Inventor 2D Sketch Blocks

Have you discovered Inventor blocks yet? You probably used blocks in AutoCAD, but have you considered using them in Inventor? If you are using Inventor for conceptual design you might find the new 2D Sketch Blocks an extremely valuable tool.

In many of our designs, standard shapes are often repeated. You can make use of 2D Sketch Blocks to capture such shapes as a fixed set, and place instances of the set where needed. For example, say you have a 2D sketch that represents a component link, and there are two or more component links in your assembly. If you have a single 2D Sketch Block that represents the component link, you can place multiple instances of the 2D Sketch Block into your sketch assembly. The instances are defined in the 2D Sketch Block so any changes to the block design are automatically reflected by the instances. This is the same behavior as a block used in an AutoCAD drawing.

Lets take a look at 2D Sketch Block characteristics:

Sketch blocks are only created in 2D part sketches.
Sketch blocks are interchangeable with AutoCAD blocks.
Sketch blocks are created with user names and descriptions.
Sketch block definitions reside under the Blocks folder in the browser.
(See green arrow in Figure1)
Sketch block instances reside under the sketch in which they are placed.
(See blue arrows in Figure 1)
Nested blocks can be created in which sketch blocks are contained within sketch blocks.
(See red box in Figure 1)
Sketch block instances can be toggled to Flexible. When a nested sketch block is flexible, the block behaves similarly to a kinematic subassembly. Use this feature to investigate kinematics of your design.
(See green box in Figure 1)
The appearance or format of sketch block definitions and instances can be modified.
The default block Insert Point is the centroid of all the geometry within the sketch block. The block Insert Point is also user definable.
Block instances can be created with the Mirror and Pattern commands.


(Figure 1)

I will also point out that some 2D sketch geometry is unavailable to 2D Sketch Blocks. When such geometry is selected and the Create Block command is executed, a warning message is shown to notify you of the issue. The block can still be created, but will not include the ineligible geometry. Here is a listing of geometry that is ineligible in sketch blocks.

Arc/circle/polygon center points the entire arc/circle/polygon must be selected.
Arc/circle/spline endpoints - the entire arc/circle/polygon must be selected.
Individual spline points - the entire spline must be selected.
Projected geometry.
Derived geometry.
Geometry copied in a sheet metal Unfold/Refold operation.
Geometry placed by an iFeature.

Lets take a look at a typical 2D Sketch Block workflow.

Step 1. Create a new sketch.
Step 2. Draw and constrain the sketch geometry.

Step 3. Use the Create Block tool under the Layout Tab on the Sketch Ribbon.

Step 4. Select the geometry, insert point, and assign the block a name.
Step 5. Draw and constrain any additional sketch geometry.
Step 6. Repeat the Create Block tool for additional 2D Sketch Blocks.

A total of four 2D Sketch Blocks have now been created for this example as shown.

Step 7. You can now apply sketch constraints between the existing 2D Sketch Blocks.  In this example I used single coincident constraints for the following point pairs

• The corner of the Cabinet Door coincident with the Cabinet door hinge location point.
• The midpoint of the Cabinet Door coincident with the end of the Long Link.
• The other end of the Long Link coincident with the end of the Short Link.

The other end of the Short Link coincident with the Cabinet mounting point.

The following image shows the results.

With the 2D Sketch Block technology you can prove out your conceptual designs and theories in a single sketch as opposed to creating a multi-part assembly. Without the 2D Sketch Block technology this example would have used four part files and one assembly file just to prove a design concept. From this stage of your design, you can also take advantage of the multi-bodied solids technology to turn each individual sketch block into a solid body. (See our August 2009 Newsletter for the article on using multi bodied solids.) Once you have multiple solid bodies you can use the Make Component tool to create a final assembly and parts.
I dont know if 2D Sketch Blocks are something you will use but I do suggest you take a few minutes and at least experiment with the new technology. If you find this article interesting you might also consider taking our Level 2 Inventor Class where we try to expose some of the lesser-known tools that are available in the Inventor product.