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GetObjectByPersistReference3 fails for ref I just got (in Assembly)

Question asked by Greg James on May 30, 2017
Latest reply on Jun 1, 2017 by Greg James

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The following code throws my exception when run from an Assembly.

Why does the ModelDoc2 not accept a persistreference3 that it just handed me?

const int PERSIST_REF_OBJ_OK = (int)swPersistReferencedObjectStates_e.swPersistReferencedObject_Ok;

public List<object> SegmentsToPersistRefs(List<SketchSegment> segments)

{

Debug.Print("SegmentsToPersistRefs called for list of " + segments.Count);

List<object> refs = new List<object>();

foreach (SketchSegment seg in segments)

{

object pid = mDoc.Extension.GetPersistReference3(seg);

if (pid == null)

{

throw new ApplicationException("SketchSegment GetPersistReference3 is null");

}

int errorCode;

object obj = mDoc.Extension.GetObjectByPersistReference3(pid, out errorCode);

if (errorCode != PERSIST_REF_OBJ_OK)

{

// *** ENDS UP HERE with errorCode = 1 == INVALID ***

throw new ApplicationException("Cannot get object from PersistRef3 we just got");

}

refs.Add(pid);

}

return refs;

}

Greg James Jun 1, 2017 2:40 PM

Correct Answer

Found the problem. I was using a part's ModelDoc2, which came from looking from a sketch up to its parent document. If I switch to the ModelDoc2 for the .SLDASM, the GetObjectByPersistReference3() works.

After opening my .SLDASM doc, there are three ModelDoc2 that can be found from SwApp.GetFirstDocument() and ModelDoc2.GetNext().

// ModelDoc2 GetPathName(): sled_01.SLDPRT

// next GetPathName(): test_part_03.SLDPRT

// next GetPathName(): sled_and_part.SLDASM

If I use the ModelDoc2 for the .SLDASM, everything works.

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8 Replies

Josh Brady May 30, 2017 11:39 PM
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I don't play with C stuff... But is your type correct for pid? Looks like you're saying it's an object. pid will be an array of bytes I think (per the help file). This is a bit over my head, but since you are using C don't you need to use the second argument of GetPersistReference3 in order to know how many elements are in the byte array that's returned? I think you don't need that in the VBA example due to the VBA version going to a Variant.
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- Peter Brinkhuis @ Josh Brady on May 31, 2017 7:26 AM
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  I use an object in C# as well, so that woud be a safe bet I think.
  
  Can you show an example of a PID that you get? In my tests (with 2017) it always was an array with 20 entries. I haven't noticed the exact type, but as the max value was 255 they were probably bytes.
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Josh Brady May 31, 2017 8:37 AM
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You said it throws the exception in an assembly... Does this mean it works in parts?

In VBA land I can't get this to not work:

Dim swApp As SldWorks.SldWorks
Dim swDoc As SldWorks.ModelDoc2
Dim swExt As SldWorks.ModelDocExtension
Dim swSelMgr As SldWorks.SelectionMgr
Dim oObj As Object
Dim vRef As Variant
Dim i As Long
Dim j As Long
Dim sRef As String
Dim failCode As Long
Dim theType As swSelectType_e

Sub main()

Set swApp = Application.SldWorks
Set swDoc = swApp.ActiveDoc
Set swExt = swDoc.Extension
Set swSelMgr = swDoc.SelectionManager

For i = 1 To swSelMgr.GetSelectedObjectCount2(-1)
    vRef = swExt.GetPersistReference3(swSelMgr.GetSelectedObject6(i, -1))
    theType = swSelMgr.GetSelectedObjectType3(i, -1)
    sRef = ""
    Debug.Print "Object type: " & theType & " ID length: " & UBound(vRef)
    For j = 0 To UBound(vRef)
        sRef = sRef & " " & vRef(j)
    Next j
    Debug.Print sRef
    Set oObj = Nothing
    Set oObj = swExt.GetObjectByPersistReference3(vRef, failCode)
    Debug.Print "Object is Nothing? " & (oObj Is Nothing) & " Fail code: " & failCode
Next i


End Sub
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- Greg James @ Josh Brady on May 31, 2017 3:03 PM
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  Thanks Josh - They work great in Parts docs using 'object'. That's what the SolidWorks C# API deals with, so I don't have to poke in to the bytes. All C# class instances can be passed around as that ultimate base 'object'. I use them to track SketchSegments during and between invocations of my PropertyManagerPage. They survive edits and rebuilds, and they tell me if the thing they reference has been deleted. It's great.... when working with a Part.
  
