I have a problem to solve
I made in part
First, I show DIMENSION
Then I pick a value of DIMENSION in Sketch
And save it auto as "L1" in the CUSOM of IPROPERTIES
Get Dimension of sketch to Iproperties
Hi @haphanthanhtam.work. Yes, it is possible to pick a DimensionConstraint within a Sketch, then get the Parameter it represents, then try to expose that Parameter as a custom iProperty. Here is a simple example iLogic code like that:
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kSketchDimConstraintFilter, "Select a Sketch Dimensional Constraint.")
If oObj Is Nothing OrElse (TypeOf oObj Is DimensionConstraint = False) Then Exit Sub
Dim oDimConst As DimensionConstraint = oObj
Dim oParam As Inventor.Parameter = oDimConst.Parameter
Try
oParam.ExposedAsProperty = True
Catch
MsgBox("Error trying to expose the parameter as a custom iProperty!", vbCritical, "Failure")
End TryIf this solved your problem, or answered your question, please click ACCEPT SOLUTION .
Or, if this helped you, please click (LIKE or KUDOS) 👍.
Wesley Crihfield
(Not an Autodesk Employee)
See this example for renaming the exported iProperty, processing the entire sketch.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
'example expects a parameter named something like E_Width 'results in an iproperty named something like L_Width Dim oDoc As PartDocument = ThisDoc.Document Dim oSketch As PlanarSketch = oDoc.ComponentDefinition.Sketches.Item("Sketch1") Dim oDimConstraint As DimensionConstraint For Each oDimConstraint In oSketch.DimensionConstraints Dim oParameter As Inventor.Parameter = oDimConstraint.Parameter 'only export parameters with E_ in the name Try : oParameter.ExposedAsProperty = oParameter.Name.Contains("E_") Catch : Logger.Info(oParameter.Name & " not exported") : End Try Next 'rename exported iproperty For Each oProp As Inventor.Property In oDoc.PropertySets.Item("User Defined Properties") If oProp.Name.Contains("E_") Then Try : oProp.DisplayName = oProp.Name.Replace("E_", "L_") : Catch : End Try End If Next
Accepted solution
Hi @haphanthanhtam.work ,
Here's another example using WCrihfield's pick method example.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kSketchDimConstraintFilter, "Select a Sketch Dimensional Constraint.") If oObj Is Nothing OrElse (TypeOf oObj Is DimensionConstraint = False) Then Exit Sub Dim oDimConst As DimensionConstraint = oObj Dim oParam As Inventor.Parameter = oDimConst.Parameter Try oParam.ExposedAsProperty = False 'set to false, to ensure it is exported again oParam.ExposedAsProperty = True Catch MsgBox("Error trying to expose the parameter as a custom iProperty!", vbCritical, "Failure") End Try 'rename exported iproperty oProp = ThisDoc.Document.PropertySets.Item("User Defined Properties").Item(oParam.Name) ThisDoc.Document.PropertySets.Item("User Defined Properties").Item(oParam.Name).DisplayName = "L_" & oProp.DisplayName
Accepted solution
OK. Here is another similar example that does not try to expose the parameter, and instead just tries to create (or update) a custom iProperty, using the 'Expression' of the Parameter. The Expression is a String, and usually includes the units specifier, just like you see it in the Parameters dialog. But it can also contain an equation, which might mess things up here. But the Value and ModelValue of a Parameter API object is always in 'database units' instead of document units or the parameter's own units, that's why I'm trying to use the Expression instead. Using the simple Parameter() method could be risky when used within an assembly scenario, and trying to control another document, so I stuck with API methods instead here.
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kSketchDimConstraintFilter, "Select a Sketch Dimensional Constraint.")
If oObj Is Nothing OrElse (TypeOf oObj Is DimensionConstraint = False) Then Exit Sub
Dim oDimConst As DimensionConstraint = oObj
Dim oParam As Inventor.Parameter = oDimConst.Parameter
Dim oDoc As Document = Nothing
Try : oDoc = oParam.Parent : Catch : End Try
If oDoc Is Nothing Then Exit Sub
If oDoc.IsModifiable = Fasle Then Exit Sub 'can't create the custom property in it, or change its value
Dim oCProps As PropertySet = oDoc.PropertySets.Item(4)
Dim oCProp As Inventor.Property = Nothing
Dim oCPropName As String = "Custom name"
Try
oCProp = oCProps.Item(oCPropName)
Catch
oCProp = oCProps.Add(oParam.Expression, oCPropName)
End Try
If oCProp IsNot Nothing AndAlso oCProp.Value <> oParam.Expression Then
oCProp.Value = oParam.Expression
End If
If this solved your problem, or answered your question, please click ACCEPT SOLUTION .
Or, if this helped you, please click (LIKE or KUDOS) 👍.
