I was trying to do calculations on an odd shape earlier and I noticed something odd about how the region properties in sketches works. Ix and Iy appear to be calculated at the centroid but at an angle to the sketch axes (whatever the principle axes is). Ixx and Iyy are calculated from the sketch origin following the sketch axes. However the centroid has to be on the sketch origin for those values to be correct.
For a tube or symmetrical part drawn around the origin none of that matters as Ix and Ixx would be the same, but for an odd shape Ixx depends on the centroids relation to the origin and Ix depends on what the principle axes is.
Is there a simple way to get Inventor to calculate Ix/Iy about the centroid without having to move the part so the centroid is on the origin? I would like if the Ix/Iy calculation was in relation to the sketch axes instead of the principle axes, since I can't see the reason you'd want Ix/Iy on the principle axes.
Could you apply the parallel axis theorem to quickly calculate your inertia tensors about an axis of your choosing?
There is no automated tool that I'm aware of. This would make a good IdeaStation request for a new feature. However, there are API commands for the Region Properties. You may be able to write an ilogic code that utilizes the API command that would automatically calculate those inertia tensors about the centroid.
For clarity, I will go through an example. The below image is the Region Properties when the section has been rotated and centered on the Principal Axis, the axis through which rotational symmetry is obtained. This screenshot is mostly for reference. Note that Ixx and Iyy have the same values as Ix and Iy.
Next I have rotated the section to align with the default work axis and origin, but I have centered the section on the Centroid. Note that the "Centroid, with respect to Sketch Origin" values are 0 for X and Y. Also, note that the Ixx/Iyy values no longer match Ix and Iy, since they are being calculated with respect to the Sketch Origin to which they have been aligned.
Next, I will move the section 10 inches above the X axis. Since I know:
Ixx = 5.282 in^2
d = 10 in
Area = 2.089 in^2
Inewxx = Ixx + d^2 * A = 214.182 in^4
Result is that the new Ixx value is 214.198 in^4. The difference (214.198 - 214.182 = .016 or .00746972 % Error ) is due to the difference in precision Inventor and I used to calculate the results.
To get a better idea of the API commands, you can Help drop down menu > Community Resources > Programming Help and search for RegionProperties Object. There is a sample for querying a sketch profile to get regions that should be a good start.
Let me know if this helps or if you have any questions.
I took a crack at some code that should get you started. This ilogic code will apply the parallel axis theorem about the centroid automatically for you. I must warn you that I haven't tested this code extensively, but it seems to work for the simple example that I demonstrated earlier.
Please review and let me know if you have any questions. Hope this helps. Thanks!
'Check that sketch is active If TypeOf ThisApplication.ActiveEditObject Is Sketch Then 'Do Nothing Else MessageBox.Show("A sketch must be active with a closed profile.", "WARNING") Return End If ' a reference to the active sketch. ' This assumes a 2D sketch is active. Dim oSketch As Sketch oSketch = ThisApplication.ActiveEditObject Dim oRegionProps As RegionProperties oRegionProps = oSketch.Profiles.AddForSolid.RegionProperties ' the accuracy to Low oRegionProps.Accuracy = 69377 Dim Ixx, Iyy, Izz, Ixy, Iyz, Ixz As Double Call oRegionProps.MomentsOfInertia(Ixx, Iyy, Izz, Ixy, Iyz, Ixz) 'Parallel Axis Theorem Applied About Centroid Dim IxCon As Double IxCon=Ixx-oRegionProps.Area * oRegionProps.Centroid.Y^2 Dim IyCon