Solved: Re: How Can I Change The Name of Features and Sketches Usin Logic

Anonymous · ‎11-02-2018

Hello Everyone,

I came across this great post about renaming features in a part using iLogic (code below is from the solution of this post.) I was hoping to take it a step further to include other features, iFeatures and sketches. Adjusting the code to update other features is pretty straight forward but, I am running into issues when I try to get iFeatures and/or sketches to rename. I think this is due to my limited knowledge of code.

Here is the Code I'm working with;

oDoc = ThisApplication.ActiveDocument
oBodies = oDoc.ComponentDefinition.SurfaceBodies

'look at the bodies
For Each oBody In oBodies
	i = 1
	'look at all the features that make up the body
	For Each oFeature In oBody.AffectedByFeatures
		'look at only extrude features
		If oFeature.Type = ObjectTypeEnum.kExtrudeFeatureObject Then
			'rename feature using solid name
			'and pad the number with zero if under 10
			oFeature.Name = oBody.Name _
			& " - Ext. " &  If(i < 10, "0" + CStr(i), CStr(i))
			i = i + 1
		End If
	Next
Next

In the code above, I think I need to change "oFeature" and ObjectTypeEnum.kExtrudeFeatureObject. However, I don't know what I need to change this to.

Any idea how I can make this work?

Thanks,

Paul

philip1009 · ‎11-02-2018

Yes, you do need to change the code to account for every kind of feature you'll come across in the model tree before you can rename it. Typically you have to get down through the component definition, then the collection of features you want to look at, then the specific feature out of that collection, then you can get to the property that stores the name you see in the browser.

Are you only looking to rename specific features in the model tree? Otherwise it'll take a while if you want to account for everything Inventor has to offer.

Right now that code is only looking at Surface Bodies, you'll have to do a loop for every kind of feature you want to rename.

clutsa · ‎11-02-2018

You were close... try this out

oDoc = ThisApplication.ActiveDocument
oFeatures = oDoc.ComponentDefinition.Features
i = 1
For Each oFeature In oFeatures 'look at all the features that make up the body
	
	'look at only extrude features
	If oFeature.Type = ObjectTypeEnum.kExtrudeFeatureObject Then
		'rename feature using solid name
		'and pad the number with zero if under 10
		oFeature.Name = oFeature.SurfaceBodies(1).Name _
		& " - Ext. " & If(i < 10, "0" + CStr(i), CStr(i))
		i = i + 1
	End If

Next

If I've helped you, please help me by supporting this idea.
Mass Override for Each Model State

philip1009 · ‎11-02-2018

Scratch what I said earlier, I wasn't aware that you could go right to the name without going through specific feature collections.

Anonymous · ‎11-02-2018

Clusta, that looks great. Thank you. What would this code look like to rename Holes, iFeatures and/or Sketches?

clutsa · ‎11-02-2018

I got this far but I have to do may actual job now I guess. I'm close on the sketch part but not all sketches have dependents so you'll have to find a way around that (I'm sure a Try/Catch could do it)

oDoc = ThisApplication.ActiveDocument
oFeatures = oDoc.ComponentDefinition.Features
oSketches = oDoc.ComponentDefinition.Sketches
ext = 1
iFeat = 1
'same pattern for other feature counts here

For Each oFeature In oFeatures 'look at all the features that make up the body
	Select Case oFeature.Type
	Case = ObjectTypeEnum.kExtrudeFeatureObject
		oFeature.Name = oFeature.SurfaceBodies(1).Name & " - Ext. " & If (ext < 10, "0" + CStr(ext), CStr(ext))
		ext = ext + 1
	Case = ObjectTypeEnum.kiFeatureObject
		oFeature.Name = oFeature.SurfaceBodies(1).Name & " - Ext. " & If (iFeat < 10, "0" + CStr(iFeat), CStr(iFeat))
		iFeat = iFeat + 1
	'Case = ObjectTypeEnum.k...
		'same pattern as above
	End Select
Next

For Each oSketch In OSketches
	If oSketch.Type = ObjectTypeEnum.kPlanarSketchObject Then
		For Each Dependent In oSketch.Dependents
'			If Not Dependent.Definition Is Nothing Then
'				oSketch.Name = Dependent.Definition.Parent.Name & " - Sketch"
'			End If
		Next
	End If
Next

If I've helped you, please help me by supporting this idea.
Mass Override for Each Model State

Anonymous · ‎11-02-2018

Thank you Clusta! that works perfect. from there I was able to make everything I needed. Sketches would be nice but, know the variables, I figured it would be more work that it was worth.

