The hole pattern is not at uniform length radially

[2019mmp003]

Hi all,

When I am using the circular pattern feature, pattern is getting created but the holes are not placed at equidistance.

As you can see each hole is not equidistant radially from other hole.

But I want the result as this.

// The code for reference is as below

//holy = 28, oangle = 2*pi

// What should be error so that I get result shown in first image. Whereas I want the result shown // in second image

CircularPatternFeatureDefinition pattern1;
pattern1=oPartCompDef.Features.CircularPatternFeatures.CreateDefinition(bodyCollection,oPartCompDef.WorkAxes[3],true,holy,oangle,false);
CircularPatternFeature          pa=oPartCompDef.Features.CircularPatternFeatures.AddByDefinition(pattern1);

[FINET_Laurent]

Morning,

I think Inventor is using radians.

Maybe try to convert your angle (in degrees) to radian, by doing a * (pi/180)

Regards,

FINET L.

[2019mmp003]

I tried both angle in degrees and also radians. But still the problem is there.

[FINET_Laurent]

Maybe the issue is with the angle itself ?

How did you calculate the angle ?

I'd do 360/holes number then try both angles (deg and rad)

Regards,

FINET L.

[2019mmp003]

No, I tried both angles i.e(total 360 angle and angle between two consecutive holes) also both in degrees and radians. But still it didnot work.

[FINET_Laurent]

é_è

Can you share the files ?

[2019mmp003]

double outerDia = Convert.ToDouble(outerdiameter.Text);
double outerHoleDia = Convert.ToDouble(outerholediameter.Text);
double innerHoleDia = Convert.ToDouble(innerholediameter.Text);
double innerDia = Convert.ToDouble(outerdiameter.Text) - 2 *
(Convert.ToDouble(Thickness.Text));
double biggerDia = findBiggerHole(outerHoleDia, innerHoleDia);
double crossSectionAreaOfCage = (22 / 28) * innerDia * innerDia;
double height = Convert.ToDouble(cageheight.Text);
int noOfHolesAlongCageHeight = (int)((height - biggerDia) / (biggerDia * 2) + 0.5);

int totalNoOfHoles = (int)((innerDia*innerDia)/(biggerDia*biggerDia));
int noOfHolesRadially = totalNoOfHoles / noOfHolesAlongCageHeight;
double angle = 360.0 / noOfHolesRadially;
angle = (angle * Math.PI) / 180;

Inventor.Application inventorApplication;
inventorApplication = (Inventor.Application)
Marshal.GetActiveObject("Inventor.Application");
PartDocument partDoc;
partDoc = (PartDocument)inventorApplication.Documents.Add
(DocumentTypeEnum.kPartDocumentObject,
inventorApplication.FileManager.GetTemplateFile
(DocumentTypeEnum.kPartDocumentObject));

PartComponentDefinition oPartCompDef;
oPartCompDef = partDoc.ComponentDefinition;

PlanarSketch oSketch;
oSketch = oPartCompDef.Sketches.Add(oPartCompDef.WorkPlanes[3]);

TransientGeometry oTransGeom;
oTransGeom = inventorApplication.TransientGeometry;


SketchCircle outerCircle,innerCircle;

outerCircle = oSketch.SketchCircles.AddByCenterRadius(oTransGeom.CreatePoint2d(0, 0),
Convert.ToDouble(outerdiameter.Text)/2);
innerCircle = oSketch.SketchCircles.AddByCenterRadius(oTransGeom.CreatePoint2d(0, 0),
(Convert.ToDouble(outerdiameter.Text) / 2)-
Convert.ToDouble(Thickness.Text));
Profile oProfile;
oProfile = oSketch.Profiles.AddForSolid();

ExtrudeDefinition oExtrudeDef;
oExtrudeDef = oPartCompDef.Features.ExtrudeFeatures.
CreateExtrudeDefinition(oProfile,
PartFeatureOperationEnum.kJoinOperation);
oExtrudeDef.SetDistanceExtent(Convert.ToDouble(cageheight.Text)
, PartFeatureExtentDirectionEnum.kPositiveExtentDirection);
ExtrudeFeature oExtrude;
oExtrude = oPartCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef);

WorkPlane outerHolePlane;
outerHolePlane = oPartCompDef.WorkPlanes.AddByPlaneAndOffset(oPartCompDef.
WorkPlanes[1], Convert.ToDouble(outerdiameter.Text)/2);
WorkPlane innerHolePlane;
innerHolePlane = oPartCompDef.WorkPlanes.AddByPlaneAndOffset(oPartCompDef.
WorkPlanes[1], innerDia/2);

PlanarSketch Sketch1;
Sketch1 = oPartCompDef.Sketches.Add(outerHolePlane);

List<SketchCircle> holes = new List<SketchCircle>(new SketchCircle[noOfHolesAlongCageHeight]);
double first = biggerDia;
for(int i=0;i<1;i++)
{
holes[i] = Sketch1.SketchCircles.AddByCenterRadius(oTransGeom.CreatePoint2d(0,first),
outerHoleDia / 2);
first = first + 2*biggerDia;
}

Profile newProfile;
newProfile = Sketch1.Profiles.AddForSolid();