As Double IyCon=Iyy-oRegionProps.Area * oRegionProps.Centroid.X^2 Dim oMessage As String Dim oConMessage oMessage= "Current Location Properties: " & vbCrLf & _ "Area: " & oRegionProps.Area & vbCrLf & "Centroid (X,Y): " & _ oRegionProps.Centroid.X & ", " & oRegionProps.Centroid.Y & vbCrLf & _ " Ixx: " & Ixx & vbCrLf & " Iyy: " & Iyy & vbCrLf & _ vbCrLf & "Parallel Axis Theorem" & vbCrLf & _ "Applied About Centroid:" & vbCrLf & _ " Ixx (centroid): " & IxCon & vbCrLf & " Iyy (centroid): " & IyCon Dim oUOM As UnitsOfMeasure ' 11272 is inch, 11268 is cm oUOM = ThisApplication.ActiveDocument.UnitsOfMeasure Dim oRegionPropsCon As RegionProperties Dim ConArea, ConCentroidX,ConCentroidY, ConIxx, ConIyy, ConIxCon, ConIyCon As Double ConCentroidX=oUOM.ConvertUnits(oRegionProps.Centro
id.X, 11268,11272) ConCentroidY=oUOM.ConvertUnits(oRegionProps.Centro id.Y, 11268,11272) 'Conversion factors Dim oConversionFactorArea As Double Dim oConversionFactorInertia As Double oConversionFactorArea=oUOM.ConvertUnits(1, 11268,11272)^2 oConversionFactorInertia=oUOM.ConvertUnits(1, 11268,11272)^4 ConArea=oRegionProps.Area*oConversionFactorArea ConIxx=Ixx*oConversionFactorInertia ConIyy=Iyy*oConversionFactorInertia ConIxCon=IxCon*oConversionFactorInertia ConIyCon=IyCon*oConversionFactorInertia oConMessage= "Current Location Properties: " & vbCrLf & _ "Area: " & ConArea & vbCrLf & "Centroid (X,Y): " & _ ConCentroidX & ", " & ConCentroidY & vbCrLf & _ " Ixx: " & ConIxx & vbCrLf & _ " Iyy: " & ConIyy & vbCrLf & vbCrLf & "Parallel Axis Theorem "& vbCrLf & _ "Applied About Centroid:" & vbCrLf & " Ixx (centroid): " & _ ConIxCon & vbCrLf & " Iyy (centroid): " & ConIyCon ' oRegionPropsCon = oUOM.ConvertUnits(oRegionProps, 11268,11272) ' Dim oMessageCon As String ' oMessageCon="Area: " & oRegionPropsCon.Area & vbCrLf & "Centroid: " & _ ' oRegionPropsCon.Centroid.X & ", " & _ ' oRegionPropsCon.Centroid.Y & vbCrLf & " Ixx: " &_ ' Ixx & vbCrLf & " Iyy: " & Iyy & vbCrLf & " Ixy: " & Ixy ' MessageBox.Show(oMessage, "Default (cm)") MessageBox.Show(oConMessage, "Default (in)")
Regarding your piece of code.
can you get it to find current Centroid (as i think it already does) and automatically move the whole sketch to X=0 & Y=0?
That would be super awesome!
Please let me know if that is possible?
I saw this piece of code that places stuff at origin:
Public Sub AlignOccurrencesWithConstraints() Dim assemblydoc As AssemblyDocument Set assemblydoc = ThisApplication.ActiveDocument ' Get the occurrences in the select set. Dim occurrenceList As New Collection Dim entity As Object For Each entity In assemblydoc.SelectSet If TypeOf entity Is ComponentOccurrence Then occurrenceList.Add entity End If Next If occurrenceList.Count < 2 Then MsgBox "At least two occurrences must be selected." Exit Sub End If ' This assumes the first selected occurrence is the "base" ' and will constrain the base workplanes of all the other parts ' to the base workplanes of the first part. If there are ' constraints on the other they end up being over constrained. ' Get the planes from the base part and create proxies for them. Dim baseOccurrence As ComponentOccurrence Set baseOccurrence = occurrenceList.Item(1) Dim BaseXY As WorkPlane Dim BaseYZ As WorkPlane Dim BaseXZ As WorkPlane Call GetPlanes(baseOccurrence, BaseXY, BaseYZ, BaseXZ) Dim constraints As AssemblyConstraints Set constraints = assemblydoc.ComponentDefinition.constraints ' Iterate through the other occurrences Dim i As Integer For i = 2 To occurrenceList.Count Dim thisOcc As ComponentOccurrence Set thisOcc = occurrenceList.Item(i) ' Move it to the base occurrence so that if the base is ' not fully constrained it shouldn't move when the flush ' constraints are added. thisOcc.Transformation = baseOccurrence.Transformation ' Get the planes from the occurrence