Mod the Machine

C# Help Examples for Parts General

Here are the VBA examples in this section of samples for parts converted to C#. This group of examples includes an example for an event (TestSelection) that allows you to get an entity from the user using events. It also has some parameter and brep examples. The WorkPointAtMassCenter c# example was already in the help file. (Saved me some time converting it).

This project has the following functions.

 Download InventorHelpExamples_Part_General

CreateParametersAndGroup
MoldBaseSample
SelectivelyLinkParams
QueryAndShowFeatureDimensions
TestSelection
IsCylindricalFaceInterior
GetPartMassProps
GetPartMassPropsWithoutDirtying
WorkPointAtMassCenter
CreateMaterial
ShowMaterials
ModelParameters
TableParameters
CreateRectangleFace

 

Here is the CreateParametersAndGroup function:

// Creating a new parameter group API Sample

//Description

//This sample demonstrates the creation of model,

//reference and user parameters and

//copying these parameters to a newly created group.

public void CreateParametersAndGroup()

{

    // Create a new Part document.

    PartDocument oPartDoc = default(PartDocument);

    oPartDoc =

      (PartDocument)ThisApplication.Documents.Add

    (DocumentTypeEnum.kPartDocumentObject,

    ThisApplication.FileManager.GetTemplateFile

    (DocumentTypeEnum.kPartDocumentObject));

 

    // Set a reference to the compdef.

    PartComponentDefinition oCompDef =

        default(PartComponentDefinition);

    oCompDef = oPartDoc.ComponentDefinition;

 

    // Create a model parameter

    ModelParameter oModelParam =

                  default(ModelParameter);

    oModelParam = oCompDef.Parameters.

    ModelParameters.AddByValue

    (2, UnitsTypeEnum.kCentimeterLengthUnits);

 

    // Create a reference parameter

    ReferenceParameter oReferenceParam =

    default(ReferenceParameter);

    oReferenceParam = oCompDef.Parameters.

    ReferenceParameters.AddByValue

    (4, UnitsTypeEnum.kCentimeterLengthUnits);

 

    // Create a user parameter

    UserParameter oUserParam =

                       default(UserParameter);

    oUserParam = oCompDef.Parameters.UserParameters.

             AddByValue("length", 6,

              UnitsTypeEnum.kCentimeterLengthUnits);

 

    // Create a new custom parameter group

    CustomParameterGroup oCustomParamGroup =

    default(CustomParameterGroup);

    oCustomParamGroup = oCompDef.Parameters.

             CustomParameterGroups.Add

                ("Custom Group", "CustomGroup1");

 

    // Add the created parameters to this group

    // Note that adding the parameters to the

    //custom group does not remove it from the

    // original group.

    oCustomParamGroup.Add((Parameter)oModelParam);

    oCustomParamGroup.Add

                     ((Parameter)oReferenceParam);

    oCustomParamGroup.Add((Parameter)oUserParam);

}

C# Help Examples for Features – Part 2

Here is the second group of VBA examples in this section of samples for features converted to C#. The project with the first set of converted samples for features is here.

This project has the following functions.

 Download InventorHelpExamples_Features_2

HoleFeatureLinearPlacement
StitchFeatureCreate
CreateNonPlanarSectionLoft
EditExtrudeFeature
SweepFeature
TrueSweepLength
ThreadSample
EditThread
test_threadinfo

Here is HoleFeatureLinearPlacement function:

//    Hole feature linear placement API Sample

//Description

//This sample demonstrates the creation of a

//hole feature using the linear placement type.

public void HoleFeatureLinearPlacement()

{

    // Create a new part document, using the

    //default part template.

    PartDocument oPartDoc = default(PartDocument);

    oPartDoc = (PartDocument)ThisApplication.

        Documents.Add

            (DocumentTypeEnum.kPartDocumentObject,

      ThisApplication.FileManager.GetTemplateFile

        (DocumentTypeEnum.kPartDocumentObject));

 

    // Set a reference to the component definition.

