iLogic to Rename All Solid Bodies

Issue:
You've created a multi-body solid model with the intent to use the Make Components tool to write out each solid as a new part file. This works fine, but you find yourself wishing there was an easier way to tag each solid with a new name based on a prefix and a series number. For instance, you'd like to name each solid in a part file called 45-723 as such: 45-723_01, 45-723_02, 45-723_03, etc.

Issue:
You can use this iLogic rule to quickly rename the solid bodies for you. In this rule we first look for a custom iProperty named "Prefix" and create it if it is not present. Then we write the part number to the custom iProperty if it is found to be empty. Then the rule uses the value of the custom iProperty named "Prefix" in an input box to query the user for the prefix:

 

The user can change the prefix at this point or accept the existing one. When we press the OK button the rule renames each solid body using the prefix and an increment number, adding a leading zero for each number less than 10.

Thanks to Barbara Han for the original code I used for this rule.

'------- start of ilogic ------

'check for custom iProperty and add it if not found

Dim prefix As String = "Prefix"

customPropertySet = ThisDoc.Document.PropertySets.Item _

("Inventor User Defined Properties")

Try

         prop= customPropertySet.Item(prefix)

Catch

      ' Assume error means not found

            customPropertySet.Add("", prefix)

End Try

'write the part number to the Prefix iProperty if it is empty

if iProperties.Value("Custom", "Prefix") = "" Then

iProperties.Value("Custom", "Prefix") = iProperties.Value("Project", "Part Number") & "_"

else

end if

'check that this active document is a part file   

Dim partDoc As PartDocument

If ThisApplication.ActiveDocument.DocumentType <> kPartDocumentObject Then

MessageBox.Show ("Please open a part document", "iLogic")

End If

'define the active document

partDoc = ThisApplication.ActiveDocument

Dim solid As SurfaceBody

Dim i As Integer

'get input from user

prefix = InputBox("Enter a prefix for the solid body names", "iLogic", iProperties.Value("Custom", "Prefix"))

'write input back to custom iProperty

iProperties.Value("Custom", "Prefix") = prefix

i = 1

'rename all solid bodies incrementing suffix

For Each solid In partDoc.ComponentDefinition.SurfaceBodies

solid.Name = prefix + IIf(i < 10, "0" + CStr(i), CStr(i))

i = i + 1

Next

------- end of ilogic ------

Set Your Drawing View Labels to Use the Model Part Number

Issue:

You'd prefer your view labels to use the model part number (or some other file property) rather than the default "View1", "View2", and so on. Re-naming the view labels manually is tedious and error prone. 

Solution:

You can change the view label default to use an iProperty from the model using these steps:

• Open a drawing file
• Go to the Manage tab
• Click the Styles and Standards button
• Click the Standard to work with from the top of the tree on the left pane
• Activate the View Preferences tab in the right pane
• Click the Edit button for Display field
• Set the Type drop down to Properties-Model
• Set the Properties drop down to Part Number (or something else)
• Click the Add Text Parameter button to add this property to your view label

You can click the image below to enlarge it and see the picks and clicks.

Click to Enlarge

Here is a bit of iLogic Code to set the view name and browser node to the model part number also:

'start of ilogic code

Dim oApp As Application: oApp = ThisApplication

Dim oDoc As DrawingDocument:  oDoc = oApp.ActiveDocument

Dim oSheets As Sheets

Dim oSheet As Sheet

Dim oViews As DrawingViews

Dim oView As DrawingView

oSheets = oDoc.Sheets

For Each oSheet In oSheets

oViews = oSheet.DrawingViews

                For Each oView In oViews

                oModelName = _

                oView.ReferencedDocumentDescriptor.ReferencedDocument.DisplayName

                oPartNumber = iProperties.Value(oModelName, "Project", "Part Number")

            oView.Name = oPartNumber

                Next

Next

'end of ilogic code

Update:

By request here is a rule that adds a custom iProperty to the view label with a dash separator.

'start of ilogic code

Dim oDoc As DrawingDocument:  oDoc = ThisDoc.Document

Dim oSheets As Sheets

Dim oSheet As Sheet

Dim oViews As DrawingViews

Dim oView As DrawingView

oSheets = oDoc.Sheets

For Each oSheet In oSheets

oViews = oSheet.DrawingViews

                For Each oView In oViews

                'capture the current view label

                ViewLabel = oView.Name

                oModelName = _

                oView.ReferencedDocumentDescriptor.ReferencedDocument.DisplayName

                Try

            o_iProp = iProperties.Value(oModelName, "Custom", "My_iProp")        

            'add the the iProperty to the current view label, with a dash separator

                oView.Name = ViewLabel & " - " & o_iProp

            Catch

            'do nothing if error

                End Try

            Next

Next

'end of ilogic code

Creating a Basic iLogic Rule with an Event Trigger

Issue:
You've found some iLogic code online, but you're not sure how to create a simple rule or have it trigger on a save event. You've found the iLogic tutorials on line, but don't have the time to go through them right now. You really just want to know how to create a simple rule and get it working.

Solution:
Here are some basics to get you going, using some simple example code to update the creation date and author iProperties, as described at this link.

Here is the iLogic Code you'll use:

'set Author iproperty to match the system user name

iProperties.Value("Summary", "Author" ) = ThisApplication.GeneralOptions.UserName

'set the Creattion Date iproperty to the current date

iProperties.Value("Project", "Creation Date" ) = Now

'update the file

iLogicVb.UpdateWhenDone = True

To use this code first create an iLogic Rule:

1. On the ribbon, click Manage tab > iLogic panel > Add Rule button.
2. Name the new rule Name-Date.
3. In the rule text area of the Edit Rule dialog box, simply paste in the code from above.
4. Click OK to save this new rule.

Next you need to have a couple of text fields that read the iProperties (you'd likely create these text objects in your title block, but for now just create some simple text on your drawing to test this first).

1. On the ribbon, click Annotate tab > Text panel > Text button.
2. Click on screen to place the text
3. In the Format Text dialog box select the Type pull down and choose Properties - Model from the list.
4. Then select the Property pull down and choose Creation Date from the list.
5. Then click the Add Text Parameter button (looks like and X with an arrow) to "push" the field to the text box.  
6. Click OK to create the text.
7. Repeat these steps for the Author iProperty

Next set the rule to trigger when the file is saved.

1. On the ribbon, click Manage tab > iLogic panel > Event Triggers button. A dialog box displays the list of available events.
2. Click the Before Save Document event in the list.
3. Click Select Rules, or right-click and choose Select Rules from the context menu.
4. Place a check mark next to the Name-Date rule.
5. Click OK.
6. Click OK to close the event list.

Now whenever this file is saved the date and name text fields are updated.
 
Note:
You might also be interested in this post from the guys at the Being Inventive blog:
http://beinginventive.typepad.com/being-inventive/2011/07/plot-date-stamp-in-title-block.html

And this article from Paul Munford:
http://www.augi.com/library/playing-by-the-ilogic-rules 


And this article from Steve Bedder:
http://autodeskmfg.typepad.com/blog/2012/01/working-with-external-ilogic-rules.html