Can you collate seperate IDW'd into one IDW easily?

[terryN2JGG]

We have a tool that automatically puts any opened parts into drawing sheets and adds basic views and BOMs etc. However each part ends up with its own IDW.

Is there an easy way of collating several separate IDWs into one multisheet IDW?

Cheers T

[hollypapp65]

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@terryN2JGG wrote:

However each part ends up with its own IDW.

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This is a good thing.  Part and drawing are "linked".  Easy to find drawing.

You can copy and paste sheet from different IDW into one IDW.

With enough sheets in the IDW, it'll get slow and unstable.

[WCrihfield]

Although it is true that we can copy a Sheet from within one DrawingDocument into another one, it does not always work out as well as expected.  Plus, the part (or assembly) is not actually 'Linked' to any drawing that it may be represented in...at least not from the part / assembly's perspective.  The drawing, on the other hand, does have a 'reference' to the part or assembly document, due to the drawing views referring to them.  That 'reference' does not go both ways though, just from the drawing to the 'model' file, not from the model to the drawing.  People often think they are linked due to our ability to open a drawing from a model document.  But that only works when the drawing file is saved in the same folder as the model file, and the drawing file has the same file name as the model file, but with different file extension, of course.  When you use that sequence of events to open the drawing from the model, it assumes those associations, and looks for it there, and if not found there, with that name, it will just show you the 'Open' dialog, and wait for you to pick out the drawing file for it to open.

Now on why the copy over idea doesn't always work out well.  It depends on several things.  One is the border and title block.  If there are any TextBoxes within them that are supposed to represent 'Linked' information, such as an iProperty, Parameter, Mass Properties, or similar, and it is 'Linked' to 'the model' then those generally refer to the first view that was added into the whole drawing document, not just the views on that sheet.  This may have changed in recent releases of Inventor, but that was the 'traditional' way they worked.  So, when you copy a sheet from one drawing into another, those 'Linked' properties may change from pointing to (or pulling data from) the 'model' in the first drawing document, to the model in the destination drawing document.  Plus, sheet numbers may change, which can cause issues, depending on how you have that set-up in your drawings.  Individual sheets in a drawing were not intended to be for independent models, but all sheets for one model.  But as I mentioned, this may have changed in recent releases of Inventor.  I am aware of the relatively new Sheet.TextPropertySource property, and the DrawingView.IsTextPropertySource property, which were both added in the 2023 version, which may help with that situation.  Where I have worked for the past 11+ years, every model file has its own drawing file, even the assemblies.  And assembly drawings only cover the details of the 'main' assembly, not any of the 'components', because all components and sub assemblies have their own drawings.  I know that is not normal for every company or user though.