Get face to face measurement
Hi @blandb. This example may not be exactly what you were looking for, but is similar and does basically the same task, with Angle also thrown in there. Only it does so using API code and geometry properties, rather than a measure command. It also takes into account if the two selected faces are not perfectly parallel. And it was designed for use in an assembly environment too, so it kind of fits the scenario.
Sub Main
Dim Face1 As FaceProxy = PickPlanarFaceProxy
If IsNothing(Face1) Then Exit Sub
Dim Face2 As FaceProxy = PickPlanarFaceProxy
If IsNothing(Face2) Then Exit Sub
Dim Plane1 As Plane = Face1.Geometry
Dim Plane2 As Plane = Face2.Geometry
Dim Distance, Angle As Double
If Plane1.IsParallelTo(Plane2) Then
If Plane1.IsCoplanarTo(Plane2, 0.0001) Then
Distance = 0.0 : Angle = 0.0
Else
Distance = Plane1.DistanceTo(Plane2.RootPoint) : Angle = 0.0
End If
ElseIf Plane1.IsPerpendicularTo(Plane2, 0.0001) Then
MsgBox("Selected Faces Are Perpendicular.", , "")
Exit Sub
Else
Distance = 0.0 : Angle = Plane1.Normal.AngleTo(Plane2.Normal)
End If
MsgBox("Distance = " & Distance & " cm" & vbCrLf & _
"Angle = " & Angle & " rad", , "")
Dim oDoc As Document = Face1.ContainingOccurrence.Parent.Document
Distance = oDoc.UnitsOfMeasure.ConvertUnits(Distance, "cm", "in")
Angle = oDoc.UnitsOfMeasure.ConvertUnits(Angle, "rad", "deg")
MsgBox("Distance = " & Distance & " in" & vbCrLf & _
"Angle = " & Angle & " deg",,"")
End Sub
Function PickPlanarFaceProxy As FaceProxy
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Select a flat face.")
If IsNothing(oObj) OrElse (TypeOf oObj Is FaceProxy = False) Then Return Nothing
Dim oFace As FaceProxy = oObj
If oFace.SurfaceType <> SurfaceTypeEnum.kPlaneSurface Then Return Nothing
Return oFace
End FunctionI left the two different feedback message, showing centimeters & radians in one, and inches and degrees in the other, because I wasn't sure if that was part of the goal or not. You could also simply select the two faces, then execute the normal measure command too ("AppMeasureDistanceCmd"), but then what's the use of doing it by code, because you've pretty much done more work this way, than doing it with the normal measure tool on the screen, and still don't have a value stored in a variable.
Wesley Crihfield
(Not an Autodesk Employee)
Sure. Here you go. I got rid of all the angle stuff, and metric stuff. I left the perpendicular message in there, just so you know that it did something, instead of just not returning any message at all, when that is the case. But you can get rid of that too, if you are just going to turn this into its own Function. The key to not getting a negative number is the Math.Abs() function.
Sub Main
Dim Face1 As FaceProxy = PickPlanarFaceProxy
If IsNothing(Face1) Then Exit Sub
Dim Face2 As FaceProxy = PickPlanarFaceProxy
If IsNothing(Face2) Then Exit Sub
Dim Plane1 As Plane = Face1.Geometry
Dim Plane2 As Plane = Face2.Geometry
Dim Distance As Double
If Plane1.IsParallelTo(Plane2) Then
If Plane1.IsCoplanarTo(Plane2, 0.0001) Then
Distance = 0.0
Else
Distance = Plane1.DistanceTo(Plane2.RootPoint)
End If
ElseIf Plane1.IsPerpendicularTo(Plane2, 0.0001) Then
MsgBox("Selected Faces Are Perpendicular.", , "") : Exit Sub
End If
UOM = ThisApplication.UnitsOfMeasure
Distance = UOM.ConvertUnits(Distance, "cm", "in")
Distance = Math.Abs(Distance)
MsgBox("Distance = " & Distance & " in",,"")
End Sub
Function PickPlanarFaceProxy As FaceProxy
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Select a flat face.")
If IsNothing(oObj) OrElse (TypeOf oObj Is FaceProxy = False) Then Return Nothing
Dim oFace As FaceProxy = oObj
If oFace.SurfaceType <> SurfaceTypeEnum.kPlaneSurface Then Return Nothing
Return oFace
End Function
Wesley Crihfield
(Not an Autodesk Employee)
Hi @blandb. I'm not sure I fully understand the overall process and your question, but if you need to be able to specify a component name within your code, but do not want to hard code the name into the code, there are usually a few options for that situation. You could use an InputBox to prompt the user to enter the component name. You could use a SharedVariable to temporarily store the component name within Inventor's 'session memory', then retrieve that SharedVariable's value within your followup code somewhere so that it can be shared multiple times by multiple rules. You could record the value/data to something like an Attribute, iProperty, or Parameter, but that will 'dirty' your document. You could write the value out to a temporary text file in your temp folder, then retrieve it as needed. Are any of these thoughts pointing in the right direction?