I would recommend editing the code you have though. Although iFeatures are renamed, they are renamed as Ext.

What you have

oFeature.Name = oFeature.SurfaceBodies(1).Name & " - Ext. " & If (iFeat < 10, "0" + CStr(iFeat), CStr(iFeat))

Should be

oFeature.Name = oFeature.SurfaceBodies(1).Name & " - iFeat. " & If (iFeat < 10, "0" + CStr(iFeat), CStr(iFeat))

Thanks again for your help

ldellaversano · ‎05-16-2023

when I use this rule for the first time everything works perfectly if after I do other processing and I use the rule again it gives me the following error:

Errore alla riga 11 nella regola: Regola0, nel documento: PivotconSA.ipt

Errore non specificato. (Eccezione da HRESULT: 0x80004005 (E_FAIL))

unspecified error
How can I fix?

WCrihfield · ‎05-16-2023

Hi @ldellaversano. It is very difficult to determine what may be going wrong just based on the information you provided. If the error happens again, can you look at the 'More Info' tab of the error message that shows, and translate that to English for us. If you just take a screenshot of the error message, it will still be in be in your native language, and some of us will not be able to read it or translate it. Usually there is a line of text within the 'More Info' tab that indicates what it was trying to do when the error was encountered, and we can use that to determine where in your code the error occurred. But even that may not help if we can not see your code. I suspect, based on your description that this may be a simple matter of needing to update the document after making some edits before trying to change the feature names again, but it is very difficult to judge on so little information. Please include as much information as possible.

Wesley Crihfield

(Not an Autodesk Employee)

ldellaversano · ‎05-16-2023

This is the other info:

System.Runtime.InteropServices.COMException (0x80004005): Errore non specificato. (Eccezione da HRESULT: 0x80004005 (E_FAIL))
in Microsoft.VisualBasic.CompilerServices.LateBinding.InternalLateSet(Object o, Type& objType, String name, Object[] args, String[] paramnames, Boolean OptimisticSet, CallType UseCallType)
in Microsoft.VisualBasic.CompilerServices.NewLateBinding.LateSet(Object Instance, Type Type, String MemberName, Object[] Arguments, String[] ArgumentNames, Type[] TypeArguments, Boolean OptimisticSet, Boolean RValueBase, CallType CallType)
in Microsoft.VisualBasic.CompilerServices.NewLateBinding.LateSet(Object Instance, Type Type, String MemberName, Object[] Arguments, String[] ArgumentNames, Type[] TypeArguments)
in ThisRule.Main() in regola: Regola0, nel documento PivotconSA.ipt:riga 11
in Autodesk.iLogic.Exec.AppDomExec.ExecRuleInAssembly(Assembly assem)
in iLogic.RuleEvalContainer.ExecRuleEval(String execRule)

This is my code:

oDoc = ThisApplication.ActiveDocument
oFeatures = oDoc.ComponentDefinition.Features

ext = 1
iFeat = 1
'same pattern for other feature counts here

For Each oFeature In oFeatures 'look at all the features that make up the body
Select Case oFeature.Type
Case = ObjectTypeEnum.kExtrudeFeatureObject
oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Es" & If (ext < 10, "0" + CStr(ext), CStr(ext))
ext = ext + 1
Case = ObjectTypeEnum.kiFeatureObject
oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Es" & If (iFeat < 10, "0" + CStr(iFeat), CStr(iFeat))
iFeat = iFeat + 1
'Case = ObjectTypeEnum.k...
'same pattern as above
End Select
Next

