Inserting Properties into an Inventor Title Block

This is my last post in my series covering Vault Properties and Inventor iProperties.  I have previously explained that there is a difference between Vault Properties and Inventor iProperties.  Then the last two posts have been instructions on how to create the property in Vault and map properties to Inventor custom iProperties.  Once you have those properties created and mapped, what can we do with those properties?  They can be shown on drawings in Parts Lists, Title Blocks, and Borders.  So I wanted to complete the series by explaining how to get these properties onto a drawing.

Placing properties on a title block isn't that difficult, but if you haven't done it before, you may not know where to start.  Also, custom iProperties are a little bit tricky.  For the purpose of explaining how to do this, I am going to say that I want to add Stock Location and Originator to my title block and I want to add Stock Location to my Parts List.  That way someone in the warehouse can look at the drawing and know where to find the parts.

Since this is something that we want on all of our drawings, I am going to edit my drawing template.  I will need to have a model that already has those iProperties.  Then I will need to open my drawing template.  To do this properly, you want to use File> Open to open your template.  You don't want to go to File> New.  Once the template is opened, you need to add a base view of a model that contains those custom iProperties.  It doesn't really matter what the model is because we will delete the view once we have placed its properties in the title block.

So the next step would be to edit the title block.  You can right-click on the title block on the active sheet, in the browser, or on a title block listed under the Drawing Resources.  Then click Edit Definition.

This will open the sketch of the title block.  It can be a little overwhelming because you are going to see dimensions, names of properties that populate the title block and labels for those fields.  Most often these will run together and make it a little hard to read.  However, zooming in on certain sections will help.

In this example, I am using the default Inventor Title Block.  So, I think I will change QA to Originator, then place the Originator property in that block.  Then I will add Stock Location at the bottom of that column.  So first I will double-click on QA to change the text of that label to Originator.  Then, I can use the Text command to add a place holder for this property into the title block sketch.  To get the custom iProperty into the place holder, you will need to use the drop-down boxes above the text window to pick the right iProperty type\source, then the desired property.  Then clicking the "x" symbol will place that property into the text window.

After the text is placed, you can control the position of the text, in relation to the insertion point, through the two sets of justification toggles.

Then at the sketch level, the insertion point can be constrained or dimensioned to locate it properly.

So now, I am going to insert a text label, using the text command to label the last box Stock Location.  Then, I will insert the Stock Location custom iProperty into that box.  The following image is what it should look like when done.

When you are done editing your title block sketch, you can click Finish Sketch to exit sketch mode.  Inventor will ask if you want to save the edits or if you want to do a Save As.  In my example, I will just save it.

Here is a YouTube video that shows how to make these changes to the title block.

Adding Stock Location to the Part List is pretty simple, but there is a wrinkle that makes it more difficult.  The issue is that Parts Lists are style based, which means it pulls definitions from the Style Library.  So I could modify the Parts List Style in the template, but if I don't add it to the Style Library, I could have the change undone by the Style Library.  

Before changing the Parts List style, you will need to make sure that your Inventor Project has Use Style Library set to Read-Write.

I typically tell users that this setting should be set to Read-Only because I don't want users inadvertently making changes to their styles.  To change this from Read-Only to Read-Write, you will have to make sure all of your Inventor files are closed and if you are using Vault, the project will have to be checked out to you.

After you have made that change, you can open the drawing template and navigate to the Style Editor.  

Under Parts Lists, you will see all the Part List definitions in this template and the Style Library.  You are most likely using one customized to your company.  I am using the default template in this case.  So I will just copy one of the default styles because I don't like modifying the default styles.  I am going to select Parts List (ANSI) and click New at the top.  This will copy Parts List (ANSI) and ask me to name the new style.  

To add the custom iProperty, I will have to click on the Column Chooser, then select New Property.  Then I can click where it says <<Click here to add a new property>>.  Then I can type Stock Location, which is the name of the custom iProperty I want to add.  This will be case sensitive, so make sure to type it so it matches the way it was spelled in the other places it was used. 

Then back in the Column Chooser dialog, the columns can be ordered using Move Up or Move Down, which are under the selected properties.

Now the style will need to be saved, by clicking on Save at the top of the Style Editor.

So that added the column to the Parts List, but there is one other issue to consider.  Is this Parts List going to be our main/default Parts List?  If so, you will want to change this style to the default Parts List under the Object Defaults.

Doing this will make sure that Parts List w\Stock Location will be the default style for Parts Lists in the future.

Now we need to save these changes to our Style Library.  That is done by using the Save command from the Styles and Standards panel of the ribbon.

This will compare styles in the drawing to styles in the Style Library and offer to change the Style Library's styles to match the ones in the drawing.  This cannot be undone, so make sure you are ready to do this before clicking OK.

Once the styles are saved to the Style Library, don't forget to save the template and change your Inventor Project back to Use Style Library =  Read-Only.  If you are using Vault, you will want to undo your check out of that file.

Here is a YouTube video I made that demonstrates this process.

The process of adding the custom iProperty to the title block or parts lists are not too difficult.  Making sure the Style Library is updated with the new Parts List style is probably the most difficult part.  However, if you can get all your properties managed in your CAD files and in your Vault, you will have a lot easier time getting the right information to show up in the right places.