API - how to unhide all sketches of an assembly in drawing views

Hi Ronan in order to hide or show model sketces in view you have to select them using their full view base name i.e. boolstatus = drwPart.Extension.SelectByID2("Sketch1@base plate-4@Drawing View1", "SKETCH", 0, 0, 0, False, 0, Nothing, 0) and then use drwPart.BlankSketch

You can travers the drawingcomponent tree in order to get to the sketch name. If the rootcomponent is an assembly you can get its children then the component of each childern and their features names and select them (using full view based path name)

if the drawing rootcomponent is not an assembly however you will get nothing when you try to reach the component of the rootcomponent to walk through its features . in this case get the referenced doc and get the sketches names and select them using full view based path name

regards dudi peer

Then, if I understand, you could only traverse children of an assembly through the DrawingComponent not the referenced component in the view itself. The only way is the view based path name to change sketches state like recorded macro does. But as I want to change the state of any of them of any referenced document, I don't know the name of the sketches. Traversing features would be the solution but it's not possible. There shouldn't be a solution for my probleme. Is that right or is there other ways to do? Regards Ronan

Hi You can traverse the assembly via the drawingcomponent. once you have the drawing component of an assembly component you can get the component (drawingcomponent.component) and travers its features. then you can use the featurec typename and if it is a profile you can get its name (feature.name) and then you can built the name sketcname@componentname@viewname and use selectbyid once selected this way. you can hide or unhide it/ its combersome but its the only way i have succeded . maybe there is aother way but i havent found it. i have try to use select2 while i get the feature but its not actualy selected in the view so it would not hide. dudi peer eci telecom

HI Ronan I wrote the program and i am posting it here since found that a little tricky put the content in a nacro and you can run it

'================================================ Dim swApp As SldWorks.SldWorks Dim oModeldoc As SldWorks.ModelDoc2 Dim oDrwDoc As DrawingDoc Dim oView As SldWorks.View Dim bStatus As Boolean Dim oDrwComp As DrawingComponent Dim oSwSheet As SldWorks.Sheet Dim m_StrViewName As String

Sub main() Dim i As Integer Dim oRootCompDoc As ModelDoc2 Dim strConfigName As String Dim oConfig As Configuration Dim strFullSketcName As String Dim lerr As Long Dim vChildren As Variant Dim oFeature As SldWorks.Feature Dim oComp As Component2

Set swApp = Application.SldWorks Set oModeldoc = swApp.ActiveDoc ' getting the active doc 'testing for drawing If oModeldoc.GetType swDocDRAWING Then swApp.SendMsgToUser ("Document is not drawing") Exit Sub End If

Set oDrwDoc = oModeldoc ' just for convinence to enable autocomplete Set oSwSheet = oDrwDoc.GetCurrentSheet 'getting the current sheet If oSwSheet Is Nothing Then swApp.SendMsgToUser ("cannot get current sheet") Exit Sub End If

Set oView = oDrwDoc.GetFirstView 'first view is the drwing sheet sketch so we have to move get the next for real view Set oView = oView.GetNextView ' getting the first view Do While Not oView Is Nothing ' make sure you get a view m_StrViewName = oView.Name ' getting the view name Debug.Print "View Name: " & m_StrViewName ' for debuging Set oDrwComp = oView.RootDrawingComponent ' getting the root drawing component Set oRootCompDoc = oView.ReferencedDocument ' getting the drawing component document since the ' root component is not exactly an assembly component ' there for when we get its component we cannot get access to the first feature ' we use as workaround by going to the specific configuration of the model and getting the ' the sketches names from there strConfigName = oView.ReferencedConfiguration ' the current configuration of the root component Set oRootCompDoc = swApp.ActivateDoc2(oRootCompDoc.GetPathName, True, lerr) ' activating the reference document

bStatus = oRootCompDoc.ShowConfiguration2(strConfigName) 'activating the configuration Set oFeature = oRootCompDoc.FirstFeature ' getting the first fieatur of the document Do While Not oFeature Is Nothing ' steping through the feature tree of root doc If oFeature.GetTypeName = "ProfileFeature" Then ' checking for sketch strFullSketcName = getSketchFullName(oView.Name, oDrwComp.Name, oFeature.Name) ' getting the sketch name for selectbyis bStatus = oModeldoc.Extension.SelectByID2(strFullSketcName, "SKETCH", 0, 0, 0, False, 0, Nothing, 0) ' selecting the sketch in drawing If bStatus Then oModeldoc.BlankSketch ' blanking the sketch End If Set oFeature = oFeature.GetNextFeature Loop Debug.Print "Drawing RootComp Name " & oDrwComp.Name If oDrwComp.GetChildrenCount > 0 Then Call traverse_drwcomponent(oDrwComp) ' travesing the children components Set oView = oView.GetNextView Loop

