iProperties Still unavailable to call into iLogic
Does the MassProperties.XYZMomentsOfInertia method not give you what you are after? iLogic rule code below.
Dim doc As PartDocument = ThisDoc.Document
Dim massProps As MassProperties
massProps = doc.ComponentDefinition.MassProperties
Dim Ixx As Double
Dim Iyy As Double
Dim Izz As Double
Dim Ixy As Double
Dim Iyz As Double
Dim Ixz As Double
massProps.XYZMomentsOfInertia(Ixx, Iyy, Izz, Ixy, Iyz, Ixz)
Dim msg As String = "Ixx " & Ixx.ToString()
MessageBox.Show(msg, "You figure out the units")
I stand corrected, those values from what I can see are the Principle Inertia Values (shown as I1, I2, & I3) in the iProps Physical tab.
The description of the variable states its about the COG, not the origin.
So, if my memory of engineering school from 20 years ago serves, I could just determine the offset of the COG from the origin, and mulitply the mass and that distance (squared), and that would be employing the parallel axis theorem?, thus giving me the global value?
It does really depend on what you are after but yes. if you want the mass moments of inertia relative to the XYZ axes you can modify the values obtained from the XYZMomentsOfInertia method which returns the MOIs about the XYZ axes translated to the COG point. Have a look at the attached part which includes a commented macro (sorry, I try to avoid iLogic for testing) that hopefully helps.
The symmetry of the part and it's alignment with the coordinate system ensures the principal axes (and thus the Principal MOIs) are the same as the MOIs about the XYZ axes translated to the COG.
The initial sketch is offset -3mm along the X axis. This offset affects the MOI about the global Y and Z axes. Check the three options on the iProperties > Physical tab (Principal, Global, and Center of Gravity) and compare them to the output from the macro. The Debug.Print statements print to the Immediate window in the VBA editor.
Sorry but the file is Inventor 2022.
So, After verifying with hand calcs, this is what I came up with.
'Calculates the value of the inertia in Fancus preferred units of Kgf*cm*S² Dim doc As AssemblyDocument = ThisDoc.Document Dim massProps As MassProperties massProps = doc.ComponentDefinition.MassProperties 'these are prinicple values. Ixy, Iyz, Ixz are not required. Dim Ixx As Double Dim Iyy As Double Dim Izz As Double Dim Ixy As Double Dim Ixz As Double Dim Iyz As Double Dim EOATMass As Double Dim Addxx As Double Dim Addyy As Double Dim Addzz As Double Dim COGx As Double Dim COGy As Double Dim COGz As Double Dim RadX As Double Dim RadY As Double Dim RadZ As Double massProps.XYZMomentsOfInertia(Ixx, Iyy, Izz, Ixy, Ixz, Iyz) 'determin mass values EOATMass = iProperties.Mass EOAT_Mass = EOATMass 'Determin offset parallel mass distance COGx = Sqrt(((iProperties.CenterOfGravity.Z)^2) + (iProperties.CenterOfGravity.Y)^2) COGy = Sqrt(((iProperties.CenterOfGravity.X)^2) + (iProperties.CenterOfGravity.Z)^2) COGz = Sqrt(((iProperties.CenterOfGravity.X)^2) + (iProperties.CenterOfGravity.Y)^2) COG_x = COGx COG_y = COGy COG_z = COGz Addxx = EOATMass * COGx ^ 2 Addyy = EOATMass * COGy ^ 2 Addzz = EOATMass * COGz ^ 2 GlobalIxx = (Ixx*100000) + Addxx GlobalIyy = (Iyy*100000) + Addyy GlobalIzz = (Izz*100000) + Addzz 'Dim msg As String = "Ixx " & Ixx.ToString() 'Use Parallel Axis Theorm to determine Global inertia based on principle values offset from origin 'MessageBox.Show(msg, "You figure out the units") FanucIxx = Ixx * 0.00000000101971621 FanucIyy = Iyy * 0.00000000101971621 FanucIzz = Izz * 0.00000000101971621
This works for now. I can equate these to parameters and then have those parameters show up in a form, so this seems to work well. The only thing I'd like to be able to do, is control the format that the variables show up as...i.e. 2 decimal places versus 10 or whatever, but this is good enough.
Secondly, its odd to me that my template file has units set to mm and g for default units of distance and mass, but I still have to apply a conversion factor to Ixx, Iyy, and Izz ? so they are at their root kg*cm² regardless of the files unit settings?
Ohh, and these were the Parameters I created.
Looks good. Inventor uses cm for length values internally, and kg for mass values so API properties and methods that extract this type data always return values in these units. Inventor does the conversions to the document units (or specified units) when showing values in the UI. There are all the conversion tools you could ever want in the UnitsOfMeasure object in the Inventor API. The developer help system is your friend! I'm not sure of the Round() syntax in iLogic but I'm sure there is a function for rounding values to specific decimal places in your code.
So, I am not sure rounding is what I need. Ultimately I need to display my Parameters to more decimal places...Inventor is only allowing me to show 8 decimal places when I use the text box tool in a drawing.
I am pullng those values from the assembly inserted into the drawing.
Are you sure your unit conversions are correct? Do you have the option of creating a text based property instead of a parameter? if so you could format the value in scientific notation with appropriate sig figs. Below is a small iLogic example.
Dim dbl As Double = .00000583455414
Dim str As String = dbl.ToString("0.####e0")
messagebox.Show(dbl.ToString("#.############") & " as string = " & str)
