Make lines into construction lines
RC on the lines, select properties and select a different line type style.
Or if you like something that was said and it was helpful, Kudos
Yeah, that's pretty key. 
I am no iLogic guru, but here is a link that might help you get what you are looking for.
https://forums.autodesk.com/t5/inventor-forum/help-with-view-label-ilogic-rule/td-p/5001126
Or if you like something that was said and it was helpful, Kudos
A little late to the party but I had the same question and finally found a solution. Posting for anyone else that might have the question.
Basically, a parameter subset of your variable you assign a boolean value to, False being default.
oTop = oSketch.AddByProjectingEntity("YourProjectedEntityHere") 'project Top side oTop.Construction = True
[Or]
oLine = oSketch.SkethLines.AddByTwoPoints(oPt1, oPt2)
oLine.Construction = True
Autodesk Inventor Certified Professional
It'll be up to you to either manage all the lines (entities actually) within a sketch or search through all the entities within the sketch to identify the specific line you are wanting to edit. You'll need to know something about the entity you're looking for in order to identify it. It could be a point that's located on a plane, you may already know a start or stop point, there's any number of ways to search for location or features, but you must know something about the line or allow the user to select the line to identify it for you.
Once you have the specific entity identified, you assign that entity to a variable name to make it easier to manage since making a modification to that entity could alter the Inventor variable you just found it as. In the case of my previous example, I assigned the line to the variable "oLine" which was my way of referencing that entity to modify it.
True I only showed a very small snippet of that code, assuming you knew a bit about coding already. It would appear there's still a bit of learning going on here so I'll include more code that would at least allow you to run the example...
'declare how variable names will be used as
Dim oDoc As PartDocument = ThisDoc.Document
Dim oCompDef As PartComponentDefinition = oDoc.ComponentDefinition
Dim oTG As TransientGeometry = ThisApplication.TransientGeometry
Dim oSketch As PlanarSketch
Dim oWorkPlane As WorkPlane
Dim oLine As SketchLine
Dim oPt1, oPt2 As Point2d
For Each oSketch In oCompDef.Sketches 'delete any previous test sketch
If oSketch.Name = "Test Sketch" Then oSketch.Delete
Next
'Create a sketch
oWorkPlane = oCompDef.WorkPlanes.Item("XY Plane") 'assign XY Plane to oWorkplane variable
oSketch = oCompDef.Sketches.Add(oWorkPlane) 'assign oSketch as the variable for this new sketch
oSketch.Name = "Test Sketch" 'Assign Model Tree name to this scketch
oGC = oSketch.GeometricConstraints 'variable name shortcut for Sketch Constraints
oPt1 = oTG.CreatePoint2d(0, 0) 'identify location for first point variable
oPt2 = oTG.CreatePoint2d(5, -12) 'identify location for second point variable
oLine = oSketch.SketchLines.AddByTwoPoints(oPt1, oPt2) 'create a new line and reference it as the variable "oLine"
oLine.Construction = True
Hope this helps.
Autodesk Inventor Certified Professional
In that case you need to translate:
"The line I want to edit" into something that programming logic can express. For example: Is the sketch geometry stable (always change the 3rd line in the sketch), or the middle line of 3 connected ones, ....
Is user interaction with your logic an option (pick it)?
Without really knowing what your inputs are and what you are trying to accomplish by changing to construction it's hard to give a more useful answer.
Thanks,
Gerald
Gerald Hochenauer
Senior Principal Engineer, Inventor
Autodesk, Inc.