Rectangular Pattern of Feature in Part - C# or .NET Example

[Anonymous]

Hello,

I'm programming my first Add-In for Inventor 2017 in C#.

The purpose of the Add-in is to create a steel grate. I already have the rectangle with 1 "grate". But now I have to create a rectangular pattern.

But here I'm stuck, I can't find any example that makes any sense.

I tried to make an objectcollection of the grate extrusion feature, and add this to a rectangularpatternfeature.

But I'm not making any progress. Could someone help me out?

  private void btn_create_Click(object sender, EventArgs e)
        {
            #region CREATE PART + GET UNIQUE FILENUMBER + SAVE PART
            PartDocument oPartDoc = (PartDocument)_invApp.Documents.Add(DocumentTypeEnum.kPartDocumentObject, _invApp.FileManager.GetTemplateFile(DocumentTypeEnum.kPartDocumentObject), true);

            try
            {
                StandardAddInServer.VLT_Conn = StandardAddInServer.LogMeInVault();
                if (StandardAddInServer.VLT_Conn != null)
                {
                    Autodesk.DataManagement.Client.Framework.Currency.FolderPathAbsolute fld = null;
                    fld = StandardAddInServer.VLT_Conn.WorkingFoldersManager.GetWorkingFolder("$");
                    StandardAddInServer.VLT_WorkingFolder = fld.FullPath;
                }
            }
            catch { StandardAddInServer.VLT_Conn = null; }
            if (StandardAddInServer.VLT_Conn == null)
            {
                MessageBox.Show("Gelieve u eerst in vault aan te melden!", "Foutmelding", MessageBoxButtons.OK, MessageBoxIcon.Exclamation);
                return;
            }
            string fileNumber = StandardAddInServer.FileNumber();
            string saveLocationPart = StandardAddInServer.fileLoc.Replace(System.IO.Path.GetFileName(StandardAddInServer.fileLoc), "PT" + fileNumber + ".ipt");

            #region SetProperties Iterate

            Inventor.Document doc = _invApp.ActiveDocument;
            Inventor.PropertySets oPropertySets;
            oPropertySets = doc.PropertySets;

            foreach (PropertySet oPropertySet in oPropertySets)
            {

                if (oPropertySet.DisplayName.ToLower() == "design tracking properties")
                {
                    foreach (Property oProperty in oPropertySet)
                    {
                        if (oProperty.DisplayName == oPropertySet.ItemByPropId[(int)PropertiesForDesignTrackingPropertiesEnum.kDescriptionDesignTrackingProperties].DisplayName)
                        {
                            oProperty.Value = txt_omsch.Text;
                            doc.DisplayName = txt_omsch.Text;
                            doc.DisplayNameOverridden = true;
                        }
                        else if (oProperty.DisplayName == oPropertySet.ItemByPropId[(int)PropertiesForDesignTrackingPropertiesEnum.kPartNumberDesignTrackingProperties].DisplayName)
                        {
                            oProperty.Value = txt_afm.Text;
                        }
                    }
                }
                else if (oPropertySet.DisplayName.ToLower() == "summary information")
                {
                    foreach (Property oProperty in oPropertySet)
                    {
                        if (oProperty.DisplayName == oPropertySet.ItemByPropId[(int)PropertiesForSummaryInformationEnum.kSubjectSummaryInformation].DisplayName)
                        {
                            oProperty.Value = txt_afm.Text;
                        }
                    }
                }
            }
            #endregion

            oPartDoc.SaveAs(saveLocationPart, false);

            #endregion

            #region DRAW ROOSTER

            TransientGeometry oTG = _invApp.TransientGeometry;
            PartComponentDefinition oCompDef = oPartDoc.ComponentDefinition;

            Point2d[] oPoints = new Point2d[4];

            oPoints[0] = oTG.CreatePoint2d(0, 0);
            oPoints[1] = oTG.CreatePoint2d(calcWidth / 10, 0);
            oPoints[2] = oTG.CreatePoint2d(calcWidth / 10, calcLength / 10);
            oPoints[3] = oTG.CreatePoint2d(0, calcLength / 10);

