Cheating (help make my life easier)

[tim.clancyYYRYC]

Hi, 

I'm working on a few projects at time moment (I'm an in house designer) and many of the parts for projects are the same but in different assembles. 

Is there an easy way to copy the technical drawing dimensions and view etc of a certain part without starting from scratch. While Still having a different title block information (or at least be editable)(still the same part numbers though).

Any advice would save me hours, thanks

[gcoombridge]

You can just copy and paste views between drawing documents and all dimensions will follow... 

[johnsonshiue · Accepted solution]

Hi Tim,

This is not cheating. This is for better productivity. If the components are reused or stemmed from the same files (copied, saved as), you can simply use Replace Model Reference (Drawing -> Manage) to swap in the new model (part to part; assembly to assembly; not part to assembly). The annotation should stay.

If the new model source is totally unrelated to the original model source, some annotation may stay but mostly will need to be recreated.

Many thanks!

[IgorMir · Accepted solution]

In such a case - it would be appropriate to create a folder, which contains all the parts, assemblies and drawings for these parts and assemblies. For example - the parts will have numbers 01-01, 01-02, 01-03 and so on.

Your next project will have index 02-GA, for example. That's a top-level assembly. In there you will have parts 01-01, 01-02, etc, as well as parts 02-01, 02-02 and so on. Parts with 02 index are unique parts for the project 02.
Later on - you will have projects 03, 04... and so on. In there you will too, have files 01-01, 01-02 (which are common for your company) and unique files, pertaining to this particular project (03-01, 03-02, 03-03...)

To control the quantity of the 01-... parts - place the corresponding file (01-01.ipt) into the assembly that part is used in, (03-GA.iam will have the part 01-01.ipt, for example). Copy/paste drawing 01-01.idw into the folder 03. Now open a copy of drawing (01-01.idw) in the folder 03 and place a part list in it from the assembly 03-GA. It will reflect the quantity of the parts 01-01 in the assembly 03-GA. But all other information, pertaining to the part 01-01 will still be relevant on the drawing. 
It all boils down to the file management at the end of the day. What I have described is, effectively - a library of parts and assemblies. Depending on your circumstances - you might keep them all in a Library folder.
In my line of work - I create folder with parts 01-... for every individual client of mine. Since standard parts for his company won't have anything to do with the standard parts for other company. Thus - each and every client will get drawings with 01-... index in the part number. But because the clients are different - there is never a confusion, whom the file belongs to.

Cheers,

Igor.

[SharkDesign]

Have I got this right? You want exactly the same drawing, but with a different titleblock?

Can you not just do a saveas and then change the titleblock and delete any views you don't want?