Problem accessing Part files's iLogic rule from an iLogic rule in Assembly file.

[Anonymous]

Dear all,

I have an Assembly file which consists of a part file containing 2 rules. When I try to access a rule from Assembly files using,

iLogicVB.RunRule("PartFile_Name:1","Rule_1")

Suprisingly this error shows up.

Unable to cast COM object of type 'System.__ComObject' to interface type 'Inventor.PartFeatures'. This operation failed because the QueryInterface call on the COM component for the interface with IID '{DA33F1A5-7C3F-11D3-B794-0060B0F159EF}' failed due to the following error: No such interface supported (Exception from HRESULT: 0x80004002 (E_NOINTERFACE)).

The Rule_1 in part file changes the sweep feature. I would like to change the paramteres used in the sweep feature from assembly files iLogic rule.

can any one please help me!

Thanks a lot in advance.

Regards,

Yatish.

[FINET_Laurent]

Morning,

I have a similar issue not long ago..

Here is the correct way :

iLogicVb.Automation.RunRule("Document", "RuleName")

You'll have to declare the document tho, something like this maybe :

Dim oDoc As Document

For Each oDoc In ThisApplication.Documents.VisibleDocuments
	If oDoc.DisplayName = "Vertical baffle 1.iam" Then
		iLogicVb.Automation.RunRule(oDoc, "RuleName")
	End If
Next

Regards,

FINET L.

[Anonymous]

Hallo @FINET_Laurent  Thank you for the solution.

The problem still arises for one of the two rules.

Rule_1: 

MessageBox.Show("Test_Message","Title")

Rule_2:

'Do Something
Dim oSweep As SweepFeature = oCompDef.Features.SweepFeatures.AddUsingPath(oProfile, oPath, kJoinOperation) 
'Do Something

I've used this code in a rule in Assembly file:

Dim oDoc As Document
For Each oDoc In ThisApplication.Documents.VisibleDocuments
	If oDoc.DisplayName = "Part1.ipt" Then
		iLogicVb.Automation.RunRule(oDoc, "Rule_1")
		iLogicVb.Automation.RunRule(oDoc, "Rule_2")
	End If
Next

 The Error still shows up at the Rule_2.

Regards,

Yatish.

[FINET_Laurent]

This may be about the rule 2 itself.

Can you post the full code for that rule ? (If not confidential)

Regards,

FINET L.

[Anonymous]

Hey @FINET_Laurent  Here is the code for rule#2. I have changed the names for some reasons.

'Rule#2

Dim oFeatures As PartFeatures
oFeatures = ThisApplication.ActiveDocument.ComponentDefinition.Features

If Feature.IsActive("Sweep") = True Then
	oFeatures("Sweep").Delete
End If

Dim oPartDoc As PartDocument = ThisDoc.Document
Dim oCompDef As PartComponentDefinition = oPartDoc.ComponentDefinition
' Create a profile.
Dim oSketch1 As Sketch = oCompDef.Sketches.Item("Sketch_2")
Dim oProfile As Profile = oSketch1.Profiles.AddForSolid
' Create a path.
Dim oSketch2 As Sketch = oCompDef.Sketches.Item("Sketch_1")
Dim oPath As Path = oCompDef.Features.CreatePath(oSketch2.SketchLines(1))

' Create the sweep feature.
Dim oSweep As SweepFeature = oCompDef.Features.SweepFeatures.AddUsingPath(oProfile, oPath, kJoinOperation)
oSweep.Name = "Sweep"

 Regards,

Yatish.

[FINET_Laurent · Accepted solution]

I think there is a mistake aroud this :

oFeatures = ThisApplication.ActiveDocument.ComponentDefinition.Features

I think The active document is the assembly document you are  lauching the rules from.

Maybe you need to activate the part document first (from the assembly) :

Dim oDoc As Document
For Each oDoc In ThisApplication.Documents.VisibleDocuments
	If oDoc.DisplayName = "part2.ipt" Then
		
		oDoc.Activate
		
		iLogicVb.Automation.RunRule(oDoc, "Test")
		'iLogicVb.Automation.RunRule(oDoc, "Rule_2")
		
	End If
Next

 The oDoc.Activate set the document to the active document.

Regards,

FINET L.

[Anonymous]

@FINET_Laurent  Hey, Thank you so much. Yes. The oDoc.Activate is the fix.