  Now I'm trying something similar in an Assembly doc, and it's all gone sideways. At first, I thought it might be related to the difference between the Assembly 'top-level' ModelDoc2 vs. the ModelDoc2 instances I can get from the Assembly Components. Doesn't seem to be. I've tried all combinations of Get/Set with the ModelDoc2 instances that I get in various ways. For example, from an Attribute:
  
  // Attribute attr. Below is edited for brevity. The instances are valid., and calls to them do the right thing.
  object entObj = attr.GetEntity2();
  Entity ent = (Entity)entObj;
  Component2 comp2 = ent.IGetComponent2();
  ModelDoc2 compDoc = (ModelDoc2)comp2.GetModelDoc2();
  // My other way to a ModelDoc2 is the SwApp ActiveDoc
  
  I'll try to get examples of the bytes after this meeting I'm supposed to be in =/
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  - Josh Brady @ Greg James on May 31, 2017 3:10 PM
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    Did you also edit your original code for brevity? Are you using the same ModelDoc2 to obtain the reference that you are using to select by that reference? Once you get to an assembly, the persistent reference for the sketch segments changes. If you get the segments PID in the context of the assembly's ModelDoc2 and then try to select them in the part's ModelDoc2 it won't work.
    
    Dim swApp As SldWorks.SldWorks Dim swDoc As SldWorks.ModelDoc2 Dim swExt As SldWorks.ModelDocExtension Dim swSelMgr As SldWorks.SelectionMgr Dim swSelComp As SldWorks.Component2 Dim swSelDoc As SldWorks.ModelDoc2 Dim oObj As Object Dim vRef As Variant Dim i As Long Dim j As Long Dim sRef As String Dim failCode As Long Dim theType As swSelectType_e Sub main() Set swApp = Application.SldWorks Set swDoc = swApp.ActiveDoc Set swExt = swDoc.Extension Set swSelMgr = swDoc.SelectionManager For i = 1 To swSelMgr.GetSelectedObjectCount2(-1) vRef = swExt.GetPersistReference3(swSelMgr.GetSelectedObject6(i, -1)) Set swSelComp = swSelMgr.GetSelectedObjectsComponent4(i, -1) Set swSelDoc = swSelComp.GetModelDoc2 theType = swSelMgr.GetSelectedObjectType3(i, -1) sRef = "" Debug.Print "Object type: " & theType & " ID length: " & UBound(vRef) For j = 0 To UBound(vRef) sRef = sRef & " " & vRef(j) Next j Debug.Print sRef Set oObj = Nothing Set oObj = swExt.GetObjectByPersistReference3(vRef, failCode) Debug.Print "Object is Nothing in Active doc? " & (oObj Is Nothing) & " Fail code: " & failCode Set oObj = Nothing Set oObj = swSelDoc.Extension.GetObjectByPersistReference3(vRef, failCode) Debug.Print "Object is Nothing in Component's doc? " & (oObj Is Nothing) & " Fail code: " & failCode & vbCrLf Next i End Sub
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    - Greg James @ Josh Brady on May 31, 2017 3:48 PM
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      >Did you also edit your original code for brevity?
      Nope. Original code is as is.
      
      > Are you using the same ModelDoc2 to obtain the reference that you are using to select by that reference?
      Yes, using the same ModelDoc2, as in the code above. I've called that func with all the ModelDoc2 that I can find, in various ways. All have the same issue. I've also tried querying one ModelDoc2 with refs from another ModelDoc2, just in case, and have tried all the combinations of getting from one and querying from another.
      
      > If you get the segments PID in the context of the assembly's ModelDoc2 and then try to select them in the part's ModelDoc2 it won't work
      Seems reasonable to expect that to fail, but I'm not trying that. I'm seeing this problem completely within the context of an Assembly. I never open a Part separately or get PersistRefs from a Part and then try them in an assembly. I'm in the assembly the whole time. I trigger the code by hitting a button in my PropertyManagerPage.
      
