HOW TO SELECT ONLY WHAT HIDDEN LINES I WANT TO SEE

[Anonymous]

Has to be a easier way.  

have a view that i only want to see a couple of hidden lines in.  Creo would allow you show all hidden lines and then allow you to select which ones you wanted to show up in views.  inventor as far as i can tell does not have that option.

what i have to do is in the first picture show all hidden lines.  then i go and select each and every hidden line to change it's visibility.  once they are all turned off i right click on the view and choose "show hidden edges" and then choose the one i want to be made visible again.  i know i can just not select the ones to keep when i'm changing the visibility but it's easier to put a box around as much as i can at one time then go back and select the ones i want.

what would be EASIER would be if someone could enlighten me on how inventor does what creo can, just select the ones you want to see without having to through the steps i take

[Cadmanto]

You can window or cross depending on the window direction to select.  You don't have to select each individually.

Below is another option in the drawing.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020

[Anonymous]

the window is how i select what i want to turn off.  tried using the "visible" on my part drawing but it gave me an error message when i tried to use it.  i use that on my assembly drawings when i want to show hidden lines but once again they all turn on and then it's back to selecting the ones i want to see.

[jhalljm]

I know this is an old thread but wanted to post this in case any one else comes across wanting this feature. 

I wrote some iLogic that lets you select a drawing view and then turns off all hidden lines in that view so you can then go to the Show Hidden Lines command and pick which ones you want.

If you find this useful or notice a way I could improve this code please let me know!

Sub Main()
Dim odoc As Document = ThisDoc.Document
Dim oApp As Inventor.Application= ThisApplication
Dim oTrans As Transaction = oApp.TransactionManager.StartTransaction(odoc, "HideLines")
ThisApplication.UserInterfaceManager.UserInteractionDisabled = False
Try
If odoc.DocumentType = Inventor.DocumentTypeEnum.kDrawingDocumentObject Then
	Dim oSheet As Sheet = odoc.ActiveSheet
	Dim oView As DrawingView
	Dim oOccs As ComponentOccurrencesEnumerator
	Dim oOcc As ComponentOccurrence
	
	oView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select View")
        oDrawCurves = oView.DrawingCurves(oOcc)
                For Each oDrawCurve In oDrawCurves
                    For Each oDrawCurveSeg In oDrawCurve.Segments
                        If oDrawCurveSeg.HiddenLine = True Then
                            oDrawCurveSeg.Visible = False
                        End If
                    Next
                Next

    oDrawCurves = Nothing
    oOccs = Nothing
Else
	MessageBox.Show("This file is not a Drawing Document", "Alert", MessageBoxButtons.OK, MessageBoxIcon.Warning, MessageBoxDefaultButton.Button1)
End If
Catch
	MessageBox.Show("Error", "Alert", MessageBoxButtons.OK, MessageBoxIcon.Warning, MessageBoxDefaultButton.Button1)
	oTrans.End
	Exit Sub
End Try
iLogicVb.UpdateWhenDone = True
oTrans.End
End Sub

[LSKELLY]

Thanks. This iLogic code is exactly what I needed!

It's view-specific, it's undoable and it does exactly what it's supposed to.

Saved me some tedious activity time today.