    PartComponentDefinition oCompDef =

                  default(PartComponentDefinition);

    oCompDef = oPartDoc.ComponentDefinition;

 

    // Create a new sketch on the X-Y work plane.

    PlanarSketch oSketch = default(PlanarSketch);

    oSketch = oCompDef.Sketches.Add

                        (oCompDef.WorkPlanes[3]);

 

    // Set a reference to the

    //transient geometry object.

    TransientGeometry oTransGeom =

                        default(TransientGeometry);

    oTransGeom = ThisApplication.TransientGeometry;

 

    // Create a square on the sketch.

    oSketch.SketchLines.AddAsTwoPointRectangle

        (oTransGeom.CreatePoint2d(0, 0),

        oTransGeom.CreatePoint2d(6, 6));

 

    // Create the profile.

    Profile oProfile = default(Profile);

    oProfile = oSketch.Profiles.AddForSolid();

 

    // Create an extrusion.

    ExtrudeDefinition oExtrudeDef =

                    default(ExtrudeDefinition);

    oExtrudeDef = oCompDef.Features.

        ExtrudeFeatures.CreateExtrudeDefinition

                                     (oProfile,

       PartFeatureOperationEnum.kJoinOperation);

    oExtrudeDef.SetDistanceExtent("2 cm",

               PartFeatureExtentDirectionEnum.

                      kNegativeExtentDirection);

    ExtrudeFeature oExtrude =

                         default(ExtrudeFeature);

    oExtrude = oCompDef.Features.ExtrudeFeatures.

                                Add(oExtrudeDef);

 

    // Get the start face of the extrude.

    Face oFace = default(Face);

    oFace = oExtrude.StartFaces[1];

 

    // Get two adjacent edges on the start face.

    Edge oEdge1 = default(Edge);

    Edge oEdge2 = default(Edge);

    oEdge1 = oFace.Edges[1];

    oEdge2 = oFace.Edges[2];

 

    // Create a bias point for hole placement to

    //place it at the expected location. This is

    //the model point corresponding to the center

    //of the square in the sketch.

    Inventor.Point oBiasPoint =

                        default(Inventor.Point);

    oBiasPoint = oSketch.SketchToModelSpace

            (oTransGeom.CreatePoint2d(1.5, 1.5));

 

    // Create the hole feature placement definition.

    LinearHolePlacementDefinition oLinearPlacementDef

            = default(LinearHolePlacementDefinition);

    oLinearPlacementDef = oCompDef.Features.

    HoleFeatures.CreateLinearPlacementDefinition

        (oFace, oEdge1, "2 cm",

                         oEdge2, "2 cm", oBiasPoint);

 

    // Create the hole feature.

    oCompDef.Features.HoleFeatures.

        AddDrilledByThroughAllExtent

        (oLinearPlacementDef, "1 cm",

            PartFeatureExtentDirectionEnum.

                     kPositiveExtentDirection);

}

C# Help Examples for Features – Part 1

Here is the first group of VBA examples in this section of samples for Features converted to C#.

This project has the following functions.

 Download InventorHelpExamples_Features_1

BoundaryPatchFeature
DecalFeature
DrawBlockWithPocket
EditFeatureProfile
ExtrudeSketchText
CreateAllRoundsFillet
CreateFilletComplex
CreateSimpleFillet
HighlightFeatureFaces
ClearHighlight

Here is CreateSimpleFillet

//    Fillet Feature (Simple) API Sample

//Description

//This sample demonstrates using the AddSimple method

//of the FilletFeatures collection

// to create a constant radius fillet.

public void CreateSimpleFillet()

{

    // Create a new Part document.

    PartDocument oPartDoc = default(PartDocument);

    oPartDoc =

     (PartDocument)ThisApplication.Documents.Add

           (DocumentTypeEnum.kPartDocumentObject,

     ThisApplication.FileManager.GetTemplateFile

         (DocumentTypeEnum.kPartDocumentObject));

 

    // Set a reference to the compdef.

