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CAD tip CAD tip # 12697:

Question CAD 
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Q - question

Opposite angle for angular dimensions in Inventor drawings (iLogic).

A - answer How to dimension angles including the value of an opposite angle (to 90°) in Inventor drawings?

If you need to show not only the main value of an angle but also a complementary opposite angle value (to 90°), you can use the following iLogic rule. It adds the "opposite" angle (in parentheses) to a selected, plain angular dimension. The displayed preecision will be the same as in the main dimension.

Any subsequent change of the angle or dimension style will not update the opposite angle dimension dynamically. You will need tu re-apply the rule. You can add an icon for this rule into Inventor ribbon e.g. by using our X-Tools.

The iLogic code:

'Adds opposite (90°) angle to ang.dimension (CAD Studio, 2020,
Dim oSelection As Object = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingDimensionFilter, "Select an angular dimension:")
If IsNothing(oSelection) Then Return
If oSelection.Type <> kAngularGeneralDimensionObject Then
	MsgBox("This is not an angular dimension!", vbCritical, "Inventor")
End If
Dim oDim As AngularGeneralDimension = oSelection
Dim opposíte As Double = 90.0-oDim.ModelValue*180.0/PI 'opposite to 90°
If oDim.Text.FormattedText.Contains("°)") Then 'update
	oDim.Text.FormattedText = "<‍DimensionValue/>" & vbCrLf & "(" & CStr(Round(opposíte,oDim.Precision)) & "°)"
Else 'create
        oDim.Text.FormattedText = oDim.Text.FormattedText & vbCrLf & "(" & CStr(Round(opposíte,oDim.Precision)) & "°)"
End If
oDim.Text.HorizontalJustification = kAlignTextCenter
100% *  CAD 
16.8.2020    506×  
applies to: Inventor ·

See also:
Tip 12712:How to set the option "Active Window on Save" through iLogic?
Tip 12644:How to identify parts and assemblies imported from STEP/IGES?
Tip 12520:How to set Inventor Display style and Lighting style from an iLogic macro?
Tip 12508:How to assign an expression (not value) to a user parameter with iLogic?
Tip 12462:Mass- (table-) rename parameters in Inventor.

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