Create a title block with enhanced attributes
Hello,
Is it possible to provide a sample for AutoCAD workflow with more details such as video since the question is not that clear though?
Generally speaking, it should doable but not sure for the details.
Thanks!
Xun
You can create an iLogic form to do what you desire. In this link, the author shows you how to create a form using single list data but you could also add iLogic rules to create multi-value list from parameters.
John Hackney, Retired
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Inventor iLogic and iLogic Forms are built into Inventor, there is no add-in. You can use both to extract other data, such as parameters, into iProperties which you can then add to your title block form. Your best bet is to post what iProperties you are looking for and where you what them to come from, ie from the model or from the drawing iProperties. I believe any iProperty that is applied to the model such as heat treatment, finish, description, part number and material should always come from the model and drawing iProperties that apply to the drawing such as author, scale and required quantity should come from the drawing. You can also use iLogic to create lists of available iProperties and add these to your title block form.
Mainly, you need to let people know what you want exactly as far a iProperties that you want to populate your title block.
John Hackney, Retired
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Hello @clowe_unit I see that you are visiting as a new member to the Inventor Forum.
Welcome to the Autodesk Community!
You can create your own by simply typing the name of the parameter you want to define when creating the dimension, for example LENGTH=12.
You can also edit them from the Parameters tab.
You can expand the Add Numeric to choose different User Parameters to create.
You can also create Custom Parameters from the iProperties.
When in a Format Text Box you can Add Parameters and insert them for use.
Please select the Accept as Solution button if a post solves your issue or answers your question.
Kelly Young
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I want to expand on what Mcgyvr mention as far as a directly entering prompted information into a title block. This is NOT a recommended method of filling in an Inventor drawing title block since the information entered is not "Associative" and will not automatically update when the model or drawing iProperties change. It is called prompted entry and is very similar to what you show in your screen capture. The title block is created with "Prompted Entry" fields just like the attributes in an AutoCAD based title block are created. These are added to the title block in your Inventor drawing template and when it is placed you receive a prompted entry dialog box to fill in the values. This does not require iLogic forms or routines and is very simple to do. Again, I want to mention that this is NOT the recommended method of adding information to an Inventor title block because it is not associative.
Below is a screen capture of a prompted entry title block I created from one of my Inventor drawings as an example. I have also attached the file for your inspection, it is in Inventor 2019 form. When a template is opened with this type of prompted entry, the entry panel opens automatically. Later on you can use the indicated box to edit the entries as needed.
John Hackney, Retired
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If the information doesn't need to be tied to or pulled from model or drawing parameters/properties then there is nothing wrong with prompted entries and that is the method I would recommend using as the best solution in certain instances. 
But yes there are likely better ways like trying to utilize drawing or model iproperties and pulling them into the titleblock so you only change them in one place and can utilize that iproperty in other files,etc...