Edit: You could swap out this line:
Dim oCPropName As String = "Custom name"for this line:
Dim oCPropName As String = InputBox("Enter Custm iProperty Name", "Property Name", oParam.Name)...to make it more interactive.
Wesley Crihfield
(Not an Autodesk Employee)
Another process which might be even better, would be to show you the current name of the parameter, and allow you to rename that first, then continue to expose that parameter as a custom iProperty. That way, you now know which parameter is controlling it, and do not need to have the parameter and the custom iProperty have different names. Just a thought.
Wesley Crihfield
(Not an Autodesk Employee)
Thanks so much @Curtis_Waguespack , @WCrihfield @A.Acheson
It's works
but now there is a problem I keep selecting another value but it's not on Sketch For example dimension on extrusion or other. Is there any way I can pick it up and output that value
Here is something that might work. It is probably a FeatureDimension.
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kFeatureDimensionFilter, "Select a feature dimension.")
If oObj Is Nothing OrElse (TypeOf oObj Is FeatureDimension = False) Then Exit Sub
Dim oFDim As FeatureDimension = oObj
Dim oParam As Inventor.Parameter = oFDim.Parameter
Dim sName As String = InputBox("Edit Parameter Name", "Rename Param", oParam.Name)
If sName <> "" Then Try : oParam.Name = sName : Catch : End Try
Try
oParam.ExposedAsProperty = True
Catch
MsgBox("Error trying to expose the parameter as a custom iProperty!", vbCritical, "Failure")
End Try
Wesley Crihfield
(Not an Autodesk Employee)
Actually, here is a version of that last code where it will allow you to pick either type of object, then check which type you selected, then get the parameter from it. If it is neither of those two types, it will exit the rule. Then it lets you rename the parameter associated with what you picked. Then it tries to expose that as a custom iProperty.
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAllEntitiesFilter, "Select a feature or sketch dimension.")
If oObj Is Nothing Then Exit Sub
Dim oParam As Inventor.Parameter = Nothing
If TypeOf oObj Is FeatureDimension Then
Dim oFDim As FeatureDimension = oObj
oParam = oFDim.Parameter
ElseIf TypeOf oObj Is DimensionConstraint Then
Dim oDimConst As DimensionConstraint = oObj
oParam = oDimConst.Parameter
Else
Exit Sub
End If
Dim sName As String = InputBox("Edit Parameter Name", "Rename Param", oParam.Name)
If sName <> "" Then Try : oParam.Name = sName : Catch : End Try
Try
oParam.ExposedAsProperty = True
Catch
MsgBox("Error trying to expose the parameter as a custom iProperty!", vbCritical, "Failure")
End TryWesley Crihfield
(Not an Autodesk Employee)
Hi @WCrihfield
Thanks for the help
Can i ask you 1 question. It will solve a string of my problems
I have a code used to get the minimum bounding box dimensions
Instead of showing 3 sizes I want it to show notifications
Ex: 20 x 37,895 x 50
I want it to announce that: This value is 20 you will assign "Custom name"(I will input custom name value)
I want it to announce that: This value is 37,895 you will assign "Custom name"(I will input custom name value)
I want it to announce that: This value is 50 you will assign "Custom name"(I will input custom name value)
I think you can help me, you can help me
This code:
' Get the current Part document.
Dim partDoc As PartDocument = ThisDoc.Document
' Get the TransientBRep and TransientGeometry objects.
Dim transBRep As TransientBRep = ThisApplication.TransientBRep
Dim transGeom As TransientGeometry = ThisApplication.TransientGeometry
' Combine all bodies in Part into a single transient Surface Body.
Dim combinedBodies As SurfaceBody = Nothing
For Each surfBody As SurfaceBody In partDoc.ComponentDefinition.SurfaceBodies
If combinedBodies Is Nothing Then
combinedBodies = transBRep.Copy(surfBody)
Else
transBRep.DoBoolean(combinedBodies, surfBody, BooleanTypeEnum.kBooleanTypeUnion)
End If
Next
' Get the oriented mininum range box of all bodies in Part.
' NOTE: "OrientedMinimumRangeBox" was added in Inventor 2020.3/2021.
Dim minBox As OrientedBox = combinedBodies.OrientedMinimumRangeBox
' Get length of each side of mininum range box.
Dim dir1 As Double = minBox.DirectionOne.Length
Dim dir2 As Double = minBox.DirectionTwo.Length
Dim dir3 As Double = minBox.DirectionThree.Length
' Convert lengths to document's length units.
Dim uom As UnitsOfMeasure = partDoc.UnitsOfMeasure
dir1 = uom.ConvertUnits(dir1, "cm", uom.LengthUnits)
dir2 = uom.ConvertUnits(dir2, "cm", uom.LengthUnits)
dir3 = uom.ConvertUnits(dir3, "cm", uom.LengthUnits)
' Sort lengths from smallest to largest.