For Each oFeature In oFeatures 'look at all the features that make up the body
Select Case oFeature.Type
Case = ObjectTypeEnum.kRevolveFeatureObject
oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Riv" & If (ext < 10, "0" + CStr(ext), CStr(ext))
ext = ext + 1
Case = ObjectTypeEnum.kiFeatureObject
oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Riv" & If (iFeat < 10, "0" + CStr(iFeat), CStr(iFeat))
iFeat = iFeat + 1
'Case = ObjectTypeEnum.k...
'same pattern as above
End Select
Next

For Each oFeature In oFeatures 'look at all the features that make up the body
Select Case oFeature.Type
Case = ObjectTypeEnum.kFilletFeatureObject
oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Racc" & If (ext < 10, "0" + CStr(ext), CStr(ext))
ext = ext + 1
Case = ObjectTypeEnum.kiFeatureObject
oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Racc" & If (iFeat < 10, "0" + CStr(iFeat), CStr(iFeat))
iFeat = iFeat + 1
'Case = ObjectTypeEnum.k...
'same pattern as above
End Select
Next

For Each oFeature In oFeatures 'look at all the features that make up the body
Select Case oFeature.Type
Case = ObjectTypeEnum.kChamferFeatureObject
oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Sm" & If (ext < 10, "0" + CStr(ext), CStr(ext))
ext = ext + 1
Case = ObjectTypeEnum.kiFeatureObject
oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Sm" & If (iFeat < 10, "0" + CStr(iFeat), CStr(iFeat))
iFeat = iFeat + 1
'Case = ObjectTypeEnum.k...
'same pattern as above
End Select
Next

Thanks thousand

WCrihfield · ‎05-16-2023

Hi @ldellaversano. Here is a modified version of your code that I just created for you, but have not tested yet. It looked to me like the problem you were likely encountering is that the code was trying to name another feature exactly the same as an already existing feature, which I don't think Inventor allows in the same document. It is very easy to do, so it is difficult to avoid with a rule like this. And I still can not guarantee that you will not encounter the same issue while using this version, but this version is a bit shorter and easier to look at.

Dim oDoc As Inventor.Document = ThisApplication.ActiveDocument
Dim oFeatures As Object = oDoc.ComponentDefinition.Features
'must be different counter for each different type of feature
Dim iExt As Integer = 1
Dim iRev As Integer = 1
Dim iFill As Integer = 1
Dim iCham As Integer = 1
Dim iFeat As Integer = 1

For Each oFeature As PartFeature In oFeatures
	Select Case oFeature.Type
	Case ObjectTypeEnum.kExtrudeFeatureObject
		Try
			oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Es" & If (iExt < 10, "0" + CStr(iExt), CStr(iExt))
		Catch
		End Try
		iExt = iExt + 1
	Case ObjectTypeEnum.kRevolveFeatureObject
		Try
			oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Riv" & If (iRev < 10, "0" + CStr(iRev), CStr(iRev))
		Catch
		End Try
		iRev = iRev + 1
	Case ObjectTypeEnum.kFilletFeatureObject
		Try
			oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Racc" & If (iFill < 10, "0" + CStr(iFill), CStr(iFill))
		Catch
		End Try
		iFill = iFill + 1
	Case ObjectTypeEnum.kChamferFeatureObject
		Try
			oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Sm" & If (iCham < 10, "0" + CStr(iCham), CStr(iCham))
		Catch
		End Try
		iCham = iCham + 1
	Case ObjectTypeEnum.kiFeatureObject
		'an iFeature can contain multiple other types of features
		'Dim oIFeature As Inventor.iFeature = oFeature
		'Dim oIFeatDef As iFeatureDefinition = oIFeature.iFeatureDefinition
		Try
			oFeature.Name = oFeature.SurfaceBodies(1).Name & "_Other" & If (iFeat < 10, "0" + CStr(iFeat), CStr(iFeat))
		Catch
		End Try
		iFeat = iFeat + 1
	End Select
Next

Wesley Crihfield

(Not an Autodesk Employee)

How Can I Change The Name of Features and Sketches Usin Logic

How Can I Change The Name of Features and Sketches Usin Logic

How Can I Change The Name of Features and Sketches Usin Logic

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