Getting Blocky with Drawings in Inventor

How to work with Inventor’s drawing blocks.

It is common for a CAD application to have the means of grouping objects together. The grouped objects then behave as a single element. AutoCAD does this through blocks. In Inventor’s drawing environment, you can also group elements together into Sketch Symbols.

For drawings, Sketch Symbols improve productivity. Why redo when you can just reuse? Sketch Symbols build consistency as you use the same block repeatedly. Extend this to your team and now everyone is using the same symbols in their drawings. Update the symbol definition and you can update your drawings to match.

Sketch Symbols

Within drawings, blocks supply a more traditional use. In Inventor, drawing blocks are called Sketch Symbols. Use these to build custom symbols. Symbols that you will use often. These can be simple, like NOT FOR PRODUCTION, or more involved, like a title block and border.

In the browser, you will find the Drawing Resources folder. This lists the Sketch Symbols contained within the drawing. You can add your own subfolders, then drag the symbols into them for further organization.

Borders and Title Blocks are special sketch symbols. The process of creating these is the same, but Inventor provides special workflows for working with them.

Pro Tip: If using DWG for drawings, you can use AutoCAD blocks in your drawings.

Your sketch symbols live in drawings or templates, but you can also save them to a library for sharing among team members. A library makes it easier to use your symbols in other drawings.

Quick Insert

To insert a symbol, right-click on it within the browser and select Insert (or double-click it). Then pick the location within the sheet. If the symbol has prompted text, Inventor will display a dialog and wait for the inputs. Inserted instances appear within the Sketch Symbols browser node for the current sheet.

With Insert, the symbol is added statically (as is). There are no options for setting the scale or rotation. Although there is no leader, you can add a vertex/leader after insertion.

Inserting Sketch Symbols

Another choice is the Sketch Symbol command. You’ll find it on the Annotate tab or from the menu when right-clicking a symbol in the browser.

In the Sketch Symbols dialog, select the symbol for insertion. If the drawing has many symbols, consider using the search to quickly locate the symbol. Set the Scale and Rotation.

Enable Static to disable the ability to scale or rotate the symbol after insertion. When disabled (i.e., unchecked), scale and rotation grips appear when you select the symbol in the sheet.

Check Symbol Clipping when you want dimension, leader and extension lines to go behind the symbol and appear trimmed by it.

When you add leaders, in addition to pointing to specific objects, the symbol associates with the selected model’s properties. You can use this metadata (iProperties) in the symbol’s text. If you don’t want the leader but you still want to associate with the model, consider turning off its visibility rather than deleting it.

Pro Tip: When inserting a symbol without a leader, hold Shift as you move over the bounding box of an existing sketch symbol. Click when the green dot appears and the new symbol stacks at the side of the selected symbol.

Creating Sketch Symbols

The Basics

To build a sketch symbol, right-click the Sketch Symbols browser folder and select Define New Symbol from the menu. You can also find this on the ribbon in the Manage tab.

Then, sketch the geometry you want. You can use constraints and dimensions to set the symbol to the exact size and shape you want. Your Sketch Symbols can have 2D geometry, text and images.

Pro Tip: Set geometry to Sketch Only for construction/reference type geometry if you don’t want it to appear in the symbol when it is inserted into the drawing.

When creating sketch symbols, use the point tool to set the insertion point location. This is the point used to position the symbol when you are placing it on a sheet. To move the sketch symbol precisely in the drawing, add one insert point and several connection points. Use connection points to snap the symbol to other geometry.

Styles manage the appearance of the sketched objects. Use the Style Editor to change the Object Defaults for sketch symbols.

When you are finished, select Save Sketch Symbol to commit the symbol to the drawing. Inventor will prompt you for its name, which will be available in the Sketch Symbols folder.

What’s in the text?

The text in your sketch symbols can be static, fixed text. But with text for Sketch Symbols, there is so much more!

Use the Prompted Entry type to build questions for the user to answer when inserting the symbol. In the text box, the text you enter becomes the text that will be shown in the Prompted Entry dialog. For AutoCAD users, this is like block attributes.

