Creating and maintaining custom symbols in Inventor

By John Garcia,
MCAD Solutions Engineer
Hagerman & Company
San Jose, CA

Have you ever needed a custom symbol to do something specific in an Inventor drawing? If you can create blocks in AutoCAD, then you have the skills needed to create and maintain your own symbols in Inventor. One of the first ones I found that I needed was a note reference callout (a box with a number in it), with the ability to enter any number I needed. To start off, we right click on Sketched Symbols in the Drawing Resources and choose Define New Symbol.



This takes us into the sketch environment where you will find all your familiar Inventor sketching tools to create with. Create your desired shapes, add dimensions if desired and then the text can be added. When creating the text, the type needs to be changed to “Prompted Entry” so that it will ask when inserted. Within the carats, the prompt the user will see when inserting is filled in; also apply any text justification here for relative positioning of the text within the symbol.

The text is placed and then oriented to the desired position within the symbol, and then one may simply right-click and choose Save Sketch Symbol to create it. A dialog will appear asking what you would like to call your new symbol, as shown below:

The Sketched Symbols section of Drawing Resources will list this newly created symbol as an available resource. It is stored within the current drawing similar to an AutoCAD block definition – it is only available to this drawing at this time. The symbol may be used in a number of ways, and Inventor includes one very useful built-in tool that allows all defined symbols to utilize a leader without the user having to create any additional customization to the symbol itself. The symbol may be utilized by either double-clicking on its name under Sketched Symbols (or right-click and choose insert). This will display the symbol on the cursor for placement within the drawing and once placed, a dialog prompting for the desired number will appear.

Note that this method does not give the user the opportunity to use the symbol with a leader. Another method of accessing symbols must be used to utilize this capability. In the Drawing Annotation Panel, there is a selection simply called Symbols. When selected a list of the available symbols will open for the user to select from, and there is an option to use the symbol with a leader.

Using this method, the symbol first starts with a user-defined leader, allowing multiple picks for the leader. When the leader is done, right-click and choose continue to place the symbol – the last pick point will be the location of the symbol and the leader will be trimmed to match the symbol. To edit this symbol, we once again return to the context-sensitive right mouse button, click on the symbol and select edit field text; the dialog will then open for editing.

To expand on this, attachment and insertion points can be added for other types of symbols. Perhaps a company has a number of similar parts that all use the same notes. Those notes may be created as one symbol and shared among all of the drawings easily. Start by creating a new symbol, with standard text. Next create a point somewhere above and to the left of the text:

The text has an attachment point that is based on the justification of the text and that point may be used to locate the text relative to the newly created point using dimensions. To make this point useful as an insertion point, the point style must be changed.

Click on the point to highlight it in the drawing and, on the styles area of the main toolbar, select the point style (default is “center point”). Change the point style to Set Insertion Point Grip – the cross with red dot shown. An attachment point functions similarly except that it is not used as an insertion point – you can use these to “stack” and align your symbols or attach to existing points on a title block or border.

When placing this symbol now, this point will be used as the “handle” for the symbol and the insertion point will “grab” onto available attachment points, in this case the upper right hand corner of the border (default). By changing the style of this point, it will not be visible as part of the drawing. When moving this symbol, it will again be attached to the cursor by this point.

Now that these symbols have been created, they are easily transferred to other drawings with a simple copy and paste via Drawing Resources. To make them always available in a new drawing, simply paste them into your default drawing template(s). Armed with these techniques and perhaps a few more that can also quickly be researched and learned, it should not be too hard for someone to be able to create their own Inventor title block in their default template, as a title block is little more than a specialized sketch symbol.