Edit Sketch, Delete Constraints
Some how i dont have this option but therefor i dont know if DimensionConstraint and/or GeometricConstraint. Any wy here a rule that deletes both when you select a sketch.
Dim Sketch As PlanarSketch = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAllPlanarEntities,
"Select a sketch")
For Each Constraint As DimensionConstraint In Sketch.DimensionConstraints
Constraint.Delete()
Next
For Each Constraint As GeometricConstraint In Sketch.GeometricConstraints
If (Constraint.Deletable) Then
Constraint.Delete()
End If
Next
Jelte de Jong
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Blog: hjalte.nl - github.com
This iLogic code lets you select individual sketch entities to delete its constraints, then loops for your next selection untill you click No.
Repeat :
Dim oSC As SketchEntity = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kSketchCurveFilter, "Select a Sketch Curve.") oConsts = oSC.Constraints For Each oGC As GeometricConstraint In oConsts oGC.Delete Next For Each oDC As DimensionConstraint In oConsts oDC.Delete Next oAns = MessageBox.Show("Keep going?","LOOP",MessageBoxButtons.YesNo,MessageBoxIcon.Question,MessageBoxDefaultButton.Button1) If oAns = vbYes Then GoTo Repeat Else Return End If
Wesley Crihfield
(Not an Autodesk Employee)
try this:
Public Sub deleteConstraint()
Dim Sketch As PlanarSketch
Set Sketch = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAllPlanarEntities, "Select a sketch")
Dim Constraint As GeometricConstraint
For Each Constraint In Sketch.GeometricConstraints
If (Constraint.Deletable) Then
If (Constraint.Type <> ObjectTypeEnum.kCoincidentConstraintObject) Then
Constraint.delete
End If
End If
Next
End Sub
Jelte de Jong
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very strange for me this works. Can u send some screeen shots of what you are doing. (Or part file if you are working with inventor 2018 or earlyer)
Jelte de Jong
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Hi @shastu
This worked to delete the constraints on the file called 2018DC.ipt.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Sub Main()
Dim oDoc As Document
Set oDoc = ThisApplication.ActiveDocument
Dim oCompDef As PartComponentDefinition
Set oCompDef = oDoc.ComponentDefinition
Dim oHole As HoleFeature
Dim oSketch As Sketch
For Each oHole In oCompDef.Features.HoleFeatures
If Not oHole.Sketch Is Nothing Then
Set oSketch = oCompDef.Sketches.Item(oHole.Sketch.Name)
oSketch.Edit
Dim oConstraint As DimensionConstraint
For Each oConstraint In oSketch.DimensionConstraints
oConstraint.Delete
Next
Dim oGeometricConstraint As GeometricConstraint
For Each oGeometricConstraint In oSketch.GeometricConstraints
If oGeometricConstraint.Deletable Then
oGeometricConstraint.Delete
End If
Next
oDoc.Update
End If
Next
End Sub
Hi @shastu ,
Okay, give this one a try, I think this is Delete Constraints context command you mentioned in the first post.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Sub Main()
Dim oDoc As Document
Set oDoc = ThisApplication.ActiveDocument
Dim oCompDef As PartComponentDefinition
Set oCompDef = oDoc.ComponentDefinition
Dim oHole As HoleFeature
Dim oSketch As Sketch
For Each oHole In oCompDef.Features.HoleFeatures
If Not oHole.Sketch Is Nothing Then
Set oSketch = oCompDef.Sketches.Item(oHole.Sketch.Name)
Dim oSelSet As SelectSet
Set oSelSet = oDoc.SelectSet
oSketch.Edit
Call oSelSet.Select(oSketch)
' Get the CommandManager object.
Dim oCommandMgr As CommandManager
Set oCommandMgr = ThisApplication.CommandManager
' Get control definition for the line command.
Dim oControlDef As ControlDefinition
Set oControlDef = oCommandMgr.ControlDefinitions.Item( _
"SketchDeleteConstraintsCtxCmd")
' Execute the command.
Call oControlDef.Execute
oDoc.Update
End If
Next
End Sub
@shastu wrote:
Thank you so much. How did you find it?
I ran this (from the iLogic editor) and then searched for "DeleteConstraint" in the resulting text file... the key part to using it though is that we have to select the sketch first (since this one is a context command) .
' Get the CommandManager object.
Dim oCommandMgr As CommandManager
oCommandMgr = ThisApplication.CommandManager
' Get the collection of control definitions.
Dim oControlDefs As ControlDefinitions
oControlDefs = oCommandMgr.ControlDefinitions
'____Create and write to a text file_________________
oFile = "C:\temp\CommandNames.txt"
oWrite = System.IO.File.CreateText("C:\temp\CommandNames.txt")
oWrite.WriteLine(vbTab & "Command Name" & vbTab & " | " & "Description")
' Iterate through the controls and write out the name.
For Each oControlDef In oControlDefs
oWrite.WriteLine(oControlDef.InternalName & vbTab & " | " & oControlDef.DescriptionText )
Next
oWrite.Close()
'open the file
ThisDoc.Launch(oFile)
i think i found the problem. In my original post i only tested with a square that i had drawn but in your example you have a square that is a refrence to a model geometry. It seem that the command "delete all constraints" also deletes the refrences to the model geometry. When i incorporate that in the code it seems to work. Try this code.
Public Sub deleteConstraint()
Dim Sketch As PlanarSketch
Set Sketch = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAllPlanarEntities, "Select a sketch")
Dim line As SketchLine
For Each line In Sketch.SketchLines
line.Reference = False
Next
Dim Constraint As GeometricConstraint
For Each Constraint In Sketch.GeometricConstraints
If (Constraint.Deletable) Then
If (Constraint.Type <> ObjectTypeEnum.kCoincidentConstraintObject) Then
Constraint.Delete
End If
End If
Next
End SubEdit:
i see now that @Curtis_Waguespack has found a other solution.
Jelte de Jong
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