Dim lengths As New List(Of Double) From {dir1, dir2, dir3 }
lengths.Sort
Dim minLength As Double = lengths(0)
Dim midLength As Double = lengths(1)
Dim maxLength As Double = lengths(2)
' Create surface to represent oriented range box...
' Create starting box with dimensions of oriented rangebox.
Dim startBox As Box = transGeom.CreateBox()
Dim boxMaxPoint As Point = transGeom.CreatePoint(minBox.DirectionOne.Length, minBox.DirectionTwo.Length, minBox.DirectionThree.Length)
startBox.Extend(boxMaxPoint)
' Create transformation matrix to move box to correct location/orientation.
Dim transMatrix As Matrix = ThisApplication.TransientGeometry.CreateMatrix
transMatrix.SetCoordinateSystem(minBox.CornerPoint, minBox.DirectionOne.AsUnitVector.AsVector, minBox.DirectionTwo.AsUnitVector.AsVector, minBox.DirectionThree.AsUnitVector.AsVector)
' Create surface body for the range box.
Dim minBoxSurface As SurfaceBody = ThisApplication.TransientBRep.CreateSolidBlock(startBox)
' Transform range box surface body to the correct location/orientation.
ThisApplication.TransientBRep.Transform(minBoxSurface, transMatrix)
' Display range box on screen.
Dim transac As Transaction = ThisApplication.TransactionManager.StartTransaction(partDoc, "DisplayRangeBox")
Dim cGraphics As ClientGraphics
Try
cGraphics = partDoc.ComponentDefinition.ClientGraphicsCollection.Add("OrientedRangeBox")
Dim surfacesNode As GraphicsNode = cGraphics.AddNode(1)
Dim surfGraphics As SurfaceGraphics = surfacesNode.AddSurfaceGraphics(minBoxSurface)
Dim targetAppearance As Asset
Try
targetAppearance = partDoc.Assets.Item("Clear - Blue")
Catch
Dim sourceAppearance As Asset = ThisApplication.AssetLibraries.Item("314DE259-5443-4621-BFBD-1730C6CC9AE9").AppearanceAssets.Item("InvGen-001-1-2") ' "Clear - Blue"
targetAppearance = sourceAppearance.CopyTo(partDoc)
End Try
surfacesNode.Appearance = targetAppearance
ThisApplication.ActiveView.Update
' Display message with minimum rangebox size.
MessageBox.Show("Oriented Minimum Rangebox Size: " &
minLength.ToString("#.###") & " x " & midLength.ToString("#.###") & " x " & maxLength.ToString("#.###"),
"Oriented Minimum Rangebox", MessageBoxButtons.OK, MessageBoxIcon.Information)
Finally
' Remove range box from screen.
transac.Abort
ThisApplication.ActiveView.Update
End Try
That is a pretty long and complex rule. Since all of that geometry it creates is just transient (math only, not real), it will not have any real dimension objects or parameters that will stay after the transaction is aborted. What would we be assigning a named to? Do you simply want to customize the final message with a custom specified name for what each size represents, or do you want this rule to create 3 custom iProperties (one for each directional size), and write these values to those iProperties? Or would you prefer to create 3 user parameters? Keep in mind that if the code creates iProperties or parameters, those values will just be static, and will not actually be linked to anything real, so they will not stay accurate if something changes in the model afterwards.
Wesley Crihfield
(Not an Autodesk Employee)
i want this rule to create 3 custom iProperties (one for each directional size), and write these values to those iProperties. I know it won't change when the model changes
OK. I added this section of code to your rule, just after the 3 values have been converted and sorted, but just before it starts the 'transaction', so that they will not be removed when the transaction is aborted.
'write values to custom iProperties with prompts for names
Dim sName1, sName2, sName3 As String
sName1 = InputBox("This value is " & minLength, "Assign Property Name", "")
If sName1 <> "" Then iProperties.Value("Custom", sName1) = minLength
sName2 = InputBox("This value is " & midLength, "Assign Property Name", "")
If sName2 <> "" Then iProperties.Value("Custom", sName2) = midLength
sName3 = InputBox("This value is " & maxLength, "Assign Property Name", "")
If sName3 <> "" Then iProperties.Value("Custom", sName3) = maxLength...below is the whole thing, after that has been added in. I hope this works the way you want it to.
' Get the current Part document.
Dim partDoc As PartDocument = ThisDoc.Document
' Get the TransientBRep and TransientGeometry objects.
Dim transBRep As TransientBRep = ThisApplication.TransientBRep
Dim transGeom As TransientGeometry = ThisApplication.TransientGeometry
' Combine all bodies in Part into a single transient Surface Body.
