iLogic include work axis from assembly to drawing

[Anonymous]

Hello all,

Could anybody help me with edditing code: 

Dim doc As DrawingDocument = ThisDoc.Document

For Each sheet As Sheet In doc.Sheets
    For Each view As DrawingView In Sheet.DrawingViews

        Dim camera As Camera = View.Camera
        If (camera.ViewOrientationType = ViewOrientationTypeEnum.kIsoTopRightViewOrientation) Then
            Continue For
        End If

        Dim refDoc = View.ReferencedDocumentDescriptor.ReferencedDocument
        Dim axis As WorkAxes = refDoc.ComponentDefinition.WorkAxes

        View.SetIncludeStatus(axis.Item(1), True)
        View.SetIncludeStatus(axis.Item(2), True)
        View.SetIncludeStatus(axis.Item(3), True)
    Next
Next

 I want include work axis from assembly to drawing - include controll ilogic rule. 

Is possible to define for what drawing view and for what axis (by name)?

Thanks a lot. 

[JhoelForshav]

Hi @Anonymous 

Are you looking for something like this?

The rule lets you pick the view in the drawing and then answer yes/no if you want to include the axes...

Dim View As DrawingView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Pick view")
Dim refDoc = View.ReferencedDocumentDescriptor.ReferencedDocument
Dim oAxes As WorkAxes = refDoc.ComponentDefinition.WorkAxes
For Each oAxis As WorkAxis In oAxes
	Dim oInclude As DialogResult
	oInclude = MessageBox.Show("Include " & oAxis.Name & "?", "Include Axis", _
	MessageBoxButtons.YesNo, MessageBoxIcon.Question)
	If oInclude = DialogResult.Yes Then
		View.SetIncludeStatus(oAxis, True)
	Else
		View.SetIncludeStatus(oAxis, False)
	End If
Next

[Anonymous]

Hello,

thats instring too. 

But this is not what I need. 

I need this: 

If teplomer not suprres do: 

include Work Axis5 - include / visibly.

If teplomer is suprres - Work Axis5 will be unvisibly. 

(in drawing will be more views, so i need to specific for what view I want to include the axis. but by name not with click set.)

I know how to do If.... and so on, but I´m fighting with VBA.

 

[JhoelForshav · Accepted solution]

@Anonymous 

I assume you mean if "teplomer" is invisible in the view, not suppressed?

Try this,

Dim oSheet As Sheet = ActiveSheet.Sheet
Dim oViewName As String = "VIEW1" 'Name of the view
Dim oView As DrawingView
For Each osView As DrawingView In oSheet.DrawingViews
	If osView.Name = oViewName
		oView = osView
		Exit For
	End If
Next
If oView Is Nothing
	MsgBox("No view found with name: " & oViewName)
	Exit Sub
End If

Dim refDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oDef As AssemblyComponentDefinition = refDoc.ComponentDefinition
Dim oOcc As ComponentOccurrence = oDef.Occurrences.ItemByName("teplomer")
Dim oAxis As WorkAxis = oDef.WorkAxes.Item("Work Axis5") 'Get axis by name
If oView.GetVisibility(oOcc) = True 'See if teplomer is visible
	oView.SetIncludeStatus(oAxis, True)
Else
	oView.SetIncludeStatus(oAxis, False)
End If

[Anonymous]

Hi, 

I want only:

Visibly axis if teplomer isn´t supress in assembly. 

I need to dimension angle of teplomer in drawing. So if I don´t have teplomer in assy, I don´t want to include axis in drawing.

Your code show me error. I don´t know why.

[JhoelForshav]

Were you running the code on a view based on a part when you got the error?

Could you attach the assembly? 🙂

[Anonymous]

Hello,

sorry my mistake. I wrote wrong view name. (first capital letter).

I little bit change your code: Visibility is controlled by linked paramter:  

Dim oSheet As Sheet = ActiveSheet.Sheet
Dim oViewName As String = "Hlavni" 'Name of the view
Dim oView As DrawingView
For Each osView As DrawingView In oSheet.DrawingViews
	If osView.Name = oViewName
		oView = osView
		Exit For
	End If
Next
If oView Is Nothing
	MsgBox("No view found with name: " & oViewName)
	Exit Sub
End If

Dim refDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oDef As AssemblyComponentDefinition = refDoc.ComponentDefinition
'Dim oOcc As ComponentOccurrence = oDef.Occurrences.ItemByName("teplomer")
Dim oAxis As WorkAxis = oDef.WorkAxes.Item("Work Axis5") 'Get axis by name
If Parameter("ENG-000218317-P.ipt.teplomer_01") = 0.000 ul 'See if teplomer is supress
	oView.SetIncludeStatus(oAxis, False)
Else
	oView.SetIncludeStatus(oAxis, True)
End If

If teplomer is availabilite then  Parameter("ENG-000218317-P.ipt.teplomer_01") = 1 ul 

If teplomer is suppress then  Parameter("ENG-000218317-P.ipt.teplomer_01") = 0 ul 

I can´t linked True/ false parametr from base component.. 

But, one more problem :/. If axis get visibly, it´s "small", can I manage size of axis in code? 

 

 

[JhoelForshav]

@Anonymous 

Seems like you want to move the endpoint of the centerline representing the axis.

Maybe something like this?