      If I relaunch SolidWorks and trigger that same code from a Part, everything works fine.
      My SubmitABug finger is tingling
      
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      - Josh Brady @ Greg James on May 31, 2017 5:49 PM
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        Can you examine the value of PID? Can you compare those values to the ones reported by my VBA macro?
        
        Where is the list of sketch segments coming from? Again, not a C guy, but it looks like you're passing in a list from somewhere to this function. How is the list created? Can you create a similar function to mine that just gets PIDs from the current selection set? If you are pulling the list out of a selection box that SolidWorks populates, the list of objects themselves may be in part context rather than assembly.
        
        Dim swApp As SldWorks.SldWorks Dim swDoc As SldWorks.ModelDoc2 Dim swExt As SldWorks.ModelDocExtension Dim swSelMgr As SldWorks.SelectionMgr Dim swSelComp As SldWorks.Component2 Dim swSelDoc As SldWorks.ModelDoc2 Dim oObj As Object Dim vRef As Variant Dim bRef() As Byte Dim theLen As Long Dim i As Long Dim j As Long Dim sRef As String Dim failCode As Long Dim theType As swSelectType_e Sub main() Set swApp = Application.SldWorks Set swDoc = swApp.ActiveDoc Set swExt = swDoc.Extension Set swSelMgr = swDoc.SelectionManager For i = 1 To swSelMgr.GetSelectedObjectCount2(-1) vRef = swExt.GetPersistReference3(swSelMgr.GetSelectedObject6(i, -1)) theLen = swExt.GetPersistReferenceCount3(swSelMgr.GetSelectedObject6(i, -1)) ReDim bRef(theLen) bRef = swExt.GetPersistReference3(swSelMgr.GetSelectedObject6(i, -1)) Set swSelComp = swSelMgr.GetSelectedObjectsComponent4(i, -1) Set swSelDoc = swSelComp.GetModelDoc2 theType = swSelMgr.GetSelectedObjectType3(i, -1) sRef = "" Debug.Print "Object type: " & theType & " Array length: " & UBound(vRef) + 1 & " Reported length: " & theLen For j = 0 To UBound(vRef) If vRef(j) <> bRef(j) Then sRef = sRef & "!!!" End If sRef = sRef & " " & vRef(j) Next j Debug.Print sRef Set oObj = Nothing Set oObj = swExt.GetObjectByPersistReference3(vRef, failCode) Debug.Print "Object is Nothing in Active doc? " & (oObj Is Nothing) & " Fail code: " & failCode 'Set oObj = Nothing 'Set oObj = swSelDoc.Extension.GetObjectByPersistReference3(vRef, failCode) 'Debug.Print "Object is Nothing in Component's doc? " & (oObj Is Nothing) & " Fail code: " & failCode & vbCrLf Set oObj = swSelDoc.Extension.GetCorresponding(oObj) Debug.Print "Got object in part context? " & Not (oObj Is Nothing) vRef = swSelDoc.Extension.GetPersistReference3(oObj) sRef = "" For j = 0 To UBound(vRef) sRef = sRef & " " & vRef(j) Next j Debug.Print sRef Set oObj = swSelComp.GetCorresponding(oObj) Debug.Print "Got object back in assembly context? " & Not (oObj Is Nothing) vRef = swExt.GetPersistReference3(oObj) sRef = "" For j = 0 To UBound(vRef) sRef = sRef & " " & vRef(j) Next j Debug.Print sRef Next i
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Greg James Jun 1, 2017 2:40 PM
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Found the problem. I was using a part's ModelDoc2, which came from looking from a sketch up to its parent document. If I switch to the ModelDoc2 for the .SLDASM, the GetObjectByPersistReference3() works.

After opening my .SLDASM doc, there are three ModelDoc2 that can be found from SwApp.GetFirstDocument() and ModelDoc2.GetNext().
// ModelDoc2 GetPathName(): sled_01.SLDPRT
// next GetPathName(): test_part_03.SLDPRT
// next GetPathName(): sled_and_part.SLDASM

If I use the ModelDoc2 for the .SLDASM, everything works.
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GetObjectByPersistReference3 fails for ref I just got (in Assembly)

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