Dim combinedBodies As SurfaceBody = Nothing
For Each surfBody As SurfaceBody In partDoc.ComponentDefinition.SurfaceBodies
If combinedBodies Is Nothing Then
combinedBodies = transBRep.Copy(surfBody)
Else
transBRep.DoBoolean(combinedBodies, surfBody, BooleanTypeEnum.kBooleanTypeUnion)
End If
Next
' Get the oriented mininum range box of all bodies in Part.
' NOTE: "OrientedMinimumRangeBox" was added in Inventor 2020.3/2021.
Dim minBox As OrientedBox = combinedBodies.OrientedMinimumRangeBox
' Get length of each side of mininum range box.
Dim dir1 As Double = minBox.DirectionOne.Length
Dim dir2 As Double = minBox.DirectionTwo.Length
Dim dir3 As Double = minBox.DirectionThree.Length
' Convert lengths to document's length units.
Dim uom As UnitsOfMeasure = partDoc.UnitsOfMeasure
dir1 = uom.ConvertUnits(dir1, "cm", uom.LengthUnits)
dir2 = uom.ConvertUnits(dir2, "cm", uom.LengthUnits)
dir3 = uom.ConvertUnits(dir3, "cm", uom.LengthUnits)
' Sort lengths from smallest to largest.
Dim lengths As New List(Of Double) From {dir1, dir2, dir3 }
lengths.Sort
Dim minLength As Double = lengths(0)
Dim midLength As Double = lengths(1)
Dim maxLength As Double = lengths(2)
'write values to custom iProperties with prompts for names
Dim sName1, sName2, sName3 As String
sName1 = InputBox("This value is " & minLength, "Assign Property Name", "")
If sName1 <> "" Then iProperties.Value("Custom", sName1) = minLength
sName2 = InputBox("This value is " & midLength, "Assign Property Name", "")
If sName2 <> "" Then iProperties.Value("Custom", sName2) = midLength
sName3 = InputBox("This value is " & maxLength, "Assign Property Name", "")
If sName3 <> "" Then iProperties.Value("Custom", sName3) = maxLength
' Create surface to represent oriented range box...
' Create starting box with dimensions of oriented rangebox.
Dim startBox As Box = transGeom.CreateBox()
Dim boxMaxPoint As Point = transGeom.CreatePoint(minBox.DirectionOne.Length, minBox.DirectionTwo.Length, minBox.DirectionThree.Length)
startBox.Extend(boxMaxPoint)
' Create transformation matrix to move box to correct location/orientation.
Dim transMatrix As Matrix = ThisApplication.TransientGeometry.CreateMatrix
transMatrix.SetCoordinateSystem(minBox.CornerPoint, minBox.DirectionOne.AsUnitVector.AsVector, minBox.DirectionTwo.AsUnitVector.AsVector, minBox.DirectionThree.AsUnitVector.AsVector)
' Create surface body for the range box.
Dim minBoxSurface As SurfaceBody = ThisApplication.TransientBRep.CreateSolidBlock(startBox)
' Transform range box surface body to the correct location/orientation.
ThisApplication.TransientBRep.Transform(minBoxSurface, transMatrix)
' Display range box on screen.
Dim transac As Transaction = ThisApplication.TransactionManager.StartTransaction(partDoc, "DisplayRangeBox")
Dim cGraphics As ClientGraphics
Try
cGraphics = partDoc.ComponentDefinition.ClientGraphicsCollection.Add("OrientedRangeBox")
Dim surfacesNode As GraphicsNode = cGraphics.AddNode(1)
Dim surfGraphics As SurfaceGraphics = surfacesNode.AddSurfaceGraphics(minBoxSurface)
Dim targetAppearance As Asset
Try
targetAppearance = partDoc.Assets.Item("Clear - Blue")
Catch
Dim sourceAppearance As Asset = ThisApplication.AssetLibraries.Item("314DE259-5443-4621-BFBD-1730C6CC9AE9").AppearanceAssets.Item("InvGen-001-1-2") ' "Clear - Blue"
targetAppearance = sourceAppearance.CopyTo(partDoc)
End Try
surfacesNode.Appearance = targetAppearance
ThisApplication.ActiveView.Update
' Display message with minimum rangebox size.
MessageBox.Show("Oriented Minimum Rangebox Size: " &
minLength.ToString("#.###") & " x " & midLength.ToString("#.###") & " x " & maxLength.ToString("#.###"),
"Oriented Minimum Rangebox", MessageBoxButtons.OK, MessageBoxIcon.Information)
Finally
' Remove range box from screen.
transac.Abort
ThisApplication.ActiveView.Update
End Try
Wesley Crihfield
(Not an Autodesk Employee)
