Hide all drawing hidden lines that aren't from an iFeature
Hi @chaines59GWR. I think you would reduce processing time my finding the iFeature in 'the model' first, then supplying that as the 'ModelObject' it is asking for in the DrawingView.DrawingCurves property, to get a DrawingCurvesEnumerator with far fewer DrawingCurve objects in it. Then you will not need to test each curve to check what it represents, and can move right on to iterating the curve's segments to turn their visibility off. But another step which may make the overall process even faster would be to collect them into an ObjectCollection, then use the Sheet.ChangeLayer method to switch them to a Layer that you have turned off.
Wesley Crihfield
(Not an Autodesk Employee)
That right-click dialog has been asked about a ton of times, but unfortunately, there is no super simple alternative to it on the Inventor API side that compares to that. The process I mentioned about getting the model object and supplying that to get the filtered collection is the closest. But then, you either have to iterate every individual curve segment, changing property values, or you have to do the Layer thing, but you can create a custom Layer on the fly, and set it how you want it, then specify that Layer as the one to switch them to. Unfortunately, there is no super easy way to undo that action later (after the rule has finished) that will put all that stuff back on their original layers, and settings.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @chaines59GWR. I initially thought you were talking about a drawing of a part, directly. If it is a drawing of an assembly directly, then that changes things. The error you are seeing with that code example is likely because of 'context' (3D model coordinate space) differences. You can only specify a model object that is 'directly' referenced within the Document that is being directly referenced by the drawing view. When we look at the DrawingView.DrawingCurves online help page's description about the 'model object', we see 'Feature' (and an iFeature is definitely a type of Feature), and we also see that it mentions 'proxies'. Proxies are sort of like geometric copies of model entities that are being 'referenced' from within other Documents which gets transformed (position & orientation changed) into the model space of an assembly. That proxy geometry in the assembly is not the 'original' geometry, which would only exist within the other Document's ComponentDefinition (context).
So, since the drawing view references an assembly, and the 'real' iFeatures are down within the definitions of other referenced documents represented by component occurrences in the assembly, we will need to dig down to those 'real' iFeatures, then use those to get a reference to their 'proxy' geometry (iFeatureProxy) that only exists within the parent level assembly's context. And even that is assuming that all component occurrences represent parts, and none are sub assemblies. If any are sub assemblies, and any component occurrences within those sub assemblies (or even lower in the overall assembly structure), then it gets even more complex, and we may need to use a 'recursive' routine to find them, and get their 'top level' proxy geometry. The point is, we cant supply something to that DrawingView that only exists down within some other referenced document...it has to be something that is directly in the context of the Document that is being directly referenced by that view, so we must find the 'proxy' versions of those iFeatures to supply to that DrawingCurves property, not the 'original' iFeatures themselves.
We get access to 'proxies' through the ComponentOccurrence object's method named CreateGeometryProxy. That method asks for 2 things. The first is a variable representing the geometry object that only exists within the context of that exact same ComponentOccurrence's Definition. The second thing it wants is a variable that you want to represent the 'proxy' of that first object, which only exists in this ComponentOccurrence's parent assembly's context. We usually declare that second variable before using that method, but do not give it a value yet, then that method sets its value. Then we can use that second variable to refer to that higher level proxy object from that point on in our code. But sometimes even a proxy is still in the 'mid' level of an assembly, such as within a sub-assembly, instead of being in the context of the top level assembly yet. So we sometimes need to repeat that step, using the ComponentOccurrence representing the sub assembly next, in order to get the proxy that only exists in the context of the top level of the main assembly. Then we can finally use that top level proxy for our measurements, constraints, or in this case in the DrawingCurves property. The idea of proxies, what they are, and how they work, can be complicated to wrap your mind around at first.
Wesley Crihfield
(Not an Autodesk Employee)
My advice at this point would be to eliminate the whole first section of code where it is getting 'all' drawing curves in the whole view, and putting them all into a List. That step is not necessary. You are already iterating through the 'filtered' collection of DrawingCurves in the second section of your code. Plus that 'List.Contains()' method call within that second iteration is likely taking a long time to process, and is completely unnecessary. Instead of taking curves out of the List at that point, that should be where you are initially putting them into the List. Not only that, but since you are only using that list to later iterate through each individual segment within it, turning their visibility off, you could just be doing that visibility change within the primary iteration directly, without needing to ever put them into a list. That would prevent the whole secondary iteration loop, and all the processing associated with that.
Try this edited version of your code, and see if it works a little faster.
