ilogic trigger/ sketch symbol
I can't think of a way to create something on the drawing that would act as a button to trigger a rule. That's a good idea.
Here's a rule that will turn a sketch symbol on and off. I tried several ways, but the only thing that worked was to set the scale of the symbol very small, which turns it into a dot on the page. I hope you can use this.
Change the name "SampleSymbol" in Sub Main to match the name of your symbol.
SymbolOn is a True/False (Boolean) parameter in the drawing. You can replace it with some other logic to decide if you want to make the symbol visible or not.
To make it visible, this changes the scale to 1:1. If your symbol needs to be at a different scale, you can edit this line, or make the scale a parameter to the function.
Sub Main
SetSymbolVisible("SampleSymbol", SymbolOn)
End Sub
Sub SetSymbolVisible(symbolName As String, visible As Boolean)
Dim drawingDoc As DrawingDocument = TryCast(ThisDoc.Document, DrawingDocument)
If (drawingDoc Is Nothing) Then Return
For Each sheetX As Sheet In drawingDoc.Sheets
For Each sketched As SketchedSymbol In sheetX.SketchedSymbols
If (sketched.Name = symbolName) Then
If (visible) Then
sketched.Scale = 1
Else
sketched.Scale = 0.001
End If
End If
Next
Next
End Sub
Mike Deck
Software Developer
Autodesk, Inc.
It is possible to make the dialog box stay open while you are doing other things in Inventor. This requires some code changes to make the dialog work non-modally. You would move the code to assign the iProperty values from your rule to the dialog. Then use the function dlg.Show instead of dlg.ShowDialog. You should also add an event handler to the dialog so that the dialog will close if the document is closed.
What version of Inventor are you using?
> how about it if I put it on a different layer that could be turned on and off?
I tried that (in Inventor 2011). I could turn the text in a Sketched Symbol off, but not the lines (sketch geometry). If you can get this to work manually (make your entire symbol invisible by turning off the layer) please let me know. You can turn off a layer using a rule function such as:
ThisDoc.Document.StylesManager.Layers("Symbol (ANSI)").Visible = False
> I have tried to tell it to put a X in the custom iproperty this works but it doesnt always turn off the X when a different status is selected.
You should be able to fix it by changing the last part of your rule to:
'AS-BUILT FOR RECORDS STATUS'
If DLG.VBSTATUS= "AS-BUILT FOR RECORDS" Then
iProperties.Value("Custom", "AS-BUILT FOR RECORDS")="X"
Else
iProperties.Value("CUSTOM", "AS-BUILT FOR RECORDS")=""
End If
'PRELIMINARY SKETCH/INFORMATION ONLY'
If DLG.VBSTATUS= "PRELIMINARY SKETCH/INFORMATION ONLY" Then
iProperties.Value("Custom", "PRELIMINARY SKETCH/INFORMATION ONLY")="X"
Else
iProperties.Value("Custom", "PRELIMINARY SKETCH/INFORMATION ONLY")=""
End If
'SUBMITTED FOR CUSTOMER APPROVAL'
If DLG.VBSTATUS= "SUBMITTED FOR CUSTOMER APPROVAL" Then
iProperties.Value("Custom", "SUBMITTED FOR CUSTOMER APPROVAL")="X"
Else
iProperties.Value("Custom", "SUBMITTED FOR CUSTOMER APPROVAL")=""
End If
'SUBMITTED FOR CUSTOMER CERTIFICATION'
If DLG.VBSTATUS= "SUBMITTED FOR CUSTOMER CERTIFICATION" Then
iProperties.Value("Custom", "SUBMITTED FOR CUSTOMER CERTIFICATION")="X"
Else
iProperties.Value("Custom", "SUBMITTED FOR CUSTOMER CERTIFICATION")=""
End If
'CERTIFIED FOR FABRICATION'
If DLG.VBSTATUS= "CERTIFIED FOR FABRICATION" Then
iProperties.Value("Custom", "CERTIFIED FOR FABRICATION")="X"
Else
iProperties.Value("Custom", "CERTIFIED FOR FABRICATION")=""
End If
Also, you can get rid of the End If at the end of the rule by changing the line:
If (i=vbOK) Then
to
If (i <> vbOK) Then Return
This will Return (exit from the rule) if i is not vbOK.
I would recommend keeping the code that I send to make the symbol invisible in a separate rule. (Unless we can make the method of turning the layer on and off work. In that case the code would be simpler.)
If you use the code I send as a separate rule, you can trigger it by creating a True/False (Boolean) parameter named SymbolOn, and setting the value of this parameter to True or False in your dialog rule. I'm not sure under what conditions you don't want to show the symbol.
Mike Deck
Software Developer
Autodesk, Inc.
A sketched symbol can have prompted text that is different from what's in the definition. It could be hard to save and restore everything that makes up the symbol. I think my solution of scaling it down to a point is useable. It makes for a simple rule that will work on any sketched symbol.
But yes, it should be possible to save all the info, and then restore the symbol later.
Mike Deck
Software Developer
Autodesk, Inc.
That makes sense. I was thinking that the sketched symbol didn't have a layer until you put an instance of it in the drawing. But the definition has layer information.
Note that you don't need the statement:
iLogicVb.RunRule("SKETCH SYMBOL VIS")
in your rule. When your main rule changes the parameter DSYMBOL, that second rule will run automationcally.
Mike Deck
Software Developer
Autodesk, Inc.
