Performance Issue when supressing many features in part document
In some cases, it helps to use a transaction. You could do something like this:
Dim doc As PartDocument = ThisApplication.ActiveDocument
Dim features = doc.ComponentDefinition.Features
Dim featuresToSuppress As New List(Of String)
featuresToSuppress.Add("Add")
featuresToSuppress.Add("your")
featuresToSuppress.Add("features")
featuresToSuppress.Add("here")
Dim trans = ThisApplication.TransactionManager.StartTransaction(doc, "Suppress features")
Try
For Each featureName As String In featuresToSuppress
features.Item(featureName).Suppressed = True
Next
Catch ex As Exception
MsgBox(ex.Message)
Finally
trans.End()
End Try
Also, have a look at this post:
https://modthemachine.typepad.com/my_weblog/2015/09/improving-your-programs-performance.html
Jelte de Jong
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I'm not sure what may be required to speed up the data collecting part from the SQLite database, but generally speaking, the fewer read and/or write calls between the two, the better. For example it is faster to copy (or paste) an entire 2-directional array of data from (or to) an Excel spreadsheet at once than it is to extract (or write) the data from (or to) each cell individually in a loop. Once you have the data held in memory (assigned to a Variable), then you can work with that data faster, with less processing.
Also, just to add to Jelte's idea in the earlier post...if you were to get all the features you want to control into one or two ObjectCollections (not a List), then you could suppress or un-suppress them all at once, instead of in a loop, using the built-in methods just for that purpose (PartComponentDefinition.SuppressFeatures() & PartComponentDefinition.UnsuppressFeatures()). That should help out some with the processing speed.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @thomas_wegerBYFE5. Did that last code you posted increase the performance noticeably, as you were hoping for? It seemed to me like it might still benefit from a little tweaking to condense & simplify it a bit, so I created an alternate version of it for you to review. This version is just one Sub routine, instead of three, and only attempts to change the suppression status of any feature, if that feature does not already match the status being called for. That testing is done before they get put into the ObjectCollection, that way the 'group' process should work OK for you.
It first makes sure that the 'active' document is actually a part, to avoid that potential problem. Then makes sure each named feature can be found, then checks suppression status. If it was found, and suppression status does not match requested status, it gets added to the collection. Then the appropriate method is used to match the requested suppression status. Then I just added a couple lines at the end for updating & saving the part, but only if needed, and left the 'save' line commented out for now.
Sub SetFeaturesSuppression(FeatureNames As List(Of String), bSuppress As Boolean)
If IsNothing(FeatureNames) OrElse FeatureNames.Count = 0 Then Exit Sub
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kPartDocumentObject Then Exit Sub
Dim oPDoc As PartDocument = ThisApplication.ActiveDocument
Dim oPDef As PartComponentDefinition = oPDoc.ComponentDefinition
Dim oFeatures As PartFeatures = oPDef.Features
Dim oFeatsToProcess As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection
For Each oName In FeatureNames
Dim oFeat As PartFeature = Nothing
Try : oFeat = oFeatures.Item(oName) : Catch : Continue For : End Try
If IsNothing(oFeat) Then Continue For
If oFeat.Suppressed <> bSuppress Then oFeatsToProcess.Add(oFeat)
Next
If bSuppress = True Then
oPDef.SuppressFeatures(oFeatsToProcess)
Else
oPDef.UnsuppressFeatures(oFeatsToProcess)
End If
If oPDoc.RequiresUpdate Then oPDoc.Update2(True)
'If oPDoc.Dirty Then oPDoc.Save
End Sub
Wesley Crihfield
(Not an Autodesk Employee)
Hi @thomas_wegerBYFE5. If any of those named features were created directly in the context of the main (top level) assembly, and not while editing components, then that code would likely work OK. But if none of those features were created directly in the top level assembly, but only in the parts within the assembly, then one major change would be needed. For your code to work on the parts within the assembly, I would suggest that you get the AssemblyDocument.ReferencedDocuments (top level referenced documents only), or AssemblyDocument.AllReferencedDocuments (all levels of referenced documents in assembly structure) to a variable (DocumentsEnumerator Type). Then create a loop of those referenced documents. Then, just inside that loop, use 'If oRefDoc.IsModifiable = False Then Continue For', and then filter for parts only using 'If oRefDoc.DocumentType <> DocumentTypeEnum.kPartDocumentObject Then Continue For'. Then either copy your code for processing parts into that loop below that point, or just call your Sub routine to run that will process the part.
Edit: If you plan on calling your Sub routine (for processing parts) within that loop of referenced documents, you may need to modify your Sub routine's definition line to include the 'input' PartDocument object for it to process, then get rid of the use of 'ThisApplication.ActiveDocument' within the routine to set the document variable's value. That would give it much better control of the situation.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @thomas_wegerBYFE5. I do not know of a built-in API or iLogic method for suppressing a group of assembly components at once. The only alternative I can think of, other than the folder suppression technique you mentioned, to simulate selecting a group of components in the browser tree, then right-click, and choose Suppress. The internal name of the ControlDefinition (command) that gets executed when you do that is called "AssemblyCompSuppressionCtxCmd". To simulate that action, you would use the Document.SelectSet.SelectMultiple method to put them all into the SelectSet, then get that ControlDefinition object and use its Execute method. I generally do not like executing commands from code if there is any other way of doing the same thing, but I will leave that decision up to you to experiment with. I do not know if that process would be any faster to process.
Edit: Upon further inspection, that command 'toggles' suppression status, not just suppresses them. So the components would need to be sorted or filtered before/filtered before adding them to the SelectSet, to avoid problems.
Wesley Crihfield
(Not an Autodesk Employee)