Wesley Crihfield
(Not an Autodesk Employee)
Below is an image with 2 faces highlighted. Obviously these would be much further apart. So, I have some components that need to fit between those faces. I'm working on the quantity that is needed to fit the space. This situation can happen multiple different times on an assembly, this is just a single instance. There could be many of the same size components highlighted with the blue faces that I need to auto fill the spacing. So that is where the issue of the names of adding components. Since I could only run this once on this run, or many different times on different runs. I cant use tube and pipe for this. I currently place the components and then pattern, but my boss is wanting to try and automate this.
I am also trying to figure out how to capture the edge names of the highlighted faces. I have named the entities, but when I choose face 1, how to extract the edge name I assigned when selecting that instances face, same for face 2.
hope that helps.
Hi @blandb. Concerning the last two sentences of your last post...Did you assign the names to those two faces within the Part environment, using the built-in user interface tool...select face, right-click, choose 'Assign Name' from right-click menu, type in name, then OK? Or did you use some other automation tool? If you used some other automation tool, are you using the same naming conventions as the built-in tool for naming entities? In an assembly environment, faces, edges, & vertex objects that were assigned names in part environment, will not be immediately available. You will have to do a little digging to identify them, or extract any possibly existing name from their 'native' object. All that type of geometry in an assembly is a proxy of the original, instead of the original directly. For instance, a face we select in an assembly environment will be a FaceProxy object, instead of a regular Face. So we would have to dig back to the original Face that this Proxy represents, then either dig down into its Face.AttributeSets for the Attribute, or get the document object that the component represents, then get the NamedEntities interface for that document, then use its tools to check if the entity has been given a name. I don't recall what version of Inventor you are using, but the user interface tool, and the NameEntities interface became available around Inventor 2019.1 I believe.
Wesley Crihfield
(Not an Autodesk Employee)
It can definitely be intimidating to tackle when you are new to the idea. Here is one way of doing it with a fairly simple iLogic rule. This example is just for Edges though, as a quickie example to suit the specific need right now. This example will also only work when the selected edge is on a top level part type component.
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartEdgeFilter, "Select part edge.")
If IsNothing(oObj) OrElse (TypeOf oObj Is EdgeProxy = False) Then Exit Sub
Dim oEdgeProxy As EdgeProxy = oObj
Dim oEdge As Edge = oEdgeProxy.NativeObject
Dim oPDoc As PartDocument = oEdge.Parent.ComponentDefinition.Document
oNEs = iLogicVb.Automation.GetNamedEntities(oPDoc)
Dim oName As String = oNEs.GetName(oEdge)
If oName = "" Then
MsgBox("No name found for selected edge.", , "")
Else
MsgBox("The Name assigned to the selected edge is: " & oName, , "")
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Wesley Crihfield
(Not an Autodesk Employee)
Is there any option to get the max distance between to edges / named geometries / surfaces?
Hi @Maximilian.Prasser. I do not believe there is a 'built-in' method for finding 'maximum distance'.
There are 3 methods for finding minimum distance:
MeasureTools.GetMinimumDistance
ICadMeasure.MinimumDistance Method (Object, Object)
ICadMeasure.MinimumDistance Method (Object, Object, Object, Object)
...but none of those have any option for getting maximum distance.
There is very likely a way to get that data, if it is important enough, but it will likely require a 'custom' method. There can be a great many things involved in creating custom measuring tools, depending on how complex the scenarios that it is expected to manage. Flat faces and straight edges are relatively simple to deal with, but the geometry of the bottom face in that image, and its edges appear to be curved in all 3 coordinate directions, so it will be much more complex to measure to/from accurately. Since the measurement you want in this specific situation could be found by an 'oriented bounding box', there may be an easier route to finding that size, but that size would be one value among 3 values, and you would need to be able to determine which of those 3 values is the correct one.
SurfaceBody.OrientedMinimumRangeBox (a Property of the SurfaceBody object, which returns an OrientedBox transient mathematical object)
OrientedBox (that returned object Type)
DirectionOne, DirectionTwo, & DirectionThree (three properties of that object, which give us 'Vector' objects)
Vector (transient mathematical object representing direction and distance)
Vector.Length (a property of the Vector object, which gives us its length)
You can collect that data from all 3 of its directions, then use known sizes to eliminate the ones you are not looking for. Just one plan, among multiple possible plans.
Wesley Crihfield
(Not an Autodesk Employee)
