Extract Plate Dimensions from Part
There are multiple ways of doing it, it depends on what you are trying to achieve, I have two things for you. You can create the Parameters Length, Width, and Height for the plate in the main part and use them after doing make components in the derived part by linking them. See the below snap for details.
Second way if you want to use iLogic Measure functions only. I would advise you to create planes and use them for Measuring, give appropriate names to planes like for Length "LengthPlane1" and "LengthPlane2" and use it in the Measure.MinimumDistance Snippet. You will have to include the Planes also after using make components in a similar way like parameters.
This will give you always correct dimensions even if your plate is rotated at any orientation.
Hope this will be helpful.
Here are a couple of links to another idea that may peak your interests, that you may be able to use.
SurfaceBody.OrientedMinimumRangeBox Property
And here is an example which uses this property:
You can get the length of each of the three vectors of the OrientedMinimumRangeBox, as your size dimensions.
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Wesley Crihfield
(Not an Autodesk Employee)
Here is a better example, more suited to your request.
The following iLogic rule (local or external) works for Part files only (as is). It assumes the part only has one body (but can be set up do loop through all bodies), gets the first solid body, then gets its OrientedMinimumRangeBox, then gets its data, then extracts the lengths of its three vectors as the overall size of the body. Then it displays a simple MsgBox showing you the result. I used math to convert the database default units from Centimeters to Inches.
Here's the code:
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kPartDocumentObject Then
MsgBox("This rule only works for Part Documents.",vbOKOnly, "WRONG DOCUMENT TYPE")
Exit Sub
End If
Dim oPDoc As PartDocument = ThisApplication.ActiveDocument
Dim oPDef As PartComponentDefinition = oPDoc.ComponentDefinition
Dim oBody As SurfaceBody
If oPDef.SurfaceBodies.Count > 0 Then
oBody = oPDef.SurfaceBodies.Item(1)
Else
MsgBox("This Part has no bodies. Exiting.", , "")
Exit Sub
End If
If Not oBody.IsSolid Then
MsgBox("The body is not Solid. Exiting.", , "")
Exit Sub
End If
Dim oCorner As Point
Dim oV1, oV2, oV3 As Vector
oBody.OrientedMinimumRangeBox.GetOrientedBoxData(oCorner, oV1, oV2, oV3)
Dim oDim1 As Double = oV1.Length / 2.54
Dim oDim2 As Double = oV2.Length / 2.54
Dim oDim3 As Double = oV3.Length / 2.54
MsgBox("First Body Size: " & oDim1 & " x " & oDim2 & " x " & oDim3,,"")
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Wesley Crihfield
(Not an Autodesk Employee)
And this version takes it one step further, filtering the resulting vector lengths from smallest to largest, so you may more accurately name each dimension, in case that is important or applies to your application.
In many cases the smallest dimension is always going to be the Thickness of the material (especially when working with "Plates"). And often the longest of the three dimensions is the Length (or material cut-length). So the remaining dimension can either be labeled as Width, Height, Depth, Gerth, etc.
So here is the same code that takes it that next step further, in case you needed it.
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kPartDocumentObject Then
MsgBox("This rule only works for Part Documents.",vbOKOnly, "WRONG DOCUMENT TYPE")
Exit Sub
End If
Dim oPDoc As PartDocument = ThisApplication.ActiveDocument
Dim oPDef As PartComponentDefinition = oPDoc.ComponentDefinition
Dim oBody As SurfaceBody
If oPDef.SurfaceBodies.Count > 0 Then
oBody = oPDef.SurfaceBodies.Item(1)
Else
MsgBox("This Part has no bodies. Exiting.", , "")
Exit Sub
End If
If Not oBody.IsSolid Then
MsgBox("The body is not Solid. Exiting.", , "")
Exit Sub
End If
Dim oCorner As Point
Dim oV1, oV2, oV3 As Vector
oBody.OrientedMinimumRangeBox.GetOrientedBoxData(oCorner, oV1, oV2, oV3)
Dim oDim1 As Double = oV1.Length / 2.54
Dim oDim2 As Double = oV2.Length / 2.54
Dim oDim3 As Double = oV3.Length / 2.54
Dim oThickness As Double = MinOfMany(oDim1, oDim2, oDim3)
Dim oLength As Double = MaxOfMany(oDim1, oDim2, oDim3)
Dim oWidth As Double
Dim oDims() As Double = {oDim1, oDim2, oDim3}
For Each oDim In oDims
If oDim <> oThickness And oDim <> oLength Then
oWidth = oDim
End If
Next
MsgBox("First Body Size: " & vbCrLf & _
"Thickness = " & oThickness & vbCrLf & _
"Length = " & oLength & vbCrLf & _
"Width = " & oWidth, , "")If this solved your problem, or answered your question, please click ACCEPT SOLUTION.
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Wesley Crihfield
(Not an Autodesk Employee)
Ah. The help page for that Property of that object (SurfaceBody.OrientedMinimumRangeBox Property ), says it was introduced in the 2021 version. Seems to me that it has been available one or two releases earlier than that though. This may be why it isn't working for you. If you're using an earlier version of Inventor, this may not be available to you yet.
If your parts were always rectangular and aligned with the origin planes, you could probably just use the regular RangeBox similarly to how I've used the OrientedMinimumRangeBox, if that's not the situation you may have to use a different method. If you parts were still rectangular, but just not oriented with the origin planes, and you are using a version later than maybe 2018 or so, you may be able to assign names to the faces of your model, then use the NameEntities interface to get those specific faces within the code, instead of creating a bunch of planes.
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Wesley Crihfield
(Not an Autodesk Employee)
