Strange things in Inventor 14

[Anonymous]

Hi,

I'm using Inventor 14 and strange things are happening: Part is shown in the tree but dissapeared from screen,option "edit" is grayed out, double click to enter edit mode is not responding. As well bunch of other options are not available: selection-all subtools ... etc. etc.

Soooo dissapointed from version to version.

[cbenner]

Are you seeing any unresolved part errors?  Can you post a screen shot or the file here?

[Anonymous]

No any errors, updated, rebuilt all. I did evrything I could. Also, from time to time, copy-paste option will not work. I couldn't drag and drop from tree into dsplay area nor to go regular copy-paste (right click-copy, right click-paste). Please see attached picture (screen shot).

Thank you.

[cbenner]

What happens if you turn the visibility of that last component (tip dresser?) back on?  Are they the same part in the assembly twice?  I'm grabbing at straws here since I don't use 2014.

[Anonymous]

I turn visibility off and on and it appears on the screen. But all of a sudden "Object visibility" button is grayed out and not active. Me and my coleague switched from R13 to R14 few days ago and we are already fed up.

Thank you, though.

[Paul.Normand]

Hi - I can tell from your screen capture that you are in Express mode. Click Load Full on the ribbon and things will return to normal for you. You might want to take a look at the What's New entry for assemblies. Scroll down about halfway to read about and watch the video on Express mode.

http://wikihelp.autodesk.com/Inventor/enu/2014/Help/0000-What_s_N0/0001-What_s_N1/0002-Assembly2

Express mode is a new method of working with large assemblies that was introduced in 2014 to improve performance. As you can see, certain workflows in the initial release of the Express functionality are not enabled. You can set default assembly open behavior in the Application Options>Assembly tab. You can turn off Express mode completely, or set the threshold value to a higher number than the default value of 500. Increasing the value allows you to open files below the threshold in Full mode by default, and files with a higher part count in Express mode.

Hope that helps.

Cheers

Paul Normand (autodesk)

[Anonymous]

Full/Express feature helped, thank you. Can you also explain to me how to solve the problem with Shared sketches showing up during part/assembly hide/unhide? I work with large assemblies (automated welding cells) and every time when I unhide some parts/assemblies, shared sketches are showing up making my screen very cluttered. I have to go inside those parts/assemblies and manualy hide them. It is a tedious job, beleive me.

[robmatthews]

At a part level:  When a new sketch is created, and then consumed by a feature the visibility is automatically turned off.  If you then Share the sketch, it turns the visibility back on so that any further features can "see" the sketch that you want to use.

When you have completed the use of that sketch, you must manually turn off the visibility. IV assumes that when you share a sketch, you might want to use it for more than one extra feature, so it leaves it on for you.

So you must (at the part level) turn off the visibility of all sketches (and workplanes) to de-clutter your assembly views. 

(I have actually written a script to do just that, as well as save and close the file, in one button click.)

This is good housekeeping. I hope this clears up any confusion.

(My script, in case anyone is interested:

Sub SaveAndClose()
' Written 2010 by Rob Matthews (c)
On Error Resume Next
Dim oDoc As Document
Dim i As Integer
Set oDoc = ThisApplication.ActiveDocument
oDoc.Dirty = True
If ThisApplication.ActiveDocument.DocumentType = kPartDocumentObject Or _
        ThisApplication.ActiveDocument.DocumentType = kAssemblyDocumentObject Then
    oDoc.Update
    For i = 1 To oDoc.ComponentDefinition.WorkPlanes.count
        oDoc.ComponentDefinition.WorkPlanes.Item(i).Visible = False
    Next
    For i = 1 To oDoc.ComponentDefinition.WorkAxes.count
        oDoc.ComponentDefinition.WorkAxes.Item(i).Visible = False
    Next
    For i = 1 To oDoc.ComponentDefinition.WorkPoints.count
        oDoc.ComponentDefinition.WorkPoints.Item(i).Visible = False
    Next
    For i = 1 To oDoc.ComponentDefinition.Sketches.count
        oDoc.ComponentDefinition.Sketches.Item(i).Visible = False
    Next
    For i = 1 To oDoc.ComponentDefinition.Sketches3D.count
        oDoc.ComponentDefinition.Sketches3D.Item(i).Visible = False
    Next
End If
      '============== Append a file to keep track of usage
      '==============
If ThisApplication.SilentOperation = False Then
    ThisApplication.SilentOperation = True
    oDoc.Close
    ThisApplication.SilentOperation = False
Else
    oDoc.Close
End If
End Sub

[-niels-]

Also, if you've already turned off the visibility for the shared sketch, you might check if the representation hasn't reset to "master" instead of "default" (or other preferred representation.)

You could also go to "View > Object visibility" and uncheck the 2D-sketch option to temporarily turn the visibility off.

[Anonymous]

I have tried everything under the Sun: I turned off sketches at part level, still once you hide/unhide in asembly they just show up. The only way around it is to turn off Sketch visibility. But qute often I need to change parts at assembly level and to turn them on the whole display light s up with thousands of shared sketches.

Also, is there any way to set up automatic centerlines upon view creation? We produce some complitated fabrications and always have to go view by view to set up automated centerlines.

Thank you.

[-niels-]

Hmm, if it's happening to parts (not sub-assemblies) then i'm a bit stumped.
I'd try making a new view rep in the part which has the shared sketches set to invisible and see if that helps some...

Regarding the automatic centerlines question, it might be better to create a new topic for that so more people see it.