IMAGINiT Manufacturing Solutions Blog

Controlling Inventor's "Look At Behavior"

I often hear comments such as "I want to control the alignment of the part model during new sketch creation" or "How do I control how the part model aligns to the origin axis of the model when I use the "Look At" command".  This article will probably not explain why every alignment occurs but I wanted to point out one control in Inventor 2015.

The Application Option setting is the same for both situations but when a new sketch is being created, another application option setting is required.  It is set active during Inventor installation but it needs to be verified before I go on.  In the Application Options dialog box under the Sketch tab, make sure the option shown below is active.  This setting will automatically align the plane, on which you are creating a new sketch, with your view basically creating a 2D sketching area.

The Application Option switch I want to discuss is located on the Display tab and is at the very bottom.  You will find it under the "Look At Behavior" heading.
When you first install Inventor 2015, the "Perform Minimum Rotation" is set by default.  When you create a new sketch on any plane, in this case a plane on the part model, the program will calculate the closest 2D view and present it to you for sketching.  Depending on the initial orientation of the part, since it rotates the minimum amount, it may leave your sketch oriented with the horizontal axis 90 degrees to what you expected.  You must be aware of this since horizontial and vertical sketch constraints will be affected.
 
You could always rotate the sketch 90 degrees but that can be accomplished automatically is you choose the "Align with Local Coordinate System" option.
When you created a new sketch with this setting, the part model may rotate more but it will always end up with your 2D sketch view aligned with an axis that is always horizontial to your 2D view.  It may be a combination of all the axis but it always presents one of the axis on the horizontal and your sketch constraints will match your sketch.

The choice is yours, but if you keep undoing a lot of horizontal or vertical sketch constraints because you selected the wrong one, it may be a good time to change your options.  A little hint - if you show your sketch axes, the darker one is always the horizontal axis.  So many choices but that is what makes Inventor so interesting for everyone.

Using Vault to set Revisions

If changes are made to a CAD file, those changes should be captured in a revision.  A revision indicates a milestone in the manufacturing process of a file and signifies a point in time in the history of the lifecycle of the file. Some of the common methods of noting a revision are by adding the revision number to the title block of the drawing or by adding a specific revision block to the drawing.  With Vault Workgroup or Professional, there is one more method available; letting the Vault software control the revision level.

When you are using Vault, an initial revision is created represented by a letter or number, depending on your revision scheme. After that, a revision increments according to the format specified in the assigned revision scheme accessed from the Behaviors tab on the Administration dialog.

There are specific commands in Autodesk Vault that allow you to set the current revision level for files and to change the revision level as needed. When loading new files into the Vault, this tool is often used to set the initial revision level.

And there we go!  The revision is set.  Done and done.

Well, not really.  Even though the revision level has been set for this file, it is not locked down at all.  There is nothing preventing someone from checking it out and making changes.  A version labels changes, but it does not prevent additional changes from occurring.

This is where the idea of lifecycle states come in.  Lifecycle states work in conjunction with revisions.  In the simplest form, lifecycle states have a Work in Progress state and a Released state.  The released state locks the file so that it cannot be edited.  

Since the file is locked, no changes can be made to the file.  It can be viewed or even linked to another assembly, but cannot be edited.  To edit the file, the lifecycle state must be changed back to Work In Progress.  As soon as the lifecycle state moves back to Work in Progress, the revision level automatically moves to the next level.

Revisions should always be used in conjunction with lifecycle states so that the current released revision cannot be accidentally edited.

This post has really just been about a working with revisions on a single file.  But Inventor files can have complex, interrelated relationships, so revisions will affect more than a single file.  Future posts will address this idea.

 

Adding Revision Callout to Custom Content Center Library

The other day I was asked how to add a revision callout to a Custom Content Library (CCL) components.  The user told me that they from time to time will change a component entry in the library and wanted to add a revision callout to keep track of changes.  This blog will define the method of adding a Revision column to the CCL and how to map it to the Revision Number of the placed component.

It is assumed that the CCL is already created and the user has permission to edit the library.  Navigate to the CCL using the Editor in Inventor and right click, select Family Table.

Select a table column after which you want to create the Revision Callout column.  Select the Add Column icon.

In Column Properties dialog box, fill in the required data.  If you are going to use a two word column name, you cannot have a space in the name.  The column caption can contain spaces.  Since I am using an alphabetic character for my revision callout, I select String for the data type.  If you would like to use numerical revision callouts, select Integer for the data type and "UL" under the Units entry.  The last important setting is to select the down arrow beside the Map to Inventor Property and choose Summary Information.Revision Number.  This property will propagate the value to the Revision Number under the Project tab of the component iProperties. Select OK to create the column.


The last step is to fill in the beginning Revision Callout.

Select OK to finish.  If you are successful, you will receive a dialog box showing the library was published successfully.  Select OK and then Done to close the Editor dialog box.

Create a new Inventor assembly, and place a component from the CCL that you just modified.  Right click on the component select iProperties then the Project tab.  The Revision Number should match the Revision Callout from the CCL.

Careful consideration must be given to editing CCL components.  Once they are edited and refreshed to the Content Center library, all assemblies that contain the edit component will be updated automatically.  More about this process in a future article.

Improved Inventor Offset Command

 Inventor 2015 has improved the Offset command and it now functions as we all have expected it should for many years.  In the past when you execute the Offset comand and selected sketch geometry, you would drag it to the desired position but it did not offer a way to specify the offset distance will dragging.  This function is now available in Inventor 2015. 

 Left click on the geometry you wish to offset and as you drag, you will recieve the "Heads Up Display" requesting an offset distance.   This of course is only available if you have enabled HUD.

 

If you have enabled "Create Dimensions from Input Values", the offset distance entered will also be entered as a dimension.


Before leaving the Offset command, I would like to mention the two configuration options available.  Both configuration options can be accessed by right clicking on the screen after the Offset command is executed.

The Loop Select option will allow the selection of all connected sketch entities with a single pick.  The Constrain Offset option allows for one dimension to constrain all offset entities with a single dimension.

The improvement of the Offset command will help speed sketch creation and is a welcome improvement.