show planes on selected parts

[bniMW775]

hi,

how do I turn on planes, on the parts I selected in the browser?

I know i can turn on all planes in "object visibility". only i dont want all, I only want the ones i selected.

Brian

[Thomas_Savage]

Hello @bniMW775 

Expand the part by clicking the expand icon >.

Then select origin, and select what planes you want, right click and select visibility.

Or if you have planes you created, select then and click viability.

Hope this solves your problem?

Thomas.

[bniMW775]

well only halfway.

coming from Solid Edge, I could pick my parts, right-click, show reference planes.

and they were shown.

have to expand the parts, manually select the planes and turn them on - not my idea of working smart.

but anyway, thanks for the input.

[Sergio.D.Suárez]

you could try an ilogic rule to see hide the main planes like this

Dim comps As ObjectCollection
Dim comp As Object
comps = ThisApplication.TransientObjects.CreateObjectCollection
While True
comp = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyOccurrenceFilter, "Select a component") 

If IsNothing(comp) Then Exit While
comps.Add(comp) 
End While

For Each comp In comps
If comp.Definition.WorkPlanes.Item(1).Visible = True Then
	comp.Definition.WorkPlanes.Item(1).Visible = False
	comp.Definition.WorkPlanes.Item(2).Visible = False
	comp.Definition.WorkPlanes.Item(3).Visible = False
Else
	comp.Definition.WorkPlanes.Item(1).Visible = True
	comp.Definition.WorkPlanes.Item(2).Visible = True
	comp.Definition.WorkPlanes.Item(3).Visible = True
End If
	iLogicVb.UpdateWhenDone = True 
Next

[johnsonshiue]

Hi Brian,

I don't believe Inventor has exact workflow you are looking for. But, may I ask you why you want to see the origin planes of the selected component? Do you want them to appear temporarily? Or, you want them to be visible until you turn them off. Are you trying to create a sketch on an origin plane?

Many thanks!

[bniMW775]

sometimes i need the planes for constraining the parts.

thats why I want to turn them on/off

[tdant · Accepted solution]

I saw your post and decided to use your situation to increase my own skill set, so I wrote a custom plugin that will add the functionality you want. I attached a Windows installer file. If you download and run it, the next time you run Inventor, you'll find a new option in your right-click menu when you're in an assembly file. It'll be called "Show/Hide Planes", and it'll be located right below "Free Rotate". Select the components that you want to show or hide the planes of, then right click and select the new option. The planes will toggle on or off for each selected component.

[mark_francis]

Thank-you Sergio. I have wanted something like this for years. Your script has instantly increased my productivity and made setting up constraints to reference planes much, much less tedious!!! This should be a standard feature.

Unfortunately I couldn't try tdant's plugin as the powers that be won't let me install software.

[ion1000 · Accepted solution]

    EOPQuery = MsgBox("Would you like to turn visibility of all planes off?" _ 
	& vbCrLf & "Click 'Yes' to turn off." _ 
	& vbCrLf & "Click 'No' to turn on." _ 
	, vbYesNo, "Sketch Visibility")
	
Dim comps As ObjectCollection
Dim comp As Object
comps = ThisApplication.TransientObjects.CreateObjectCollection
While True
    comp = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyOccurrenceFilter, "Select a component") 
    If IsNothing(comp) Then Exit While
    comps.Add(comp) 
End While

If EOPQuery = vbYes Then
For Each comp In comps
    Dim workPlanes As WorkPlanes
    workPlanes = comp.Definition.WorkPlanes
    If workPlanes.Count > 0 Then
        For i = 1 To workPlanes.Count
            If workPlanes.Item(i).Visible = True Then
                workPlanes.Item(i).Visible = False
            Else
                workPlanes.Item(i).Visible = False
            End If
        Next
    Else
        MsgBox("Selected component does not have any workplanes.")
    End If
Next

Else If EOPQuery = vbNo Then
	For Each comp In comps
    Dim workPlanes As WorkPlanes
    workPlanes = comp.Definition.WorkPlanes
    If workPlanes.Count > 0 Then
        For i = 1 To workPlanes.Count
            If workPlanes.Item(i).Visible = False Then
                workPlanes.Item(i).Visible = True
            Else
                workPlanes.Item(i).Visible = True
            End If
        Next
    Else
        MsgBox("Selected component does not have any workplanes.")
    End If
Next
End If
ThisApplication.ActiveView.Update

[Nedeias]

Amazing! Great help!

I have a quick query regarding the content center parts. Is it possible to implement a feature that allows the planes of these content center parts to be hidden and shown?

[tdant]

Afraid not. I developed that addin on a different machine than I have now, so I don't have access to the source code anymore. I'm happy it helps though!

[michael_janssenCN38L]

Than you for this wonderfull tool!!!

[m.vanosch]

Thanks, perfect AddIn! This is going to increase my productivity a lot.