Shimming Your Knowledge - Adding Parameters to Text in Autodesk Inventor

In my last post, I mentioned that I've been doing a lot of work with Autodesk Inventor drawings.

I've found that this week, the trend has continued.  And while this can be a bit monotonous, it has given me an opportunity to blow the dust off some old tricks I've learned over the years.

One common thing I've seen is inserting a certain value into a block of text, such as note text.  These values can be things like sheet metal thickness, bend radius, or any other value that needs to be stated in the body of the text. 

A typical example.  I've added the radius dimension for comparison.

\It's never hard to type these values in, but if the value is just typed, then it's static.  If the value is changed in the model, there's no way to make sure that value updates, short of using the good old Mark 1 memory and Mark 1 eyeball.  

So let's take a look at how to automate that process.  Let's make the bend radius note update automatically. 

Start by editing the text the same way you always have.  Right click on the text and choose Edit Text. 

The editing screen

Once inside the text editor, focus on the set of bars just at the top of the text editing portion of the screen. 

From left to right, here's the information each pull down contains, starting from left, and working right. 

• Component - Which component are you drawing the data from.  In this case, the model is named "Sheet Metal"
• Source - Are you calling the parameter from the Model Parameters, or User Parameters
• Parameter - The actual parameter you're placing. 
• Precision - How many decimal places does the parameter contain. 
• Add Parameter - This will actually put the parameter into the text. 
• Special Symbols - Expand this menu to see common drafting symbols to place. 

The toolbar to add your parameters in. 

Clicking the Add Parameters button will add the value to the text, but inside of a gray box.  This tells you that the value is being read from an outside source. The sheet metal part in this case. 

Using the Add Parameter tool to make the magic happen!

Click OK to complete the operation. Now when that value changes in the model, the value will automatically be saved in the text!  

But there's one more thing.  What if you want to adjust the format even more?  To do that, right click on the text again, but this time, choose "Edit Unit Attributes". 

Now you can change the format of the units, including units, precision, and format.  In this case, I removed the leading zero, and added the unit string to make sure the units fit my standard.

All that's left to do, is hit OK, serve, and enjoy!  The units and leading zeros are gone, and the value on the drawing will update should the model change! 

And once that's done, you're all set!  Take a look at this tool, and see how it can help you!

If you prefer to see this information in video form, take a look at the video below!