Changing the parameter value in the form creates a new feature
If your local parameter is called "del", then I can see why this rule is running every time the value of that parameter changes. In a local (saved within a document) iLogic rule contains the unquoted name of a parameter that exists in that same document, then every time the value of that parameter changes it will cause this rule to run. Try getting the value of that parameter in a different way and store it in a variable, without leaving it's name unquoted, then use that variable instead of 'del' in that last line of code.
So, try replacing this:
Dim oFeat1 As ExtrudeFeature
oFeat1 = ocomp1.Features.ExtrudeFeatures.AddByDistanceExtent(profil01, del, kPositiveExtentDirection, kJoinOperation)with this:
Dim oDel As Double = Parameter("del")
Dim oFeat1 As ExtrudeFeature
oFeat1 = ocomp1.Features.ExtrudeFeatures.AddByDistanceExtent(profil01, oDel, kPositiveExtentDirection, kJoinOperation)That should eliminate it running automatically every time the value of that parameter changes.
Wesley Crihfield
(Not an Autodesk Employee)
Yes. That can be done to, if you want it that way. Basically we could have it search for the existing feature first, and if it already exists, then don't proceed to create it again. It's usually best to do this by the feature's name, but if you only have one extrude feature in your model (and it will always be that way) we can just look for the first extrude feature. Then if it doesn't find one, proceed through the rest of your code to create it. You can also add an additional line of code after you create the feature to give it a specific name if you wanted. That would ensure it will be named what you are expecting to find the next time. Is this what you want?
Wesley Crihfield
(Not an Autodesk Employee)
I think you just missed a step when trying to get the ExtrudeFeatures object.
Instead of this:
oVysu = ocomp1.ExtrudeFeaturesit should have been this:
oVysu = ocomp1.Features.ExtrudeFeaturesThis version might work for you.
Dim oprt1 As PartDocument = ThisApplication.ActiveDocument
Dim ocomp1 As PartComponentDefinition = oprt1.ComponentDefinition
'check to see if this feature already exists
'create a Boolean type parameter to record if we find it or not
Dim oFound As Boolean = False
'check for it by name with this code
If ocomp1.Features.ExtrudeFeatures.Count > 0 Then
For Each oEF As ExtrudeFeature In ocomp1.Features.ExtrudeFeatures
'<<<< CHANGE THIS FEATURE NAME TO MATCH YOURS >>>>
If oEF.Name = "My Extrude Feature" Then
'it was found
oFound = True
End If
Next
Else
'there were no extrude features yet
oFound = False 'not necessary, because it would still be False already
End If
If oFound = True Then 'it was found, so don't do anything and exit the rule
Exit Sub 'or Return 'this will exit the rule
ElseIf oFound = False Then 'it was not found, so create it
Dim osketch1 As PlanarSketch = ocomp1.Sketches.Add(ocomp1.WorkPlanes(1))
Dim otgeo As TransientGeometry = ThisApplication.TransientGeometry
Dim jcko As SketchArc
Dim jcko1 As SketchLine
jcko = osketch1.SketchArcs.AddByCenterStartEndPoint(otgeo.CreatePoint2d(0, 0), otgeo.CreatePoint2d(0, 10), otgeo.CreatePoint2d(0, -10), True)
jcko1 = osketch1.SketchLines.AddByTwoPoints(osketch1.SketchArcs.Item(1).StartSketchPoint, otgeo.CreatePoint2d(50, 10))
jcko1 = osketch1.SketchLines.AddByTwoPoints(osketch1.SketchLines.Item(1).EndSketchPoint, otgeo.CreatePoint2d(50, 5))
jcko1 = osketch1.SketchLines.AddByTwoPoints(osketch1.SketchLines.Item(2).EndSketchPoint, otgeo.CreatePoint2d(0, 5))
jcko = osketch1.SketchArcs.AddByCenterStartEndPoint(otgeo.CreatePoint2d(0, 0), osketch1.SketchLines.Item(3).EndSketchPoint, otgeo.CreatePoint2d(0, -5), True)
jcko1= osketch1.SketchLines.AddByTwoPoints(osketch1.SketchArcs.Item(1).EndSketchPoint,osketch1.SketchArcs.Item(2).EndSketchPoint)
Dim profil01 As Profile = osketch1.Profiles.AddForSolid
Dim oDel As Double = Parameter("del")
Dim oFeat1 As ExtrudeFeature
oFeat1 = ocomp1.Features.ExtrudeFeatures.AddByDistanceExtent(profil01, oDel, kPositiveExtentDirection, kJoinOperation)
'<<<< CHANGE THIS FEATURE NAME TO MATCH YOURS >>>>
oFeat1.Name = "My Extrude Feature"
End IfWesley Crihfield
(Not an Autodesk Employee)
