Derived solid visibility off - iLogic

[Anonymous]

Hey,

Recently we have been receiving files that when the solid of the part is derived its appears translucent (refer to image below) and also this appears on a drawing, as well as looks very messy in an assembly. I have two questions, is there an ilogic i can use to turn of all solid bodies from a derived parts in an open assembly. And is there anything that i can do in the settings to hide these features in drawings? 

[IgorMir]

Hi Grant,

Try to apply the View Filter first.

Cheers,

Igor.

[CCarreiras]

Hi!

Question1: You can use "make components" tool in manage tab to turn multisolids into Assembly. Each solid will be a part.

Question 2, already awnswered above.

[GKPByDesign]

This only works at a part and or assembly level, i need this to work at the drawing level. 

[GKPByDesign]

The parts are created as serrate parts, and they used the derived surface bodies as reference, they do not create these using make components, i cannot change how these are made, as its external from this company, but i want to know if there is a quick way to turn them off, without having to go through every file. 

[IgorMir]

Well, I am not really sure what the issue is. Even if a derived surface is visible in the part itself - upon creating the view that surface is not visible in that view. Can you share an example of the issue?

Regards,

Igor.

---

@GKPByDesign wrote:

This only works at a part and or assembly level, i need this to work at the drawing level. 

[Anonymous]

The attached image on my first post shows a large derived pat, for a part that is 5% the size of what you see in the image, if you place this in a drawing, it shows the derived part in the drawing of the part that is 5% the size. Make sense? The part in the image is a smaller white plastic cover 

[IgorMir]

OK, the derived part has been created as a surface one and scaled up during the derive process. That's if I follow your description and the image you have posted earlier.  Without the actual file I can not add anything else to it.

Cheers,

Igor.

[kelly.young]

Hello @Anonymous if you are looking for an iLogic snippet this might help:

Set all surfacebodies to invisible. VBA code attached

iLogic - API access to Surface Bodies

Here are a few other good posts on how to turn the visibility off. 

turn off a surface in drawing view

Globally turn off surfaces in idw views

Hiding Surface Bodies in Drawing views by default?

The best might be to turn off all surfaces and create a Level Of Detail to reference from the drawing.

For iLogic inquiries post at Inventor Customization Forum for best results.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Anonymous]

From one of the post there were multiple codes, but they were VBA, how do i get this to become an iLogic ule? 

Sub HideSurfacesInAsm()


'catch and skip errors
On Error Resume Next
'define the active assembly
Dim oAssyDoc As AssemblyDocument
Set oAssyDoc = ThisApplication.ActiveDocument
Dim oSurfacebody As WorkSurface

Dim Vis As Boolean
Dim result
result = MsgBox("Make all surfaces visible?", vbYesNoCancel)
Select Case result
    Case vbYes
        Vis = True
    Case vbNo
        Vis = False
    Case vbCancel
        Exit Sub
End Select

Dim oDoc As Inventor.Document

For Each oDoc In oAssyDoc.AllReferencedDocuments
    
    For Each oSurfacebody In oDoc.ComponentDefinition.WorkSurfaces
        oSurfacebody.Visible = Vis
    Next
Next
ThisApplication.ActiveDocument.Update

End Sub

[Lewis.Young]

This should work with iLogic now:

SyntaxEditor Code Snippet

Sub Main()


'catch and skip errors
On Error Resume Next
'define the active assembly
Dim oAssyDoc As AssemblyDocument
oAssyDoc = ThisApplication.ActiveDocument
Dim oSurfacebody As WorkSurface

Dim Vis As Boolean
Dim result
result = MsgBox("Make all surfaces visible?", vbYesNoCancel)
Select Case result
    Case vbYes
        Vis = True
    Case vbNo
        Vis = False
    Case vbCancel
        Exit Sub
End Select

Dim oDoc As Inventor.Document

For Each oDoc In oAssyDoc.AllReferencedDocuments
    
    For Each oSurfacebody In oDoc.ComponentDefinition.WorkSurfaces
        oSurfacebody.Visible = Vis
    Next
Next
ThisApplication.ActiveDocument.Update

End Sub

Lewis Young
Windows 7 x64 - 32GB Ram
Intel Xeon E5-1620 v2 @ 3.70GHz
nVidia Quadro M2000 - 4GB
Inventor Professional 2017.3
Vault Basic 2017
3ds Max 2018

[emanuel.c]

Updated to work from Part Document also:

Sub Main()

	'catch and skip errors
	On Error Resume Next
		
	Dim Vis As Boolean
	Dim result = MessageBox.Show("Yes" & vbCrLf & "No - Turn Visibility OFF" & vbCrLf & _
		"Cancel - Exit", "Make all surfaces visible?", MessageBoxButtons.YesNoCancel)
	Select Case result
	    Case vbYes
	        Vis = True
	    Case vbNo
	        Vis = False
	    Case vbCancel
	        Exit Sub
	End Select
	
	'define the active assembly
	Dim oAssyDoc As AssemblyDocument
	oAssyDoc = ThisApplication.ActiveDocument	
	Dim oDoc As Inventor.Document = ThisApplication.ActiveDocument
	DocType = oDoc.DocumentType
	Dim oSurfacebody As WorkSurface
	
	If DocType = DocumentTypeEnum.kAssemblyDocumentObject Then		
		For Each oDoc In oAssyDoc.AllReferencedDocuments		    
		    For Each oSurfacebody In oDoc.ComponentDefinition.WorkSurfaces
		        oSurfacebody.Visible = Vis
		    Next
		Next
	Else		
		For Each oSurfacebody In oDoc.ComponentDefinition.WorkSurfaces
		        oSurfacebody.Visible = Vis
		    Next
	End If

	ThisApplication.ActiveDocument.Update

End Sub