Mirror multible solids with ilogic

[ejaL9K8H]

Hi

I would like to mirror multible solids (166) with one miror feature.

I have a code, which is working with one solid at the time, but what do I have to change or add to mirror more solids at once?

I dont want 166 new mirror features added to model, but only one.

Sub Main()

'Create Mirror Part and remove orginal part.
    
    Dim oDoc As PartDocument
    oDoc = ThisApplication.ActiveDocument

    Dim oCol As ObjectCollection
    oCol = ThisApplication.TransientObjects.CreateObjectCollection

    oCol.Add(oDoc.ComponentDefinition.SurfaceBodies(1)) ' What do i have to write in this line, to mark multible solids?

    Dim oPlane As WorkPlane
    oPlane = oDoc.ComponentDefinition.WorkPlanes(3)

    Dim oMirror As MirrorFeature
    oMirror = oDoc.ComponentDefinition.Features.MirrorFeatures.Add(oCol, oPlane, True, kOptimizedCompute)

    oMirror.NewBodyOperation = True
	
End Sub

Thanks in Advance.

[ejaL9K8H]

This rule are able to count all solids in the model:

Dim oDoc As PartDocument = ThisApplication.ActiveDocument
Dim SolidList As New ArrayList()
For Each SurfaceBodies In oDoc.ComponentDefinition.SurfaceBodies
	SolidList.Add(SurfaceBodies.Name)
Next

SolidCount = SolidList.Count
MessageBox.Show(SolidCount, "Number of Solids")

How can I mirror all these solids with one Mirror feature in iLogic?

[Ralf_Krieg]

Hello

Untested:

Sub Main()

'Create Mirror Part and remove orginal part.
    
    Dim oDoc As PartDocument
    oDoc = ThisApplication.ActiveDocument

    Dim oCol As ObjectCollection
    oCol = ThisApplication.TransientObjects.CreateObjectCollection
	
	For Each SurfaceBody In oDoc.ComponentDefinition.SurfaceBodies
		oCol.Add(SurfaceBody)
	Next
	
    'oCol.Add(oDoc.ComponentDefinition.SurfaceBodies(1)) ' What do i have to write in this line, to mark multible solids?

    Dim oPlane As WorkPlane
    oPlane = oDoc.ComponentDefinition.WorkPlanes(3)

    Dim oMirror As MirrorFeature
    oMirror = oDoc.ComponentDefinition.Features.MirrorFeatures.Add(oCol, oPlane, True, kOptimizedCompute)

    oMirror.NewBodyOperation = True
	
End Sub

[ejaL9K8H]

It gives an error:

Unspecified error (Exception from HRESULT: 0x80004005 (E_FAIL))

[Ralf_Krieg · Accepted solution]

Sorry, you have to create a mirrorfeaturedefinition first.

Sub Main()

'Create Mirror Part and remove orginal part.
    
    Dim oDoc As PartDocument
    oDoc = ThisApplication.ActiveDocument

    Dim oCol As ObjectCollection
    oCol = ThisApplication.TransientObjects.CreateObjectCollection
	
	For Each SurfaceBody In oDoc.ComponentDefinition.SurfaceBodies
		oCol.Add(SurfaceBody)
	Next
	
    'oCol.Add(oDoc.ComponentDefinition.SurfaceBodies(1)) ' What do i have to write in this line, to mark multible solids?

    Dim oPlane As WorkPlane
    oPlane = oDoc.ComponentDefinition.WorkPlanes(3)
	
	Dim oMirrorFeatureDefinition As MirrorFeatureDefinition=oDoc.ComponentDefinition.Features.MirrorFeatures.CreateDefinition(oCol, oPlane)
	
    Dim oMirror As MirrorFeature
    oMirror = oDoc.ComponentDefinition.Features.MirrorFeatures.AddByDefinition(oMirrorFeatureDefinition)

    oMirror.NewBodyOperation = True
	
End Sub

[ejaL9K8H]

Thanks for you help.

But it still shows the same error... 

[Ralf_Krieg]

Hello

Possible to post the file or a screenshot of the model browser?

