Welcome to the forum. Would it work for you to have a note in the title block that's linked to the drawing file name (instead of or in addition to the project number) and page number?
I have linked the title to the file name and the sub title to the sheet name already. Here is how the we would numbered our drawing when we used autocad.
DWG-"project number"-"drawing number" which looks like this
which is fine when we worked with one file but when we start to add more drawing files to the project, the numbering was getting hard to follow and we would end up with duplicate drawing numbers
Since I will be adding the project number directly to the drawing, I don't think it is necessary to also include it in the drawing number.
I am not sure what is the most efficient way to number drawing automatically.
Kevin, if you want to automatically generate drawing numbers you'll either need to have someone do some custom programming or you'll need to get a PDM system with this kind of capability.
With respect to generating a unique number for each sheet of a drawing: I'm inferring from your question that you want to make a SolidWorks drawing into a plan book with multiple components detailed therein. I have two cautionary statements for you. First, by this method, you lose individual revision control over your components. Put another way, changing a single component detail would mean giving the designer access to all of them-and that's not good document management.
Second, SolidWorks really bogs down and gets unweildy when you have more than a dozen sheets in a drawing. In general, it's better to have a one-to-one relationship between model files and drawings.
Thank you for your answer,
I understand that it is better to have a file for each part and then use sheets if more drawing are required for this particullar part.
What if I have an assembly with sub-assembly? I attached an example which was my first solidworks project and I did everything manually and it took a long time. where the final assembly was one file with part details on different sheet. Then each sub assembly was on a different file with the parts detailed on a sheet of its assembly. Any tip on how you would improve the numbering on this project?
The answer to any file naming/numbering/organizational system is always, look to your existing document control policies. This is your ISO9001 and TS16949 stuff.
General guidelines start with the maxim: If you have a part number for it, you should hvae a file for it. The unit of organization is usually the revision-controlled document. A revision controlled document can be edited in it's entirety by a change-order without your having to touch any part number not in the scope of the change order. That means if you make a family different sized parts one part number, than a change order to that part number means the change-order applies to all sizes (or dash numbers) in that family. If your organization uses flattened assembly trees, then in a nut shet, your subassemblies are documented in your top-level assembly drawing. Now, you can have subassemblies as seperate files (I avoid virtual subassemblies in most circumstances) from the main assembly, but you can't revise them seperately. You can refer to the subassembly with a dash-number in your parent assembly BOM and you can create a sheet to detail just that dash number (which sounds similar to what you're doing) but you can't revise that dash number in an activity seperate from its parent assembly. What this usually means is that if you have a subassembly that's used in more than one top-level assembly, or you stock it in inventory, you need to pull a new part number for it.
There isn't in SolidWorks the functionality to name and number sheets based on subassemblies, but you can link title-block and note text to subassembly properties or assembly configuration properties.
ONe solidworks assembly/part files = one drawing, no questions asked. If you have a main assembly, it gets a drawing. If you have a sub assembly with 30 components in it, it gets a drawing. If you have a sub assembly with 2 components in it, it gets a drawing.
Remember, if it made your job easier to make a sub assembly in solidworks, it will make your shop's job easier when it comes time to understand it.
With that said, there are a few 'rules' to follow when doing so:
Assemblies and sub-assemblies should 'bolt together' or 'weld together' or 'glue together'. What this means: don't make a sub- assembly of two components that have nothing in common except for the air between them...
keep your assemblies small. If your feature manager gets long enough that you have to scroll when it is collapsed, you are getting too big....
put some thought into your assemblies before you start!
As far as numbering/naming your files: do yourself a big favor and name your files (assembly/part and drawing) with the number you want to show up on your drawing. If you want your drawing to be something like DD14056-520-240a then name your part/assembly and drawing that. This gains you a few things:
you can easily find the model/drawing in your electronic storage based on the number on the drawing (think about what happens when the shop comes in and asks questions)
If your drawings and model/assembly have the same name you can right click on a component and choose 'open drawing'
Thank you for all of your answers,
After reading your tips I think the best way would be to name the file the same as the drawing number that I want.
Then link the fille name property to the drawing number so that I know all the drawing numbers of one project folder.
Now if I have a new drawing I just follow the sequence in that folder.
as Jason said, if I want to know what is in the drawing I can just open it.