Autodesk Inventor

[#1]

Is there a better way to turn alot of features on and off than haveing it turn them on and off for each case?  I have put the code but this takes a while to process and I was wondering if there was a faster way to make this happen than markign each one for being turned on or turned off.  I am using 2011 and this is ilogic for a multi body solid that will be made into an assembly later.

'EFFLUENT RULES FOR TURNING FEATURES ON AND OFF
If EffluentType="Drop Pipe" Then
    Feature.IsActive("DropPipeFlange")=True
    Feature.IsActive("DropPipeEndRim")=True
    Feature.IsActive("DropPipeExtrusion")=True
    Feature.IsActive("DropPipeCut")=True
    Feature.IsActive("DropPipeChannelEnd")=True
    Feature.IsActive("EffluentChannelRim")=False
    Feature.IsActive("PipedEffluentTrim")=False
    Feature.IsActive("PipedEffluentFill")=False
    Feature.IsActive("PipedEffluentPipe")=False
    Feature.IsActive("PipedEffluentFlange")=False
    Feature.IsActive("PipedEffluentCut")=False
    Drop = iFeature.FindRow("DropPipeFlange", "PipeDiameter", "=", EffluentPipeDiameter)'Change iFeature Flange size
    iFeature.ChangeRow("DropPipeFlange", Drop)

ElseIf EffluentType="Channel" Then
    Feature.IsActive("DropPipeFlange")=False
    Feature.IsActive("DropPipeExtrusion")=False
    Feature.IsActive("DropPipeCut")=False
    Feature.IsActive("DropPipeChannelEnd")=False
    Feature.IsActive("EffluentChannelRim")=True
    Feature.IsActive("DropPipeEndRim")=False
    Feature.IsActive("PipedEffluentTrim")=False
    Feature.IsActive("PipedEffluentFill")=False
    Feature.IsActive("PipedEffluentPipe")=False
    Feature.IsActive("PipedEffluentFlange")=False
    Feature.IsActive("PipedEffluentCut")=False

ElseIf EffluentType="Pipe" Then
    Feature.IsActive("DropPipeFlange")=False
    Feature.IsActive("DropPipeExtrusion")=False
    Feature.IsActive("DropPipeCut")=False
    Feature.IsActive("DropPipeChannelEnd")=False
    Feature.IsActive("EffluentChannelRim")=False
    Feature.IsActive("DropPipeEndRim")=False
    Feature.IsActive("PipedEffluentTrim")=True
    Feature.IsActive("PipedEffluentFill")=True
    Feature.IsActive("PipedEffluentPipe")=True
    Feature.IsActive("PipedEffluentFlange")=True
    Feature.IsActive("PipedEffluentCut")=True
    Piped = iFeature.FindRow("PipedEffluentFlange", "PipeDiameter", "=", EffluentPipeDiameter)'Change iFeature Flange size
    iFeature.ChangeRow("PipedEffluentFlange", Piped)
End If

[#2 · Accepted solution]

Every call to Feature.IsActive will do an Update, so it can be slow.  As a workaround, you can have the rule set the end-of-part marker to the top of the model tree.  The part will be temporarily empty, and updates will be fast.  Add this to the top of your rule:

DipartDoc as PartDocument = ThisDoc.Document

partDoc.ComponentDefinition.SetEndOfPartToTopOrBottom(True)' Set to top

Dim partDoc as PartDocument = ThisDoc.Document
partDoc.ComponentDefinition.SetEndOfPartToTopOrBottom(True)' Set to top

And add this at the bottom:

partDoc.ComponentDefinition.SetEndOfPartToTopOrBottom(False) ' Set to bottom

If you need more control over the end-of-part, there is a way to move it before or after a particular feature.

[#3]

the colors of all that text is brown (like its incorrect maybe)  Should it be purple like the rest of the commands?

ThisDoc.Document is purple and Dim is red  I just wanted to make sure this is correct the rule closes and like there is no syntax error but I wanted to make sure there was no error.

[#4]

Those colors sound OK.  Most of that code is Inventor API code (not iLogic functions), so iLogic doesn't show it in purple.  Dim shows up in red because it is a Visual Basic keyword.

[#5]

Thanks that worked I think.

[#6]

I think moving the End Of Part could be useful for a rule I am setting up. How do you go about writing a command to specify where to move the EOP to?

Sorry for jumping into an old thread.