    PartComponentDefinition oCompDef =

             default(PartComponentDefinition);

    oCompDef = oPartDoc.ComponentDefinition;

 

    // Create a sketch on the xy work plane.

    PlanarSketch oSketch = default(PlanarSketch);

    oSketch = oCompDef.Sketches.Add

                        (oCompDef.WorkPlanes[3]);

 

    // Draw a rectangle.

    oSketch.SketchLines.AddAsTwoPointRectangle

    (ThisApplication.TransientGeometry.

                           CreatePoint2d(-6, -4),

   ThisApplication.TransientGeometry.

                            CreatePoint2d(6, 4));

 

    Profile oProfile = default(Profile);

    oProfile = oSketch.Profiles.AddForSolid();

 

    // Create an extrusion.

    ExtrudeDefinition oExtrudeDef =

                   default(ExtrudeDefinition);

    oExtrudeDef = oCompDef.Features.

         ExtrudeFeatures.CreateExtrudeDefinition

(oProfile, PartFeatureOperationEnum.kJoinOperation);

 

    oExtrudeDef.SetDistanceExtent

             (5, PartFeatureExtentDirectionEnum.

                      kSymmetricExtentDirection);

 

    ExtrudeFeature oExtrude =

                          default(ExtrudeFeature);

    oExtrude = oCompDef.Features.

                  ExtrudeFeatures.Add(oExtrudeDef);

 

    // Define the set of edges that are for the start

    //and end faces of the solid.

    EdgeCollection oEdges =

                    default(EdgeCollection);

    oEdges = ThisApplication.TransientObjects.

                             CreateEdgeCollection();

 

    foreach (Edge oEdge in oExtrude.

                               StartFaces[1].Edges)

    {

        oEdges.Add(oEdge);

    }

 

    foreach (Edge oEdge in oExtrude.

                                EndFaces[1].Edges)

    {

        oEdges.Add(oEdge);

    }

 

    // Create the fillet feature.

    FilletFeature oFillet = default(FilletFeature);

    oFillet = oCompDef.Features.FilletFeatures.

                              AddSimple(oEdges, 1);

}

- Wayne

C# Help Examples for sketch – Part 2

Here is the second installment of VBA examples converted to C#. This project has the following functions. (converted from VBA   procedures in the help file). This blog post has the other examples in the help section on 2D Sketches.

 Download InventorHelpExamples_Sketch_2

Offset
DrawSketchLine
ToggleSketchVisibility
CreateSketchBlockDefinition
InsertSketchBlockDefinition
CreateSketchBlock
CreateSketchedSymbolDefinition
InsertSketchedSymbolOnSheet
AddSymbolWithLeader
DrawSketchEllipticalArc
SketchEntities
SplineByDefinition
DrawSketchSpline
CopyBodyFromPartToPart

Here is the Offset example:

//  Offset a 2D sketch API Sample

//Description

//This sample demonstrates the creation of offsets

//in 2d sketches. Two ways of creating the offset

//are shown - one uses a distance and the other

//uses the input point.

public void Offset()

{

    // Check to make sure a sketch is open.

    // Set a reference to the active sketch.

    PlanarSketch oSketch = default(PlanarSketch);

    try

    {

        Object actObj =

              ThisApplication.ActiveEditObject;

        oSketch = (PlanarSketch)actObj;

 

    }

    catch

    {

        MessageBox.Show("A sketch must be active.");

        return;

    }

 

    // Reference the transient geometry collection.

    TransientGeometry oTransGeom =

                        default(TransientGeometry);

    oTransGeom = ThisApplication.TransientGeometry;

 

    // Create a rectangle

    SketchEntitiesEnumerator oRectangleLines =

        default(SketchEntitiesEnumerator);

    oRectangleLines = oSketch.SketchLines.

        AddAsTwoPointRectangle(oTransGeom.