            PlanarSketch oSketch = oCompDef.Sketches.Add(oCompDef.WorkPlanes[3]);
            SketchLine[] oLines = new SketchLine[4];

            oLines[0] = oSketch.SketchLines.AddByTwoPoints(oPoints[0], oPoints[1]);
            oLines[1] = oSketch.SketchLines.AddByTwoPoints(oLines[0].EndSketchPoint, oPoints[2]);
            oLines[2] = oSketch.SketchLines.AddByTwoPoints(oLines[1].EndSketchPoint, oPoints[3]);
            oLines[3] = oSketch.SketchLines.AddByTwoPoints(oLines[2].EndSketchPoint, oLines[0].StartSketchPoint);

            Profile oProfile = oSketch.Profiles.AddForSolid();

            oProfile.AttributeSets[0].Name = "Length";

            ExtrudeFeature oExtrude = oCompDef.Features.ExtrudeFeatures.AddByDistanceExtent(oProfile, cb_rdikte.SelectedItem, PartFeatureExtentDirectionEnum.kNegativeExtentDirection, PartFeatureOperationEnum.kNewBodyOperation, 0);


            MessageBox.Show(oExtrude.FeatureDimensions.Count.ToString());

            oExtrude.FeatureDimensions[1].Parameter.Name = "DikteRooster";
            oExtrude.FeatureDimensions[2].Parameter.Name = "TaperAngleRooster";

            oSketch = oCompDef.Sketches.AddWithOrientation(oExtrude.StartFaces[1], oCompDef.WorkAxes[1], true, true, oCompDef.WorkPoints[1], false);
            oSketch.SketchLines.AddAsTwoPointRectangle(oTG.CreatePoint2d(0.7, 0.7), oTG.CreatePoint2d(3.8, 3.8));

            oProfile = oSketch.Profiles.AddForSolid();
            oExtrude = oCompDef.Features.ExtrudeFeatures.AddByDistanceExtent(oProfile, cb_rdikte.Text, PartFeatureExtentDirectionEnum.kNegativeExtentDirection, PartFeatureOperationEnum.kCutOperation, 0);

            oExtrude.FeatureDimensions[1].Parameter.Name = "MaasExtrudeDikte";
            oExtrude.FeatureDimensions[2].Parameter.Name = "TaperAngleMazen";
            oExtrude.Name = "Mazen";

            #endregion

            #region CREATE PATTERN

            ObjectCollection objColFeatures = _invApp.TransientObjects.CreateObjectCollection();
            objColFeatures.Add(oCompDef.Features.ExtrudeFeatures[2]);

            RectangularPatternFeature oRectFeature = oCompDef.Features.RectangularPatternFeatures.AddByDefinition();
            

            #endregion


            oPartDoc.Update();
            oPartDoc.Save();

            this.Close();
        }

Thanks in advance

[dgreatice · Accepted solution]

Hi,

http://help.autodesk.com/view/INVNTOR/2018/ENU/?guid=GUID-6D6F1140-F264-42E2-A0DB-4C967742267E

My example solution, but I'm using inventor 2014 and VBA:

https://forums.autodesk.com/t5/inventor-customization/rectangular-pattern-part-ilogic/m-p/7599859#M7...

When I see API inventor 2017 there are difference:

RectangularPatternFeatures.AddByDefinition(....) or

RectangularPatternFeatures.CreateDefinition(....) <-- Same like my example

but in inventor 2014:

Dim RecFeat as RectangularPatternFeatures

set RecFeat  = ....RectangularPatternFeatures.Add(...)

Maybe you can find any clue from my example.

[Anonymous · Accepted solution]

Hello,

Thanks for the push in the right direction.

This is what I came up with:

#region CREATE PATTERN
            ObjectCollection oObjColl = _invApp.TransientObjects.CreateObjectCollection();
            oObjColl.Add(oExtrude);
            RectangularPatternFeatureDefinition oRecFeatDef = oCompDef.Features.RectangularPatternFeatures.CreateDefinition(oObjColl, oCompDef.WorkAxes[1], true, 5, 3.8, PatternSpacingTypeEnum.kDefault);
            RectangularPatternFeature oRecFeat = oCompDef.Features.RectangularPatternFeatures.AddByDefinition(oRecFeatDef);         
#endregion

Now I just have to find out how to create a pattern in two directions