Dim oSheet As Sheet = ActiveSheet.Sheet
Dim oViewName As String = "Hlavni" 'Name of the view
Dim oView As DrawingView
For Each osView As DrawingView In oSheet.DrawingViews
	If osView.Name = oViewName
		oView = osView
		Exit For
	End If
Next
If oView Is Nothing
	MsgBox("No view found with name: " & oViewName)
	Exit Sub
End If

Dim refDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oDef As AssemblyComponentDefinition = refDoc.ComponentDefinition
'Dim oOcc As ComponentOccurrence = oDef.Occurrences.ItemByName("teplomer")
Dim oAxis As WorkAxis = oDef.WorkAxes.Item("Work Axis5") 'Get axis by name
If Parameter("ENG-000218317-P.ipt.teplomer_01") = 0.000 ul 'See if teplomer is supress
	oView.SetIncludeStatus(oAxis, False)
Else
	oView.SetIncludeStatus(oAxis, True)
End If

Dim oAxisLine As Centerline = oSheet.Centerlines.Item(oSheet.Centerlines.Count)
'Should be the last centerline, otherwise try below for loop to get it...

'For Each ocLine As Centerline In oSheet.Centerlines
'	If ocLine.ModelWorkFeature Is oAxis
'		oAxisLine = ocLine
'		Exit For
'	End If
'Next
Dim oPoint As Point2d = oAxisLine.EndPoint.Copy
Dim oVector As Vector2d = oAxisLine.Geometry.Direction.AsVector.Copy
oVector.ScaleBy(10) 'Set distance to move endpoint of line.
oPoint.TranslateBy(oVector)
oAxisLine.EndPoint = oPoint

[Anonymous]

Hi,

Yes you´re right. But it´s look that end point going to out of drawing view. 

I tried to change vector to (-10) etc..But nothing help. Maybe change: 

oAxisLine.EndPoint.Copy 

To something like: 

oAxisLine.StartPoint.Copy ?

[JhoelForshav · Accepted solution]

@Anonymous 

try this instead 🙂

Dim oSheet As Sheet = ActiveSheet.Sheet
Dim oViewName As String = "Hlavni" 'Name of the view
Dim oView As DrawingView
For Each osView As DrawingView In oSheet.DrawingViews
	If osView.Name = oViewName
		oView = osView
		Exit For
	End If
Next
If oView Is Nothing
	MsgBox("No view found with name: " & oViewName)
	Exit Sub
End If

Dim refDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oDef As AssemblyComponentDefinition = refDoc.ComponentDefinition
'Dim oOcc As ComponentOccurrence = oDef.Occurrences.ItemByName("teplomer")
Dim oAxis As WorkAxis = oDef.WorkAxes.Item("Work Axis5") 'Get axis by name
If Parameter("ENG-000218317-P.ipt.teplomer_01") = 0.000 ul 'See if teplomer is supress
	oView.SetIncludeStatus(oAxis, False)
Else
	oView.SetIncludeStatus(oAxis, True)
End If

Dim oAxisLine As Centerline = oSheet.Centerlines.Item(oSheet.Centerlines.Count)
'Should be the last centerline, otherwise try below for loop to get it...

'For Each ocLine As Centerline In oSheet.Centerlines
'	If ocLine.ModelWorkFeature Is oAxis
'		oAxisLine = ocLine
'		Exit For
'	End If
'Next
Dim oPoint As Point2d = oAxisLine.StartPoint.Copy
Dim oVector As Vector2d = oAxisLine.Geometry.Direction.AsVector.Copy
oVector.ScaleBy(-10)
oPoint.TranslateBy(oVector)
oAxisLine.StartPoint = oPoint

[Anonymous]

@JhoelForshav thank you a lot!

Where do you learn it?
I tried to find some books, but I found just one book from Autodesk, but there are just elementary knowledge.

[JhoelForshav]

@Anonymous 

You're welcome. I think it's best to move the scaling of the axis to within the if-statement. So you don't do all of that if the axis isn't included...

Dim oSheet As Sheet = ActiveSheet.Sheet
Dim oViewName As String = "Hlavni" 'Name of the view
Dim oView As DrawingView
For Each osView As DrawingView In oSheet.DrawingViews
	If osView.Name = oViewName
		oView = osView
		Exit For
	End If
Next
If oView Is Nothing
	MsgBox("No view found with name: " & oViewName)
	Exit Sub
End If

Dim refDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oDef As AssemblyComponentDefinition = refDoc.ComponentDefinition
'Dim oOcc As ComponentOccurrence = oDef.Occurrences.ItemByName("teplomer")
Dim oAxis As WorkAxis = oDef.WorkAxes.Item("Work Axis5") 'Get axis by name
If Parameter("ENG-000218317-P.ipt.teplomer_01") = 0.000 ul 'See if teplomer is supress
	oView.SetIncludeStatus(oAxis, False)

Else
	oView.SetIncludeStatus(oAxis, True)
	
	Dim oAxisLine As Centerline = oSheet.Centerlines.Item(oSheet.Centerlines.Count)
	'Should be the last centerline, otherwise try below for loop to get it...

	'For Each ocLine As Centerline In oSheet.Centerlines
	'	If ocLine.ModelWorkFeature Is oAxis
	'		oAxisLine = ocLine
	'		Exit For
	'	End If
	'Next
	Dim oPoint As Point2d = oAxisLine.StartPoint.Copy
	Dim oVector As Vector2d = oAxisLine.Geometry.Direction.AsVector.Copy
	oVector.ScaleBy(-10)
	oPoint.TranslateBy(oVector)
	oAxisLine.StartPoint = oPoint
End If

I've learnt a lot from this forum or just googling stuff.

The API reference manual here is great for looking up objects and their properties, functions etc.

https://help.autodesk.com/view/INVNTOR/2020/ENU/

[TecnicoPanni]

Hi JhoelForshav

I'd like to include the work axis of a part in the assembly view, not of the assembly itself.

After selecting the view, is there a way to select the part I like in the selected view?

Thank you