End Sub

Function getSketchFullName(strViewName As String, strComponentName As String, strSketchName As String) As String 'this function construct the name of the sketch for selection in drawing Dim vStr As Variant Dim i As Long Dim tmpStr As String Dim StrParentName As String

vStr = Split(strComponentName, "/") tmpStr = strSketchName & "@" & vStr(0) & "@" & strViewName For i = 0 To UBound(vStr) - 1 StrParentName = Left(vStr(i), InStrRev(vStr(i), "-") - 1) tmpStr = tmpStr & "/" & vStr(i + 1) & "@" & StrParentName Next i getSketchFullName = tmpStr Debug.Print getSketchFullName End Function

Sub traverse_drwcomponent(oDrcmp As DrawingComponent) Dim vChildren As Variant Dim oComp As Component2 Dim tmpDrcmp As DrawingComponent Dim i As Long Call traverse_Features(oDrcmp) If oDrcmp.GetChildrenCount > 0 Then vChildren = oDrcmp.GetChildren For i = 0 To oDrcmp.GetChildrenCount - 1 Debug.Print vChildren(i).Name Set tmpDrcmp = vChildren(i) Call traverse_drwcomponent(tmpDrcmp) Next i End If End Sub

Sub traverse_Features(oDrcmp As DrawingComponent) 'this program traverse feature of child component and blank the sketch in the drawing view Dim i As Long Dim oFeature As Feature Dim oComp As Component2 Dim strSketchFullName As String

Set oComp = oDrcmp.Component Set oFeature = oComp.FirstFeature Do While Not oFeature Is Nothing If oFeature.GetTypeName = "ProfileFeature" Then strSketchFullName = getSketchFullName(oView.Name, oDrcmp.Name, oFeature.Name) bStatus = oModeldoc.Extension.SelectByID2(strSketchFullName, "SKETCH", 0, 0, 0, False, 0, Nothing, 0) If bStatus Then oModeldoc.BlankSketch End If Set oFeature = oFeature.GetNextFeature Loop End Sub '==================================================================== regards dudi peer

Yes that is what I manage to do, going through the feature of the subcomponents of an assembly. But what I would like to list are the sketches (then "features") at the assembly level. That ones in the assembly document not those in the parts of the assembly. How to get the sketches name at the assembly level? I have no clue (Set swComp = swRootDrawComp.Component gives me nothing). Did you managed that? Thanks for your contribution. Ronan

What works but only for parts of an assembly:

While Not swView Is Nothing Debug.Print " " Debug.Print "View = " & swView.GetName2 & " [" & swView.Type & "]" Debug.Print "View = " & swView.Name Debug.Print "Ref = " & swView.GetReferencedModelName

Set swRootDrawComp = swView.RootDrawingComponent If Not swRootDrawComp Is Nothing Then Debug.Print "RtComp = " & swRootDrawComp.Name vDrawChildCompArr = swRootDrawComp.GetChildren For Each vDrawChildComp In vDrawChildCompArr Set swDrawComp = vDrawChildComp Set swComp = swDrawComp.Component Debug.Print "Comp = " & swComp.Name Set swFeat = swComp.FirstFeature Do While Not swFeat Is Nothing Debug.Print " Feat = " & swFeat.Name Set swFeat = swFeat.GetNextFeature Loop Next End If Set swView = swView.GetNextView Wend

Sorry, I just posted a message without having seen this one. My ISP is good but not for his news server. I have to check both my news client and google to get answers. I will read what you posted and then answer you. Thanks, Ronan

Thanks very much for your job. That is exactly what I would like to do about accessing sketches in views. That saves me times and errors on quite some of my assemblies. Now I'm like an idiot because I should noticed first two thing that not works:

swAnnotations = oDrwDoc.InsertModelAnnotations3(0, swInsertDimensionsMarkedForDrawing, True, False, True, False) Doesn't work in a macro for unhidden sketches, nothing happens.

No way to automatically show dimensions after hiding sketches. It seems there is no function in the API to do that. Recording a macro gives no information.

I will investigate but without hope. I'm a little disapointed with this API. It seems there is quite some holes in this tool. Workarounds aren't always enough.

Regards, Ronan