Avatech Tricks: Entering Property Information into the Title Block4 Sep, 2006 By: Kevin Keene
Link part or assembly information, add a prompted value or add a custom property to your Inventor title block.
This article discusses the procedure for linking part or assembly information, adding a prompted value and adding a custom property to the title block. For this example, I'll use the Autodesk STANDARD.IDW template with the ANSI -- Large title block located in C:\Program Files\Autodesk\Inventor 11\Templates.
Link Data from a Part or Assembly
How many times do you currently enter data about a part or assembly in Inventor? If it's more than once, it's too many. Linking part or assembly data to the IDW is a very useful practice that can prevent you from re-entering information, and can also reduce the chance for error.
By default, the STANDARD.IDW template title block is set to pull information from the drawing iProperties and place it into the title block. To change where and how these fields get their information, open this template file by right-clicking on the title block and then choosing Edit Definition from the context menu (figure 1).
Figure 1. Edit the definition of the ANSI -- Large title block.
After clicking the Edit Definition command, Inventor displays all of the properties, lines and dimensions that define the title block in a 2D sketch (figure 2).
Figure 2. Title block sketch representation.
To begin, right-click on the Title property and select Edit Text. Make sure the word Title is highlighted in red to that the Format Text dialog box comes up (figure 3). First delete the red Title in the text area. Next, in the Type drop-down menu, select Properties -- Model. This command tells Inventor to look at the model for the information instead of the drawing file.
Figure 3. The Format Text dialog box.
Once you have selected Properties -- Model, click the Property down arrow (figure 4) to display a list of properties associated with the model. Select Title from the list.
Figure 4. Setting the property in the Format Text dialog box.
Once you have selected Title from the list, click the Add Text Parameters button to apply the change. Title once again shows up in text area, only this time it's pointing to the title field in the model, not the drawing. Click OK.
You have just modified the first property to pull from the model. Continue the same process with any additional fields.
When you are done, right-click and select Save Title Block. Inventor takes you back to the drawing sheet. Once this file is saved as a template, this dialog box appears each time you start a new drawing with it.
Add a Prompted Value
Prompted entries force a dialog box to appear when a new IDW is created. This dialog box requests that you provide information to be placed in the title block (much like an AutoCAD attribute).
For this example, let's change the revision number in the STANDARD.IDW template to be a prompted entry. Right-click on the Revision Number property and select Edit Text. Make sure the word Revision Number is highlighted in red. This brings up the Format Text dialog box. In the Type drop-down menu, select Prompted Entry. You can now enter the revision number in the dialog box when creating new drawings. Click OK.
When you are done, right-click and select Save Title Block. Inventor takes you back to the drawing sheet and a dialog box requesting the revision number appears. Once this file is saved as a template, this dialog box appears each time you start a new drawing with it.
Create a Custom Property
So far, I've talked about default properties that exist in every model or drawing. However, there are occasions where companies need additional data that's relevant to them, but Autodesk doesn't have a property for it. This is when custom properties come into play. The use of custom properties lets you add any relevant data to a model or drawing. Once you add the custom property to an IPT or IAM file, you then can pull that information into the title block of an IDW file.
Using the same example as above, let's create a custom property within the IPT template file and then pull that information into the title block of the IDW template. Start Windows Explorer and navigate to your template file location (I found mine at C:\Program Files\Autodesk\Inventor 11\Templates) and locate the STANDARD.IPT template file. Right-click on the STANDARD.IPT file and click iProperties. In the Properties dialog box, click on the Custom tab (figure 5). In the Name field enter the custom property name (Part Crib Number), change the type if needed and click Add. Close the Properties dialog box.
Figure 5. Custom tab in the IPT Properties dialog box.
In order to add the custom property to the title block in the STANDARD.IDW, create a temporary model using the newly updated STANDARD.IPT template. Start a new part file using the updated IPT template. Save the file as Part 1. Switch to the IDW template file that you are modifying above. Place a blank view from Part 1. Right-click on the title block and select Edit Definition. Using the Text command, place text in the title block area. I'm placing mine in the lower left corner. When the Format Text dialog box appears (figure 6), change the Type to Custom Properties -- Model and the Property to Part Crib Number. Click the Add Text Parameters button to apply the change. Click OK. You should see Part Crib Number in the lower left corner of the title block (figure 7).
Figure 6. Modifying the type and property in the Format Text dialog box.
Figure 7. Adding a custom property to the title block sketch.
Right-click and select Save Title Block. Inventor takes you back to the drawing sheet. In the tree browser, right-click on the View from Part 1 and delete it. Save the STANDARD.IDW template file. Close all files.
Now it's time to practice using this file as you would in everyday business. Start a new model using the STANDARD.IPT. Create a part. In the iProperties of that part, modify the Title field located on the Summary tab, then add 1234 to the Part Crib Number field located on the Custom tab. Save the file. Start a new drawing using the STANDARD.IDW. Inventor prompts you for a revision number. Enter A. Place a view from the new part you just created. The Title, Author and Part Crib Number should all be filled in (figure 8). Save your IDW.
Figure 8. Finished title block.
Hopefully you can see the benefit of editing your title block to create prompted entries and to automatically pull standard and custom properties into your drawings.