder is usually located in the user Inventor directory where you save your project files. On my computer (default installation setup for R11), the Content Center folder is:
C:\Documents and Settings\Daniel Zollman\My Documents\Inventor\Content Center Files\R11
Move those files to your project folder. You will then have to redefine the file references within your assembly, either with Design Assistant, or by going into the assembly file and Replacing each bolt manually.

There's one more way to store Content Center files inside your project folder. Assuming that you're working with a project (.ipj file), you can:
1. Go to the Projects window (File>Projects)
2. Select your project on the list
3. Click the plus sign next to Folder Options
4. Specify a new path for "Content Center Files" to something inside your project folder
That way, the next time you add a part using the Content Center or Design Accelerator, it will automatically save the part in that folder. When you move the project folder, the parts will move with it.

Sorry if my instructions are incorrect for Inventor 2008--I'm still using R11, but I can't imagine that Inventor 2008 is significantly different.

[Gherkinman]

Oh, wow, inventor makes it easy. I'm glad I don't have to find all those bolts myself. Thanks for your assistance : )

[pmax]

Also consider using the "Pack and Go" utility, ensuring to review the library options in the left of the dialog.

[grim]

Chris, to put the whole enchilada in one place your option is pack-n-go. Right click the upper most level drawing in Windows Explorer and the pack-n-go option is available. By selecting the drawing instead of the assembly you will pull all the references along with it. This will include content center files as you wish.

Good luck.