For example, “paint color?” prompts the user to enter the color of paint used on the design.

Pro Tip: Sketch Symbols can have many prompted entries. The default order is the order of creation. However, use the Reorder Prompted Entries feature to adjust the order.

For auto-populating text, use one of the property types. Use the Type and Property drop-down list to set what you are extracting. The Source sets where the information is coming from and the Add button inserts the field into the text.

Inventor prefixes and suffixes the field with brackets (< >). Unlike Prompted Entries, you cannot remove the brackets. In the text editor, you should also notice the field highlighted in gray.

You can also surround the property fields with static text. Text can also contain multiple property fields.

Use the iProperties type (Standard and Custom) to extract iProperty information from the primary (or attached) model or from the active drawing. The primary model is the model of the first view on the first sheet. The primary model is what the sketch symbol uses if there is no leader.

If you use a leader with the symbol and associate a model (select an edge) with it, then the iProperty information will be extracted from that attached model.

Pro Tip: With the newer versions of Inventor, you can adjust the primary model by editing the sheet.

Drawing and Sheet Properties come from the active drawing. This includes properties like the sheet number, sheet size and the number of sheets.

Physical and Sheet Metal Properties can only come from the primary or attached models. Use this to include the mass, volume, surface area, flat pattern extents and other model properties.

Symbol Library

To add a specific symbol to a library, right click on it within the browser and select Save to Symbol Library. To add all a drawing’s symbols to the library, right-click on the Sketch Symbol node in the browser and select Save All to Symbol Library.

In the Save to Symbol Library dialog, select the library and click Save. Optionally, you can also enable Retain Resource Folder Structure to publish the folder structure to the library.

If no library exists, select Create a New Library. This creates a new IDW drawing, which Inventor uses as an external library. The Application Options (File tab) sets where libraries will be created and referenced.

You cannot save two sketch symbols to the same library with the same name. In these instances, the Paste Resource dialog displays, prompting you to replace the existing symbol or create a new symbol. When selecting New, Inventor prefixes the symbol name with “Copy of.” You can rename it after that.

Inventor also displays the Paste Resource dialog when trying to insert a symbol from the library that already exists in the drawing. In this situation, select Replace to update the definition and all instances inserted into the drawing.

Editing Symbols

To edit a symbol, right-click on it in the browser or drawing canvas and select Edit Definition. This puts you back into the sketch environment, where you can make the necessary changes. By saving the changes, Inventor updates the definition and all instances in the drawing.

Title Blocks and Borders


The Default Border is special because you will find it in every drawing. When inserting into the drawing, you define the zones and margins and the border conforms to the sheet.

Pro Tip: The Default Border is dynamic as it automatically adjusts to changes that are made to the sheet size. The size of the border is managed by the margins you set. You control the inclusion of zones.

Creating a custom border is like creating a sketch symbol. Right-click the Borders browser node and select Define New Border. In the sketch environment, build the border with geometry, text and images.

Unlike sketch symbols with borders, the insertion point is irrelevant. Inventor places the border as it lies within the sketch. So, use dimensions to locate the border from the lower left corner of the sheet.

Connection points are important if you want to snap other objects (like sketch symbols) to the border.

Connection points also set the location for title block placement. The outermost corner of the title block attaches to the connection point. If there is more than one connection point per drawing quadrant, the title block attaches to the point farthest from the center of the drawing.

To start your custom border with zones, use the Define a Zone Border option. You set border parameters first, like the number and type of zones. Then you can add, remove and change geometry.

Title Blocks

There is not much to say about title blocks that we have not already discussed. Create new title blocks by right-clicking on the Title Blocks browser node and selecting Define New Title Block. The options match those when you create sketch symbols, including the various types of text.

A sheet can only have one title block. Therefore, if you try to insert another title block, Inventor will prompt you to delete the existing one before inserting the title block.

More Tools

The Drawing Resource Transfer Wizard is a stand-alone tool included with Inventor. Use this to copy Drawing Resources, like Sketch Symbols, from one drawing into other drawings. You have the choice of whether to update existing resources or create copies.