I would like to create a macro to change the color of a circle on a Solidworks drawing.
I would like to launch the macro select a diameter to search for example: 5 , then in the view that I would have selected that it searches for all the diameters and selects them to then be able to change the color.
Is this possible? If so, how to find circles and selection?
This tutorial allows you to select a single circle, but I have a lot more. And renaming each edge of each circle in the room to make the macro work, is much longer than directly selecting the circles in the drawing. The idea was good but it doesn't work for me.
If you just want to select the circles: erase the last 2 lines
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim swView As SldWorks.View
Dim Comp As SldWorks.Component2
Dim vComps As Variant
Dim vComp As Variant
Dim vEdges As Variant
Dim vEdge As Variant
Dim swEdge As SldWorks.Edge
Dim swCurve As SldWorks.Curve
Dim swEntity As SldWorks.Entity
Dim CurveParam As Variant
Dim IsClosed As Boolean
Dim Diameter As Double
Dim boolstatus As Boolean
Sub main()
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swDraw = swModel
Set swView = swDraw.ActiveDrawingView
swModel.ClearSelection2 True
vComps = swView.GetVisibleComponents
Diameter = InputBox("Entrer le diamètre en mm")
For Each vComp In vComps
Set Comp = vComp
vEdges = swView.GetVisibleEntities(Comp, swViewEntityType_e.swViewEntityType_Edge)
For Each vEdge In vEdges
Set swEdge = vEdge
Set swCurve = swEdge.GetCurve
If swCurve.IsCircle Then
swCurve.GetEndParams Empty, Empty, IsClosed, Empty
If IsClosed Then
CurveParam = swCurve.CircleParams
If Abs(Diameter - CurveParam(6) * 2 * 1000) < 0.0001 Then
Set swEntity = swEdge
swEntity.Select4 True, Nothing
End If
End If
End If
Next
Next
swModel.SetLineColor 255
swModel.ClearSelection2 True
End Sub