CAD Forum

This may be a stupid question, because I think the answer is no.

In a drawing,
Can you "Explode" an annotation linked to a custom property in the component it is attached to, so that the text that was linked now shows (and is editable) and breaks its link to property?

Right now, the only way I can consider to achieve this is to open the component, view its custom properties, copy the text value, return to the drawing, and paste the text into the annotation.

I'm not aware of any way to do that. You can of course pull the end of the leader off the model so it loses the link, and then the text box will display the property text, but you can't edit it (other than deleting it and starting over).

Thanks Glenn and Toby.

I'm quite comfortable by now to use notepad as a format-cleansing text filter for importing a copied text string from a webpage into a drawing annotation. I keep Notepad as a pinned app next to Calculator and Snipping tool, my basic basics that don't run at startup. I had not considered copying it through there, but that is still far easier than: opening component (wait), open properties (wait), select and copy, close, then close without saving and also discarding changes. This is a time saver, Toby. I indicate this here as the correct answer without marking it correct. It is a delightful workaround to me.

To expand on the copy/paste, it also covers a single annotation with multiple properties linked: Description, Brand, & PartNo, all in one go.

I tend to overwrite, break, and explode pretty much anything if it's used and applied this once-here for fair reasons. At least I use an override specific color to denote it (purple before purple was sarcasm). Therefore, I'd also love to have that opportunity to break a link anywhere, and not just in a BOM.

Is this something you need to do a lot?
Here is a dumb little macro that will do what you're looking for. Just select any note and run it.

Dim swApp As SldWorks.SldWorks
Dim swSelMgr As SldWorks.SelectionMgr
Dim swNote As SldWorks.Note

Sub main()

Set swApp = Application.SldWorks
Set swSelMgr = swApp.ActiveDoc.SelectionManager
If swSelMgr.GetSelectedObjectType3(1, -1) <> swSelNOTES Then
MsgBox "Please select a note and run the macro"
Exit Sub
End If
Set swNote = swSelMgr.GetSelectedObject6(1, -1)
swNote.PropertyLinkedText = swNote.GetText
End Sub

TooTallToby wrote: ↑Tue Jan 25, 2022 4:15 pm This isn't a "great" solution, but you can do this:

1. Make sure VIEW>HIDE/SHOW is set to NOT show annotation link variables (not checked)
2. Double click on the annotation which is linked to a custom property
3. Select the entire note, CTRL+C
4. Go into NOTEPAD. CTRL+V. Select all. CTRL+C
5. Go back into SOLIDWORKS. Double click the linked annotation. Delete the existing note text. CTRL+V

A macro (already posted by @josh ) would be much quick method handy but if you want to do the steps manually, you can shorten them to following:

1. Double click on the annotation which is linked to a custom property (this will select the complete annotation)
2. CTRL+C
3. Right click on the annotation and select "edit in window"
4. In the open window CTRL+V and click OK.

josh wrote: ↑Thu Jan 27, 2022 7:51 pm Is this something you need to do a lot?

No not often, but when I do it would apply to a series of similar drawings where one project contains an exception.