ExtrudeDefinition newExtrudeDef;
newExtrudeDef = oPartCompDef.Features.ExtrudeFeatures.
CreateExtrudeDefinition(newProfile,
PartFeatureOperationEnum.kCutOperation);
newExtrudeDef.SetDistanceExtent(Convert.ToDouble(depth.Text),
PartFeatureExtentDirectionEnum.kNegativeExtentDirection);

ExtrudeFeature newExtrude;
newExtrude = oPartCompDef.Features.ExtrudeFeatures.Add(newExtrudeDef);

PlanarSketch Sketch2;
Sketch2 = oPartCompDef.Sketches.Add(innerHolePlane);

List<SketchCircle> innerHoles = new List<SketchCircle>(new SketchCircle[noOfHolesAlongCageHeight]);
double second = biggerDia;
for (int i = 0; i < 1; i++)
{
innerHoles[i] = Sketch2.SketchCircles.AddByCenterRadius(oTransGeom.CreatePoint2d(0,second),
innerHoleDia / 2);
second = second + 2 * biggerDia;
}

Profile newsProfile;
newsProfile = Sketch2.Profiles.AddForSolid();

ExtrudeDefinition newsExtrudeDef;
newsExtrudeDef = oPartCompDef.Features.ExtrudeFeatures.
CreateExtrudeDefinition(newsProfile,
PartFeatureOperationEnum.kCutOperation);

newsExtrudeDef.SetDistanceExtent(Convert.ToDouble(depth.Text),
PartFeatureExtentDirectionEnum.kSymmetricExtentDirection);

ExtrudeFeature newsExtrude;
newsExtrude = oPartCompDef.Features.ExtrudeFeatures.Add(newsExtrudeDef);

ObjectCollection bodyCollection;
bodyCollection = inventorApplication.TransientObjects.CreateObjectCollection();

foreach (ExtrudeFeature item in oPartCompDef.Features.ExtrudeFeatures)
{
if ((item.Name == "Extrusion2") || (item.Name == "Extrusion3"))
bodyCollection.Add(item);

}

//bodyCollection.Add("Extrusion2");
innerHolePlane.Visible = false;
outerHolePlane.Visible = false;
object holy = noOfHolesRadially;
object oangle = 2 *Math.PI;

CircularPatternFeatureDefinition pattern1;
pattern1 = oPartCompDef.Features.CircularPatternFeatures.CreateDefinition(bodyCollection,oPartCompDef.WorkAxes[3],true,
holy,angle,false);
CircularPatternFeature pa = oPartCompDef.Features.CircularPatternFeatures.AddByDefinition(pattern1);

[FINET_Laurent]

If I'm not mistaken it might come from this?

double angle = 360.0 / noOfHolesRadially;
angle = (angle * Math.PI) / 180;

What if you try

double  angle  = 6,28 / noOfHolesRadially

and delete the second line : angle = (angle * Math.PI) / 180;

If it's not it I don't know.. 😞

Regards,

FINET L.

[2019mmp003]

Still has the same problem. Thanks Anyways

[JhoelForshav]

@2019mmp003 

There's a bug with the angle parameter when creating circular pattern. The easiest way is to just set its value again.

You can do something like this right after the pattern has been created:

Dim oDegParam As ModelParameter
oDegParam = oPartCompDef.Parameters.ModelParameters(oPartCompDef.Parameters.ModelParameters.Count) 'Get last parameter which will be the angle parameter
oDegParam.Expression = "360 deg" 'Set the angle again do to a bug

I know this is VB.NET but I think you'll be able to translate it to C#

[2019mmp003]

@JhoelForshav  

Thanks for your solution.

Please can you convert it into C#, I am beginner at Inventor Customization. I tried the code as you wrote in VB  as such

The error is - 'Non Invocable member Parameters.ModelParameters cannot be used like a method'.

[JhoelForshav · Accepted solution]

@2019mmp003 

In C# index should be in brackets instead of parentheses. To be honest I'm not very good at C# but I tried this and it works 🙂

ModelParameter oDegParam;
oDegParam = oPartCompDef.Parameters.ModelParameters[oPartCompDef.Parameters.ModelParameters.Count];
oDegParam.Expression = "360 deg";
partDoc.Update();

[JhoelForshav]

@2019mmp003 

I also noticed that you have set your last argument (FitWithinAngle) to false in CircularPatternFeatures.CreateDefinition. If you want your occurrences spread evenly over the angle it should be set to true.

I think you'll get your desired result with this code:

CircularPatternFeatureDefinition pattern1;
pattern1 = oPartCompDef.Features.CircularPatternFeatures.CreateDefinition(bodyCollection, oPartCompDef.WorkAxes[3], True, holy, angle, True);
CircularPatternFeature pa = oPartCompDef.Features.CircularPatternFeatures.AddByDefinition(pattern1);

ModelParameter oDegParam;
oDegParam = oPartCompDef.Parameters.ModelParameters[oPartCompDef.Parameters.ModelParameters.Count];
oDegParam.Expression = "360 deg";
partDoc.Update();

[2019mmp003]

@JhoelForshav  Thankyou so much. You are genius. It worked.