iLogic Sketch Creation
Dear Tefkleidis,
Then I'll show you what I understood from your query
- Once done the "Sketch", proceed to the "Manage" tab:
- Once there, deploy "Ilogic" which is where you can add the form or manage the necessary rules:
- You can work from "Parameters" yes you need:
This is what you needed?
Accepted solution
Hi tefkleidis,
Here are 3 quick examples adapted from the Inventor API samples.
Also just as a tip, you can search and ask programming questions of this type on the Inventor Customization forum too:
http://forums.autodesk.com/t5/Autodesk-Inventor-Customization/bd-p/120
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Example 1
Draw 3 lines to make a Triangle example:
' Check to make sure a sketch is open.
If Not TypeOf ThisApplication.ActiveEditObject Is PlanarSketch Then
MessageBox.Show("A sketch must be active.", "iLogic")
Return
End If
'set a reference to the active sketch.
Dim oSketch As PlanarSketch
oSketch = ThisApplication.ActiveEditObject
'set a reference to the transient geometry collection.
Dim oTransGeom As TransientGeometry
oTransGeom = ThisApplication.TransientGeometry
' Create a new transaction to wrap the construction of the three lines
' set into a single undo.
Dim oTrans As Transaction
oTrans = ThisApplication.TransactionManager.StartTransaction( _
ThisApplication.ActiveDocument, _
"Create Triangle Sample")
' Create the first line of the triangle. This uses two transient points as
' input to definethe coordinates of the ends of the line. Since a transient
' point is input a sketch point is automatically created at that location and
' the line is attached to it.
Dim oLines(0 To 2) As SketchLine
oLines(0) = oSketch.SketchLines.AddByTwoPoints(oTransGeom.CreatePoint2d(0, 0), _
oTransGeom.CreatePoint2d(4, 0))
' Create a sketch line that is connected to the sketch point the previous lines
' end point is connected to. This will automatically create the constraint to
' tie the new line to the sketch point the previous line is also connected to.
' This will result in the the two lines being connected since they're both tied
' to the same sketch point.
oLines(1) = oSketch.SketchLines.AddByTwoPoints(oLines(0).EndSketchPoint, _
oTransGeom.CreatePoint2d(2, 3))
' Create a third line and connect it to the start point of the first line and the
' end point of the second line. This will result in a connected triangle.
oLines(2) = oSketch.SketchLines.AddByTwoPoints(oLines(1).EndSketchPoint, _
oLines(0).StartSketchPoint)
' End the transaction
oTrans.End
iLogicVb.UpdateWhenDone = True
Example 2
2 Point Rectangle example:
' Check to make sure a sketch is open.
If Not TypeOf ThisApplication.ActiveEditObject Is PlanarSketch Then
MessageBox.Show("A sketch must be active.", "iLogic")
Return
End If
'set a reference to the active sketch.
Dim oSketch As PlanarSketch
oSketch = ThisApplication.ActiveEditObject
'set a reference to the transient geometry collection.
Dim oTransGeom As TransientGeometry
oTransGeom = ThisApplication.TransientGeometry
' Create a rectangle
Dim oRectangleLines As SketchEntitiesEnumerator
oRectangleLines = oSketch.SketchLines.AddAsTwoPointRectangle( _
oTransGeom.CreatePoint2d(0, 0), _
oTransGeom.CreatePoint2d(8, 5))
iLogicVb.UpdateWhenDone = True
Example 3
3 Point (rotated) Rectangle example:
' Check to make sure a sketch is open.
If Not TypeOf ThisApplication.ActiveEditObject Is PlanarSketch Then
MessageBox.Show("A sketch must be active.", "iLogic")
Return
End If
'set a reference to the active sketch.
Dim oSketch As PlanarSketch
oSketch = ThisApplication.ActiveEditObject
'set a reference to the transient geometry collection.
Dim oTransGeom As TransientGeometry
oTransGeom = ThisApplication.TransientGeometry
' Create a rotated rectangle
oRectangleLines = oSketch.SketchLines.AddAsThreePointRectangle( _
oTransGeom.CreatePoint2d(0, 0), _
oTransGeom.CreatePoint2d(7, 3), _
oTransGeom.CreatePoint2d(8, 8))
iLogicVb.UpdateWhenDone = True
Accepted solution
Hi Eugene,
It may be doable via iLogic. But, you don't actually need to do it in iLogic. Go to Tools -> Application Options -> Part -> Sketch on New Part Creation -> select an origin plane -> Ok.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
