Using Inventor Sketch Blocks for Feature Placement

When we uses AutoCAD for our 2D designs, we often turned to the Block and sometimes the Group feature to combine numerous entities together in order to select and perform operations on all the entities at once.  We could not live without them.  Along came Dynamic Blocks and we found even more uses for them.

A lot of designing has moved into the 3D world as we moved from AutoCAD to Inventor but our love for blocks did not follow along.  Inventor has the ability to create and save Sketch Blocks inside IPT files.  These blocks can be simple or can be complex parameter sketches that group sketch entities together making repetitive sketches easier and definitely faster.  In this article I want to demonstrate one use of a parametric sketch block to place an external shaft keyway.  

One of the first things to consider is where you would like to develop the sketch block.  This block will be used for the design of numerous shafts so you may want to place it in your IPT template.  Some designers use a master sketch block part where all the special sketch blocks are saved and can be copied to any new part when needed.  We will get into the methods of doing this later.  I will be choosing the second method.

The first step is to create a master sketch and add dimensional parameters to it. I also changed the color property of the sketch entities.  This will serve two purposes, it will denote that this is a sketch block and the color change will be dramatic when it is placed and full constrained.  The original parameter values are not important, these are for a 2 1/2 inch shaft.

The next step is to create the sketch block.  While still in the original sketch, select the "Create Block" command.  You will find it under the Sketch tab in the Create drop down menu in Inventor 2018.

The "Select" icon will already be highlighted in the Create Block dialog box.  Using a window or crossing select all the entities from your sketch which will be a part of the sketch block.  Do not worry about the parametric dimensions, they will be included automatically.  Once you are finished selecting your sketch, pick the "Select" icon under Insert Point and I suggest also placing a check mark in the "Visibility" box.  This will show a small red "+" on the block indicating the insertion point when you later place the block.  This of course is not required.  Give the block a distinctive name since you may have other sketch blocks in your model, a description is optional.  Select the "Insert Point" in your sketch and then select "OK" to finish and create your sketch block.

If you make an error, you can select the newly created block and right click to bring up "Edit Block" in the context menu.  This command is available if you are in the original sketch or not.  One note of caution here, you cannot edit the insert point using this routine.  If you selected a bad insertion point, delete the sketch block from the Browser folder and recreate it.

Once you are satisfied with the sketch block you should delete the original development sketch from the model.  Last you need to save the IPT or IPT template to make the sketch block a permanent part of the IPT.

Now you should try out your creation.  If the sketch block was created in your IPT template, create a new drawing, if it was a part of a standard block IPT, as mine was, use the "Save As" command to create a new IPT.  Either method will create a new part model with the included sketch block and the parametric values.  I will talk about other ways to create a new files later on in this article.  

In your new model create your shaft.  If you use the "Cylinder" primitive function this step will take you only a few seconds.  For my demo shaft I will create a 3" Diameter shaft, 10 inches long.  At this point do not add any end chamfers, it will only complicate the placement of the sketch block.  Next you will create a workplane tangent to the outside surface of the shaft parallel to one of the origin planes running the length of the shaft.  At this point the model looks like this.

Next create a sketch on the workplane you just created.  You are ready to place the External Keyway sketch block.  This can be done using one of two methods, either left click and drag the sketch block from the Browser folder or right click on the sketch block and select "Place Block" from the context menu.  One the sketch block in on your cursor select the insertion point in your sketch, probably somewhere along the axis of the shaft although this is not necessary since you will be applying sketch constraints to accurately position it is a moment.

This is a completely new sketch so you will need to add sketch constrains to position the sketch block.  In my sketch block the points outside of the slot sketch will be constrained to one end of the shaft with a coincident constrain.  If you refer back to the original sketch, this point is used to locate the slot along the shaft length.  Once the sketch block is constrained it will change color, this is one reason I like to make my sketch blocks red, the change is dramatic.  

The next step is to "Extrude" it as a cut by listing the model parameters, selecting "Width_of_Keyway" then adding "/2" since all inch keyways are cut so half their width is inside the outside tangent of the shaft.

The last step is to open the Parameter table and edit the values of the sketch block to match the current shaft size.  

You can streamline the previous step by creating an iLogic table to help you fill out the parameters. 

The shaft keyway is finished!  Add a couple of chamfers to each end of the shaft and you are done.  I encourage you to do another one for practice and see just how fast you can place external keyways.

I mentioned earlier that I would cover other ways of distributing your sketch blocks.  If you have an existing part model and would like to add your configured sketch blocks to it just use the "Derive" command and select the sketch blocks you would like to include.  If your sketch blocks include parameters, do not forget to include them in your selection.

I would suggest that you "Break Link With Base Component" once you have derived all the features into your part model and even go one step further and delete the derived component from the model to avoid confusion.

The last method of copying sketch blocks and their supporting parameter values is to use the "iLogic Design Copy" command located on the iLogic panel under the Tools tab.  This is only available if you do not have any models open in Inventor.

Sketch blocks can be copied directly from model to model by right clicking on a sketch block(s) and selecting "Copy" from the context menu.  Moving to you new model, right click on top of the Browser and select "Paste".  One disadvantage to this method occurs if the sketch block has any attached named parameters.  The parameters are copied but the configured parameter names are lost.

This is just one use of sketch blocks.  You could not live without AutoCAD blocks, I think you will find Inventor sketch blocks just as valuable.