I use multiple sheet drawings most of the time. I design injection molds, so when I need to provide detailed drawings this can go to a number of sheets. One thing I have done in the past is a combination of what you are talking about. I will keep my assembly drawing as a multi-sheet drawing. (this is vital for the balloons and BOM.) Then when it is time to create the details, I will start a new drawing file. Then-however many sheets I have for the assembly drawing-I leave that many sheets blank in the details drawing. I have a block that I put on each of these that reads:"intentionally blank". My title block has a property for sheet number and this ensures that the correct sheet number will be in the title block without requiring a manual edit. Perhaps a little clunky, but it has been working for me. Not exactly what you are asking, but I don't know the answer to your issue, so am just offering an alternative.
As a general rule I don't use multiple sheets, mainly for two reasons. As you add sheets, the performance goes down. The other resaon is that if for whatever reason that drawing becomes unreadable, all the sheets are gone, not just one. I prefer to not have all my eggs in the same basket.
Now, that being said, the reason to use multiple sheets are to keep everything together and because properties and links work better amongst them.
But what about the file naming issue I listed. We name are tool drawings like let's say T-5432. If I make everything a unique file then I'm not going to be able to use that linked property for the file name, because it will name the same tool the different names I choose; at this time I've diabled that link and just use dumb text in the file to give it the same name on all sheets.
Thks again for all input.
rob_d (2009 sp4)
Well, no one says you have to use the properties values in the model on the drawing. A lot of people like to do this, but I prefer not to myself due to several issues, including the one you mentioned. I'm used to an environment that is usually one part per drawing, but that is not always the case, such as weldments or other inseparatable assemblies, or in drawings that are only lines (old fashion 2D CAD for schemos and such) which have no parts at all; or in certain types of cable assemblies where no model of the assembly level may exist, but the components are used on the drawing.
I would say the most standard is to assign different part number to each part and assembly. Then each part will have its own drawing. That drawing will then have as many sheets as necessary to adequately describe the part or assy. This is typically how I document something.
I have however in a job shop environment documented differently. In that context I have shown the assembly and all detail parts within the same drawing file. These types of designs will typically have 10-20 sheets. I don't experience substantial performance hits, but these designs are relatively simple. They are welded sheetmetal enclosures with around 20-30 parts.
The issues you describe with file naming and sheet numbering seem to indicate that your chosen method is sub-optimal. I would consider the unique part numbering scheme for your products... since it seems you are experiencing a performance hit with multi-sheet drawings.
General rule: fixture/tooling:multi-sheet
product design: single sheet except where multiple views of the same part are needed
We do fixtures and tooling. We use one part/asm to one drawing. Have done it this way for years in 2D AutoCAD and 3D SolidWorks.
Works great for us.
I have worked both ways. For our needs, I prefer to have assembly sheets in the first file, and the details in their own files, as has already been described. For simple projects, I sometimes put everything in one file. The file names include drawing and sheet numbers with a description, and sometimes the detail number too.
Since we have to have the detail number and quantity on each detail sheet, I store those values in the custom properties of each component. The custom properties are then available anywhere that component appears, including views of subassemblies. I also include the sheet number in the custom properties. The sheet number property gets pulled into the BOM. I also add columns to the BOM for the detail number and quantity custom properties so I can easily check the custom properties against the BOM-generated numbers. I hide the extra columns before release. On versions that support it, I enter these values via the BOM. Someday, when I have time, I'll automate this with a macro.
If you have to support call-backs, the process is similar, but more complex, since detail number, quantity and sheet number custom properties must be unique to each drawing.