Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.
FINET_Laurent
in reply to: Anonymous

Hi,

 

This isn't how it's done.. You are creating lines geometry but not constraining them together.

Here is a test iLogic Rule from me where I tested this a while ago.. :

 

'///////////////////////////////////VARIABLES////////////////////////////////////

Dim oDoc As Document 
oDoc = ThisApplication.ActiveDocument

Dim oPartComp As PartComponentDefinition
oPartComp = oDoc.ComponentDefinition

Dim oPlanarSketch As PlanarSketch

Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry

'////////////////////////////SET DEFAULT UNIT TO MM//////////////////////////////

Dim oMillimeterUnit As UnitsTypeEnum
oMillimeterUnit = UnitsTypeEnum.kMillimeterLengthUnits 

	oDoc.UnitsOfMeasure.LengthUnits = oMillimeterUnit
	
'//////////////////////////////CREATE USER PARAMETERS////////////////////////////

Dim oGap1 As UserParameter = oPartComp.Parameters.UserParameters.AddByExpression("Gap_1","50","mm")

'///////////////////////////////CREATE SKETCH////////////////////////////////////

oPlanarSketch = oPartComp.Sketches.Add(oPartComp.WorkPlanes.Item(3))
oPlanarSketch.Name = "Sketch 1"

oPlanarSketch.Edit

'///////////////////////////////PROJECT ORIGIN POINT/////////////////////////////

Dim oOrigin As WorkPoint
	oOrigin = oPartComp.WorkPoints.Item(1)
		Dim oOriginPoint As SketchEntity = oPlanarSketch.AddByProjectingEntity(oOrigin)

'//////////////////////FINALY DRAW THE ACTUAL PART SKETCH////////////////////////

Dim oPoint1 As Point2d = oTG.CreatePoint2d(0, 0)
Dim oPoint2 As Point2d = oTG.CreatePoint2d(0, 3.3)

Dim oValue1 As Double = oGap1.Value + 3 + 5
Dim oPoint3 As Point2d = oTG.CreatePoint2d(oValue1,3.3)

Dim oLine1 As SketchLine = oPlanarSketch.SketchLines.AddByTwoPoints(oPoint1, oPoint2)
	Dim oDimention1 As TwoPointDistanceDimConstraint = oPlanarSketch.DimensionConstraints.AddTwoPointDistance(oLine1.StartSketchPoint,oLine1.EndSketchPoint,DimensionOrientationEnum.kAlignedDim,oLine1.Geometry.MidPoint)
		oLine1.StartSketchPoint.Merge(oOriginPoint)
		oPlanarSketch.GeometricConstraints.AddVertical(oLine1)
		
Dim oLine2 As SketchLine = oPlanarSketch.SketchLines.AddByTwoPoints(oPoint2, oPoint3)
	Dim oDimention2 As TwoPointDistanceDimConstraint = oPlanarSketch.DimensionConstraints.AddTwoPointDistance(oLine2.StartSketchPoint,oLine2.EndSketchPoint,DimensionOrientationEnum.kAlignedDim,oLine2.Geometry.MidPoint)
		oDimention2.Parameter.Expression = "Gap_1 + 30 + 50"
		oLine1.EndSketchPoint.Merge(oLine2.StartSketchPoint)
		oPlanarSketch.GeometricConstraints.AddPerpendicular(oLine1, oLine2)
	
Dim oPoint4 As Point2d = oTG.CreatePoint2d(oPoint3.X,0.8)	
	
Dim oLine3 As SketchLine = oPlanarSketch.SketchLines.AddByTwoPoints(oPoint3, oPoint4)
	Dim oDimention3 As TwoPointDistanceDimConstraint = oPlanarSketch.DimensionConstraints.AddTwoPointDistance(oLine3.StartSketchPoint, oLine3.EndSketchPoint, DimensionOrientationEnum.kAlignedDim, oLine3.Geometry.MidPoint)
		oLine3.StartSketchPoint.Merge(oLine2.EndSketchPoint)
		oPlanarSketch.GeometricConstraints.AddPerpendicular(oLine2, oLine3)
		
Dim oPoint5 As Point2d = oTG.CreatePoint2d(3, oPoint4.Y)	

Dim oLine4 As SketchLine = oPlanarSketch.SketchLines.AddByTwoPoints(oPoint4, oPoint5)
	oLine4.StartSketchPoint.Merge(oLine3.EndSketchPoint)
	oPlanarSketch.GeometricConstraints.AddPerpendicular(oLine3, oLine4)
	
Dim oPoint6 As Point2d = oTG.CreatePoint2d(3, 0)	

Dim oLine5 As SketchLine = oPlanarSketch.SketchLines.AddByTwoPoints(oPoint5, oPoint6)
	oLine5.StartSketchPoint.Merge(oLine4.EndSketchPoint)
	oPlanarSketch.GeometricConstraints.AddPerpendicular(oLine4, oLine5)

Dim oLine6 As SketchLine = oPlanarSketch.SketchLines.AddByTwoPoints(oPoint6, oPoint1)
	Dim oDimention4 As TwoPointDistanceDimConstraint = oPlanarSketch.DimensionConstraints.AddTwoPointDistance(oLine6.StartSketchPoint,oLine6.EndSketchPoint,DimensionOrientationEnum.kAlignedDim,oLine6.Geometry.MidPoint)
		oLine6.StartSketchPoint.Merge(oLine5.EndSketchPoint)
		oLine6.EndSketchPoint.Merge(oLine1.StartSketchPoint)
		oPlanarSketch.GeometricConstraints.AddPerpendicular(oLine5, oLine6)	

oPlanarSketch.ExitEdit

'//////////////////////////////EXTRUDE THE SKETCH/////////////////////////////

Dim oProfile As Profile 
oProfile = oPlanarSketch.Profiles.AddForSolid

Dim oExtrude1 As ExtrudeFeature = oPartComp.Features.ExtrudeFeatures.AddByDistanceExtent(oProfile, 0.5 , kSymmetricExtentDirection, kJoinOperation)
oExtrude1.Name = "Extrusion1"

'/////////////////////////////////CHANGE COLOR////////////////////////////////

Dim oAppearence As Asset
oAppearence = oDoc.Assets.Add(kAssetTypeAppearance, "Generic", "Appearances")

Dim oColor As ColorAssetValue
oColor = oAppearence.Item("generic_diffuse")

oColor.Value = ThisApplication.TransientObjects.CreateColor(0,145,255)

oExtrude1.Appearance = oAppearence

 Hope this helps ,


Regards,

 

FINET L.

If this post solved your question, please kindly mark it as "Solution"

If this post helped out in any way to solve your question, please drop a "Like"

@LinkedIn     @JohnCockerill