[ejaL9K8H]

[Ralf_Krieg]

Hello

I've tried to model a similar part as of the picture shows. The visible plane is XY-Plane?

My code runs without any errors. Which version of inventor do you use?

[ejaL9K8H]

That is correct. The visible plane is the XY plane.

Im am using Inventor Professional 2020, release 2020.2

But I am also using Autodesk Factory Design Utilities 2020, releade 2020.1.3, because i am trying to make a asset model.

[ejaL9K8H]

I just tried to biuld a new part, and it works if I join the two extrusions.

But I would like to make it as two different solids, because i need to add some different colours to the part and make a pattern.

And when i am doing this, it is not able to run the rule...

[ejaL9K8H]

In adition to this I would like to remove the original part, but the rule would run if i add this:

Dim oMirrorFeatureDefinition As MirrorFeatureDefinition=oDoc.ComponentDefinition.Features.MirrorFeatures.CreateDefinition(oCol, oPlane, True, kOptimizedCompute)

[dutt.thakar · Accepted solution]

@ejaL9K8H 

I have created a similar code with a bit of variation, see below code. The thing is that adding multiple bodies in an object collection seems like an issue in Inventor 2019, (I am using it and I see the same error that you see in Inventor 2020). I also have tested the same code in Inventor 2021 and it is working perfectly fine.

The code created by @Ralf_Krieg  will also work fine in Inventor 2021

			Dim oDoc As PartDocument
    		oDoc = ThisApplication.ActiveDocument
	
			Dim oDef As PartComponentDefinition = oDoc.ComponentDefinition
			Dim oBody As SurfaceBody
			Dim oFeatures As PartFeatures = oDef.Features
			Dim oPlane As Object = oDef.WorkPlanes.Item(3)
			Dim oCol As ObjectCollection
   			oCol = ThisApplication.TransientObjects.CreateObjectCollection
    		        oCol.Clear

			For i = 1 To oDef.SurfaceBodies.Count
				oCol.Add(oDef.SurfaceBodies.Item(i))	
			Next
			
			Dim oMD As MirrorFeatureDefinition = oDef.Features.MirrorFeatures.CreateDefinition(oCol, oPlane)
			Dim oMirror As MirrorFeature = oDef.Features.MirrorFeatures.AddByDefinition(oMD)

This seems like a problem/bug in Inventor 2020 or 2019 versions.

I am tagging @MjDeck here, he might be able to answer us in more detail and if it is a bug, it can be reported as well.

@MjDeck 

can you elaborate on this a bit? Any help from you is appreciated.

[dutt.thakar]

@ejaL9K8H 

You need to add the MirrorFeatureDefinition like this. 'Only two inputs Object collection and Mirror Plane is needed, no other arguments are necessary

Dim oMD As MirrorFeatureDefinition = oDef.Features.MirrorFeatures.CreateDefinition(oCol, oPlane)

To remove the original solid, use this.

oMD.RemoveOriginal = True

[ejaL9K8H]

Thanks a lot to the both of you!

But I still get the same error.

Is there any posibility to get this running in Inventor 2020?

[dutt.thakar]

@ejaL9K8H 

One way to do in Inventor 2020 is to use multiple mirror features, for each solid body a new mirror feature can be created, if you are okay with that I can alter the code and post.

[ejaL9K8H]

I am able to write the code myselvers that makes multible mirror features, if this is the only posibility.
But I would just like to do it with a single mirror feature.

[dutt.thakar]

@ejaL9K8H 

I understand your concern here, but as mentioned it is not working in Inventor 2019 and 2020, let's wait for some response from MJDeck, as he is from Autodesk and a real expert, he might have some idea on this. If we are doing something wrong, he may be able to guide us/show some alternatives or if it is a bug, he can confirm and report it.

Hope this will help you.

[ejaL9K8H]

Thanks for your time 

[WCrihfield]

Have you tried specifying a different 'PatternComputeTypeEnum' variation, within the 'MirrorFeatureDefinition' line yet?  It sounds like those options mostly apply to when you are mirroring Features, rather than bodies, but you could give it a try anyways to see if it makes any difference for you.