Sub Main
Dim StartTime As DateTime = Now
Dim oView As DrawingView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select Drawing View")
If oView Is Nothing Then Return
Dim oAsm As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
For Each oComp As ComponentOccurrence In oAsm.ComponentDefinition.Occurrences.AllLeafOccurrences
If oComp.Suppressed Then Continue For
If TypeOf oComp.Definition Is VirtualComponentDefinition Then Continue For
For Each iFeat As Inventor.iFeature In oComp.Definition.Features.iFeatures
Dim iFeatProxy As Inventor.iFeatureProxy = Nothing
oComp.CreateGeometryProxy(iFeat, iFeatProxy)
Dim oDCurves As DrawingCurvesEnumerator = Nothing
'if proxy was obtained from lower level component in sub assembly, then
'proxy obtained may not yet be in context of main assembly yet
'a top level proxy can only be obtained directly from top level components
'or from the proxies of lower level components that exist at highest level
'proxies at deeper levels will need to be stepped up to highest level
Try : oDCurves = oView.DrawingCurves(iFeatProxy) : Catch : End Try
If oDCurves Is Nothing OrElse oDCurves.Count = 0 Then Continue For
For Each oiFeatCurve As DrawingCurve In oDCurves
For Each oiFeatSegment As DrawingCurveSegment In oiFeatCurve.Segments
If oiFeatSegment.HiddenLine = True Then oiFeatSegment.Visible = False
Next oiFeatSegment
Next oiFeatCurve
Next iFeat
Next oComp
Logger.Info("ALL SEGMENTS HIDDEN [" & Round(Now.Subtract(StartTime).TotalSeconds, 1) & "s]")
End Sub
...Or, you can do it with the Layer idea, like this...
Sub Main
Dim StartTime As DateTime = Now
Dim oView As DrawingView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select Drawing View")
If oView Is Nothing Then Return
Dim oAsm As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oObjColl As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection
For Each oComp As ComponentOccurrence In oAsm.ComponentDefinition.Occurrences.AllLeafOccurrences
If oComp.Suppressed Then Continue For
If TypeOf oComp.Definition Is VirtualComponentDefinition Then Continue For
For Each iFeat As Inventor.iFeature In oComp.Definition.Features.iFeatures
Dim iFeatProxy As Inventor.iFeatureProxy = Nothing
oComp.CreateGeometryProxy(iFeat, iFeatProxy)
Dim oDCurves As DrawingCurvesEnumerator = Nothing
'if proxy was obtained from lower level component in sub assembly, then
'proxy obtained may not yet be in context of main assembly yet
'a top level proxy can only be obtained directly from top level components
'or from the proxies of lower level components that exist at highest level
'proxies at deeper levels will need to be stepped up to highest level
Try : oDCurves = oView.DrawingCurves(iFeatProxy) : Catch : End Try
If oDCurves Is Nothing OrElse oDCurves.Count = 0 Then Continue For
For Each oiFeatCurve As DrawingCurve In oDCurves
For Each oiFeatSegment As DrawingCurveSegment In oiFeatCurve.Segments
If oiFeatSegment.HiddenLine = True Then oObjColl.Add(oiFeatSegment)
Next oiFeatSegment
Next oiFeatCurve
Next iFeat
Next oComp
Dim oSheet As Inventor.Sheet = oView.Parent
Dim oDDoc As DrawingDocument = oSheet.Parent
Dim oMyLayer As Inventor.Layer = oDDoc.StylesManager.Layers.Item(1).Copy("Hidden iFeature Curves")
oMyLayer.Visible = False
oView.Parent.ChangeLayer(oObjColl, oMyLayer)
Logger.Info("ALL SEGMENTS HIDDEN [" & Round(Now.Subtract(StartTime).TotalSeconds, 1) & "s]")
End Sub
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After looking back at the title of this discussion, I may have misunderstood the task you were trying to do in these two code examples. You are not trying to control the visibility of iFeature hidden lines, but trying to turn off 'all other' hidden lines that do not belong to any iFeatures. My mistake. But you probably understand the process better now than you did before, so maybe this will still help somehow.
Wesley Crihfield
(Not an Autodesk Employee)
And yes, there is a way to turn 'defer updates' on/off by by code. It is different, depending on the document type, but for drawings, it is in the 'Document Settings' (manually), and that setting can be accessed through the DrawingDocument.DrawingSettings property, which returns a DrawingSettings object, then use its DeferUpdates property, which is Read/Write, with a Boolean value. Not sure if that will work for this situation, but definitely worth trying out.
Wesley Crihfield
(Not an Autodesk Employee)
Good idea with the selection and command execution idea @marcin_otręba. It does seem like the process that the user interface tools use behind the scenes to do these types of tasks are somehow able to get the job done faster than our traditional Inventor API code methods are able to do it. Maybe they somehow incorporate multi-threading capabilities or something like that in their supporting code, not sure. The process of capturing the group of drawing curves multiple times (once to get them all, potentially multiple other times when specifying specific model objects to filter out), then iterating through two levels of every entity in those collections, takes a long time, no matter what we are doing with them.
On a side note...I don't know why I didn't really pay attention to this earlier but, if testing how much time these tasks are taking is important, and you want to get accurate results, then you should not capture the start time before the 'Pick' function is used, but after that point. Because that Pick function starts a user interface selection session, which can last an unknown/dynamic amount of time, depending on how long the user takes to manually select that type of object. There are also likely cleaner ways of doing something like that, such as using the built-in System.Diagnostics.StopWatch object. You can create a new instance of that Class using the 'New' keyword, then you can use its super convenient properties and methods for keeping track of how long code based tasks take, and can get the results in multiple formats (units of time, or 'ticks').
Wesley Crihfield
(Not an Autodesk Employee)
