Add a button to show overwritten dimensions in drawing

[l.paasch]

Problem:

Inventor has the ability to overwrite dimensions. This is good to easily make new drawings from the same model with different sizes. On the other hand it sometimes leads to confusions when another user (or the same user after a long time) works with the drawing without noting that there are some dimensions overwritten. This can lead to wrong dimensions when parts are manufactured acc. to the model behind the drawing.

Idea:

Please add a button (similar to the constraints in the assembly) to show dimensions in a drawing that are overwritten, hidden or with added text.

This would hugely simplify to search the drawing for false dimensions that where made in the "quick and dirty" stage of the drawing.

[swalton]

Inventor has a "Select all Overridden Dimensions" tool available in the drawing environment.  Its not as nice as a ribbon button, but can be helpful.

[SReitberger]

The button / command is already there.

-> Select All Overridden Dimensions

You´ll find it in the "Quick Access Toolbar" under the Selection-Dropdown

https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-3E3537A9-565E-4F2E-B69D-069EDCDF1AE1

The command only selects dimensions. If you have many dimensions on the drawing and many of them are overwritten you could move them to a different layer (with a different color). Then you are able to see the dimensions you have to work on.

[l.paasch]

Thank you @SReitberger for the hint. There I found it. 

@swalton Unfortunately I could not find it as you described. When I click on the drawing environment it looks like this:

I tried to get it into the user command but could not find it. Is there a way to get this command into the ribbon?

[SReitberger]

The hint from @swalton works with Shift + Right Click. I think you missed pressing the Shift key.

[Yijiang.Cai]

This should be implemented in very legacy release, and you can get it from selection filter.

[alexkCP9VX]

This button -> Select All Overridden Dimensions

It is good, but not enough.

I will find and press this button ONLY if I will know or suspect the overridden dimensions are presents on this drawings. 

I will not check every drawing!

My idea is MARK with color or font or some symbol on the drawing - this dimension is overridden, but were it will be printed it MARK will be eliminated and on the paper it will be regulars drawing. 

(But mainly I against to use overridden function at all - for new drawing need to make new 3d model)

[SReitberger]

@alexkCP9VX  Maybe an iLogic-rule can do the job for you.

You can store the following code in an external rule and run it with an event trigger for drawings. I can´t say if you would prefer the "After Open Document" or "Before Save Document" event. 

If there are overridden dimensions a messagebox will inform you about that. Finally the "Select All Overridden Dimensions" command will be executed. 

Option Explicit ON
Dim oIVApp As Application = ThisApplication
Dim oDoc As DrawingDocument = oIVApp.ActiveDocument
Dim oSheet As Sheet = oDoc.ActiveSheet

Dim oDim As DrawingDimension, lOverriddenFound As Long
For Each oDim In oSheet.DrawingDimensions
    If oDim.ModelValueOverridden Or oDim.HideValue Then
        lOverriddenFound += 1
    End If
Next

If Not 0 = lOverriddenFound Then
    MsgBox(lOverriddenFound & " overridden dimensions found in drawing.")
    oIVApp.ActiveView.Fit
    oIVApp.CommandManager.ControlDefinitions.Item("DrawingSelectAllOverriddenDimsCmd").Execute
End If

[Edit: "Or oDim.HideValue " added in line 8 ]

[alexkCP9VX]

Dear  @SReitberger

Thank you very much, you make a good solution!!!