Inserting Parameter Values into Drawing Text

The last parameter workflow that I wanted to share is how to insert a model parameter into a drawing note.  It is a feature I rarely use, but I don't do production work full-time.  The process is pretty simple but will link the value from the model to the drawing note text.  You will be at your most productive when you can create these types of relationships which cause Inventor to do the bulk of your time-consuming tasks.

To illustrate this, I thought about scenarios where drawings have notes about unmarked fillet radii.  This is where filleted edges are not dimensioned but the user will place a note that reads, "All unmarked fillets to be 1/16 in."  To make that note more intelligent, I could create a user parameter named FilletRadius, then use that parameter when creating the required fillets.  When I add the note on the drawing, I could insert the FilletRadius parameter's value into my note, instead of typing that value out.  Which would save me from having to edit the note if the FilletRadius value changes.

So the first step would be to create the necessary Model or User parameter.  For my example, I am going to create one called FilletRadius.

Then I need to create the Fillet features that use that value as the radius value.

The last step would be in the drawing file.  You start a Text Annotation as usual and type and static text that you need in the note.  For my example, I would type, "Unmarked radii have a radius of."  To get the User Parameter into the annotation, I configure the drop-down menus above the text pane.  Selecting the file, User or Model parameter, the required parameter, and the precision.  After those selections are correct, you can click on Insert Parameter, which will insert the specified value into the note text.  Then you can finish the note off with any other static text.

Here is a video demonstration of how to insert the parameter.

That is all there is to it.  Again, this creates a dynamic link between the model parameter and the text note.  This will eliminate having to update the model value and the note text if the unmarked fillet radii change.  The scenarios of where this can be useful are numerous.  Hopefully, you can use this technique to build similar relationships between model parameters and text notes.

Automation Through Linked Inventor Parameters

Building automation into Inventor models is one of the biggest requests that I hear in my job.  Customers have a few projects that they have built and they want to find a way to leverage that and build new projects faster.  In most cases, the designs have variations in them that make them unique.  When I review these customer models, looking for ways to add automation to them, I first look for ways to utilize basic Inventor functionality before considering custom programing.  One of the easiest ways to get automation into a design or project is to link parameters.  

A model's parameters can be linked to either another model or an Excel file.  Once the parameters are linked, changing the values in one location will cause the linked parameter in all the other locations to update.  In most cases, the local update icon will light up in the other files, letting you know that Inventor sees new values and wants to update the models to reflect the new values.  The process of creating the link is pretty simple but can be very powerful and save time for the user and eliminate mistakes.

To link parameters to an Inventor file or Excel file, you will first need to open the Parameter dialog box and click the "Link" button.  

Inventor will then display the Open dialog, where the user can filter based on the file type they are looking for.  

If an Inventor model is picked, a dialog box will be displayed asking which parameters you would like to link.  

If the selected parameters are not marked for Export, Inventor will ask if it is okay to mark it for export.

Once that is done, Inventor will bring all the parameters into the parameter list.  

If an Excel file is picked, the user can also pick the Start Cell for where Inventor should start reading parameter values. 

Then Inventor will add the parameters to the list.

Here is a video demonstrating the process of linking parameters between Inventor files.

Here is a video demonstrating the process of linking parameters to an Excel file.

Having done this multiple times, I have a few tips that will save you from errors and make the process more manageable.  First of all, even though you can link parameters between models, Inventor will complain about a cyclical reference if you link parameters between an assembly and one of its parts.

If you prefer to control parameters by linking between Inventor files, you could create a separate file that holds all the parameters and then link the models to that file, as a shared resource. 

If you want to link parameters to an Excel file, you have to put all the values on the first tab in the file.  I have seen customers create multiple tabs for different calculations, then push those values to the main tab.  Also, when you link the parameters to an Excel file, you will be asked for a start cell.  Inventor will then start reading that column for parameter names and use the next cell to the right as the value.  If it sees a blank row, it will stop reading values.  By using different Start Cells and blank rows, you will have better control of which parameter values get pulled into which files.  One limitation of this is that you will not be to link one part file to a specific Excel file more than once. 

Lastly, I advise you to keep the parameter names of each file unique.  If you link in a parameter named "Length" and you already have a parameter named "Length" in your file, Inventor will change the name of the linked parameter to "Length_1."  I haven't seen this cause an error or issue, but it might cause confusion.

So that is all there is to it.  Using the ability to link parameters to other models or Excel files should give you an easy way to add some automation to your new or existing project.