Dim occPlaneXY As WorkPlane Dim occPlaneYZ As WorkPlane Dim occPlaneXZ As WorkPlane Call GetPlanes(thisOcc, occPlaneXY, occPlaneYZ, occPlaneXZ) ' Add the flush constraints. Call constraints.AddFlushConstraint(BaseXY, occPlaneXY, 0) Call constraints.AddFlushConstraint(BaseYZ, occPlaneYZ, 0) Call constraints.AddFlushConstraint(BaseXZ, occPlaneXZ, 0) Next End Sub ' Utility function used by the AlignOccurrencesWithConstraints macro. ' Given an occurrence it returns the base work planes that are in ' the part or assembly the occurrence references. It gets the ' proxies for the planes since it needs the work planes in the ' context of the assembly and not in the part or assembly document ' where they actually exist. Private Sub GetPlanes(ByVal Occurrence As ComponentOccurrence, _ ByRef BaseXY As WorkPlane, _ ByRef BaseYZ As WorkPlane, _ ByRef BaseXZ As WorkPlane) ' Get the work planes from the definition of the occurrence. ' These will be in the context of the part or subassembly, not ' the top-level assembly, which is what we need to return. Set BaseXY = Occurrence.Definition.WorkPlanes.Item(3) Set BaseYZ = Occurrence.Definition.WorkPlanes.Item(1) Set BaseXZ = Occurrence.Definition.WorkPlanes.Item(2) ' Create proxies for these planes. This will act as the work ' plane in the context of the top-level assembly. Call Occurrence.CreateGeometryProxy(BaseXY, BaseXY) Call Occurrence.CreateGeometryProxy(BaseYZ, BaseYZ) Call Occurrence.CreateGeometryProxy(BaseXZ, BaseXZ) End Sub
This one is not as straight forward as the last request.
Fully constrainted or projected sketch geometry can be difficult to deal with. One rule may not best fit every situation. For example, in the Sketch Tab of Application Options, the "Auto-project sketch origin on sketch creation" creates a sketch point that cannot be moved with the below MoveSketchObjects function. How should that project sketch point be treated?
Rather than deal with that, I kept it simple. In the below example, I only include sketch geometry that is underconstrained. In general, it is not a good idea to have underconstrained sketches. However, once the sketch is moved, you may be able to add fixed constaints or dimension to fully constrain the sketch.
Please note that I only tested this in the attached file. There are many more scenarios that this would need to be tested in.
'Check that sketch is active
If TypeOf ThisApplication.ActiveEditObject Is Sketch Then 'Do NothingElse MessageBox.Show("A sketch must be active with a singular closed profile.", "WARNING") Return End If ' Requires reference to the active sketch with single profile to obtain Region PropertiesDim oSketch As Sketch oSketch = ThisApplication.ActiveEditObject Dim oRegionProps As RegionProperties oRegionProps = oSketch.Profiles.AddForSolid.RegionProperties oRegionProps.Accuracy = 69377 ' the accuracy to Low 'Create Vector to moveDim oVec As Vector2d oVec = ThisApplication.TransientGeometry.CreateVector2d(-oRegionProps.Centroid.X, -oRegionProps.Centroid.Y) 'Create a collection of all underconstrained Entities in the sketch '***Note 'kFullyConstrainedConstraintStatus 51713 Object Is fully constrained. 'kOverConstrainedConstraintStatus 51715 Object Is over-constrained. 'kUnderConstrainedConstraintStatus 51714 Object Is under-constrained. 'kUnknownConstraintStatus 51716 Constraint status Is unknown. Dim oSketchObjects As ObjectCollection oSketchObjects = ThisApplication.TransientObjects.CreateObjectCollection Dim oSketchEntity As SketchEntity For Each oSketchEntity In oSketch.SketchEntities If oSketchEntity.ConstraintStatus() = 51714 oSketchObjects.Add(oSketchEntity) Else End If Next ' Move all sketch object in collectionoSketch.MoveSketchObjects(oSketchObjects, oVec, False, True) oSketch.Solve
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