        CreatePoint2d(0, 0),

        oTransGeom.CreatePoint2d(10, -10));

 

    // Create a new object collection

    ObjectCollection oCollection =

                      default(ObjectCollection);

    oCollection = ThisApplication.TransientObjects.

                          CreateObjectCollection();

 

    // Add the first sketch line of the rectangle

    // to the collection

    oCollection.Add(oRectangleLines[1]);

 

    // Create a point at (0,3). The entity resulting

    // from the offset of the first sketch line must

    // pass thru this point.

    Point2d oOffsetPoint = default(Point2d);

    oOffsetPoint = oTransGeom.CreatePoint2d(0, 3);

 

    // Create an offset rectangle using the

    // offset point.

    oSketch.OffsetSketchEntitiesUsingPoint

        (oCollection, oOffsetPoint, true);

 

    // Get the sketch normal

    UnitVector oNormalVector = default(UnitVector);

    oNormalVector = oSketch.PlanarEntityGeometry.Normal;

 

    // Get the direction of sketch line being offset

    SketchEntity oSkEnt = oRectangleLines[1];

 

    // Get the geometry associated with the sketch

    // entity. Since the Geometry property will

    // return one of various types of objects,

    // we need to use late binding here

    // which C# doesn't

    // handle very nicely.

    object geom = oSkEnt.GetType().

           InvokeMember("Geometry",

            BindingFlags.GetProperty,

                 null, oSkEnt, null);

 

        UnitVector2d oLineDir =

            (UnitVector2d)geom.GetType().

                   InvokeMember("Direction",

        BindingFlags.GetProperty, null, geom, null);

 

    UnitVector oLineVector = default(UnitVector);

    oLineVector = oTransGeom.CreateUnitVector

                    (oLineDir.X, oLineDir.Y, 0);

 

    // The cross product of these vectors is the

    // natural offset direction for the sketch line.

    UnitVector oOffsetVector = default(UnitVector);

    oOffsetVector = oLineVector.

                       CrossProduct(oNormalVector);

 

    // Get the desired offset vector (the +ve y-axis)

    UnitVector oDesiredVector = default(UnitVector);

    oDesiredVector = oTransGeom.

                          CreateUnitVector(0, 1, 0);

 

    bool bNaturalOffsetDir = false;

 

    if (oOffsetVector.IsEqualTo(oDesiredVector))

    {

        bNaturalOffsetDir = true;

    }

    else

    {

        bNaturalOffsetDir = false;

    }

 

    // Create an offset at a distance of 6 cms.

    oSketch.OffsetSketchEntitiesUsingDistance

        (oCollection, 6, bNaturalOffsetDir, true);

}

- Wayne

C# Help Examples for sketch – Part 1

One of the takeaways from the Inventor API survey results this year was the request for help file examples in other languages besides VBA. To help address this, I am planning on converting the samples to C# over the next several months. Here is the first installment.

Download InventorHelpExamples_Sketch_1 

In this project you will find these VBA Procedures converted to C# functions:

CopySketch
SilhouetteSample
ChangeSketchPlane
MakeSketchShared
AddSketch
AddOrientedSketch
GetProfileRegionProperties
SketchProfileControl
CopySketchContents
DeferSketchUpdate
DeleteSketch
StartSketchEdit       
MoveSketchObjects

This is 13 out of the 26 examples in this group of examples on Sketches. (The next post on this topic will be the others in this section).

When you run this stand alone Windows Forms project you will see a combo box with a list of the examples. Click on one you want to run.

 

- Wayne

Set “Embed Interop Types” to False to avoid problems with events

We have had several cases recently where events such as OnFileSaveAsDialog were not working properly. Problems with events can occur if the property “Embeding Interop Types” of the referenced Inventor Interop is set to True. This setting is new in Visual Studio 2010 with .NET 4 and it defaults to True. If you change the setting to False and rebuild the events work normally.

Here is a screenshot of the properties window in VB.NET. 

-Wayne