Inventor Shafts and Splines
Autodesk Inventor® has had nice shaft design tools for some time. While the complex manner in which Inventor delivers the shafts might seem overdone, it offers some unique capabilities with a fabulous user interface.
I was working with other CAD software to develop some preliminary compressor designs, and wanted to automate the splined shaft designs. I was quite disappointed to learn that not only would I need to manually add common shaft features, but also what features were included would need to be manually adjusted if changes were required later. I don’t know about the business you are in, but in mine, changes are always required.
That led me back to Inventor, just to feel how nice a shaft design user interface (UI) could be, and this article.
Figure 1: Splined shaft and hub example.
Inventor Shaft Design
Any long-time AUGIWorld reader will know that I love the design accelerators in Inventor. I think Autodesk did a fine job of putting the features and UI together in a well-rounded package. The only problem I have is that it can be a bit tedious editing accelerated features because they should be edited through their editing dialog. This is a small price to pay for the ability to return to the design and modify the shaft design in an easy, consistent, and stable manner; a blessing of untold proportion.
Shaft design is grouped within the Design Accelerator tab in the Assembly environment. You might ask “why the Assembly environment, when I am trying to develop a part?” The reason is that power transmission components such as shafts and bores, gears, splined shafts and hubs, bearings, etc. are all part of assemblies, and designing these is a function of an assembly. In addition, Inventor enables users to automate the sizing of additional components, such as bearings and splines, based on the size of mating component features in the assembly.
From the Design Accelerator tab, picking the ‘Shafts’ tool will open the Shaft Component Generator dialog box.
Figure 2: The Shaft Component Generator dialog box opened. Notice the references highlighted in the Assembly Browser, and the adjustment glyphs on the selected feature in the Graphics Window.
A generic shaft design fills the features area as a starting placeholder, a model of that follows the cursor, and the process of placement and design is begun.
The toolset includes:
- Design, Calculations, and Graphs tabs
- Import/Export Configurations, Component File Naming, Enable Calculations, Reset Calculations, and HTML Report buttons
- Placement Buttons and Assembly Mate option
- Sections/Bores pulldown, section and bore type (such as cylinder, taper, etc.), and assembly component geometry selector
- Feature type and options
- Lower expansion (messages and warnings), right expansion (feature size list), as well as the chevron that expands the saved configurations area, similar to the Bolted Connection dialog
The placement is directed by feature references such as circular faces, axes, planes, etc. until the user is satisfied with the location.
TIP: Expand the feature group in the Assembly Browser that you want to use to reference and place your shaft by. You can easily select these rapidly when you start your shaft design right from the browser without having to struggle in the Graphics Window.
Each feature on the shaft can be modified by selecting it from within the dialog and/or the Graphics Window. Once selected, the feature is highlighted in the Graphics Window and glyphs appear that allow dragging and resizing. Furthermore, the size and location can be modified by picking the ellipsis button at the right of each Section in the “Sections” area of the dialog box.
Shaft functionality is divided into Sections. Each Section consists of concentric masses arranged along the shaft axis, namely:
The length, width, and number of faces for each can be changed easily, and each Section can be split at will.
Figure 3: Shaft Sections – note the end treatments flyout showing treatments and reliefs available.
Start and end treatments for each Section include:
- No Feature – left unchanged
- Fillets and Corner Rounds
- Reliefs – SI, DIN, and GOST types
Users can arrange these however they desire.
Figure 4: Add Features button.
In addition, features may be added within the limits of each section, as many as needed, including:
- Keyway Grooves
- Retaining Ring recesses
- Wrench flats
- Reliefs (SI)
- Through hole
- Grooves – Concentric (A) and Tangent (B)
Each of these can be edited, like the Sections themselves, in the dialog boxes initiated with the ellipsis button attached to each, or graphically by dragging the glyphs attached to the 3D model in the Graphics Window.
Figure 5: Retaining Ring Library – note the company- and standard-based selections.
In addition to features segmenting the shaft, Bore sections can be added along the shaft and are defined with measurements from either end. These are added by the Sections pulldown, replacing the editing area of the Sections (see Figure 4) with the Bores that are present.
Figure 6: Bores present are found in the Sections pull-down.
Once the shaft Sections have been established, designers can proceed to the Calculations tab and apply loads and supports to the shaft as needed for basic static engineering calculations. Again here, glyphs and markers are present in both the dialog box and the Graphics Window, allowing easy additions and editing of loads and supports.
Figure 7: The Calculations tab – note the support and load glyphs in the Graphics Window and the dialog box.
The Loads available are:
- Radial and Axial Force
- Continuous Load along the section
- Bending Moment
- Common Load – combined loads in one definition
Supports include both fixed and free types, which if enabled, will allow calculations to consider the support subtended by bearing type.
Figure 8: Support types.
At any point, the Calculation button may be picked and the updated results thereof are posted in the Results panel at the right side of the panel (see Figure 7).
The results shown include:
- Maximum Bending Stress
- Maximum Shear Stress
- Maximum Torsional Stress
- Maximum Reduced Stress
- Maximum Deflection
- Angle of Twist
Below these, the specific makeup of each load and support are displayed—all of which can be offloaded to an HTML report with the push of a button (see Figure 2, item 2).
In the Graphs tab, graphic representations of individual calculations may be reviewed as well as the combined stress on the shaft.
Figure 9: The calculation results Graphs tab.
Inventor Spline Features
I do a fair amount of shaft and hub design; manually extruding these features repeatedly is not part of my plan.
Figure 10: Parallel Splines Connection Generator.
Splines are created through the Splines tool found on the ribbon’s Design tab. Actually, you should see “Parallel Splines,” and if you pull the tool down, you will also find “Involute Splines.” For the scope of this discussion, we will cover Parallel Splines.
Starting the tool opens the Parallel Spline Connection Generator, a dialog box with the following features (see Figure 10):
- Design and Calculation tabs
- File Naming and Enable/Disable calculations
- Spline Type pull-down, along with respective size and length controls
- Shaft Groove controls
- Hub Groove controls
- Shaft/Hub feature selection
- Message box
The tool is called a Connection Generator because it can discern features that exist and create matching splines for the mating component, as well as creating both shaft and hub splines simultaneously.
When creating new splines, Inventor expects users to identify which standard they want to reference. Inventor offers S.A.E, DIN, ISO, and GOST, with variations for light, medium, and heavy duty in some cases; there are 13 total categories. In each, there are numerous sizes from which to choose
In order to continue, the user will need to select the outer diameter face, and a starting plane (or face) as references for Inventor to use.
Tip: Review the standards well, and create a cheat sheet that describes the features you are concerned with. If the shaft or bore diameters are not available in the standard, Inventor will alert the user, but will not change the size of the feature. It’s best to know the size and set the diameter before starting the tool.
Glyphs appear on the shaft (or hub) that permit the user to resize the feature directly in the Graphics Window, as well as by direct input within the dialog box.
Tip: New users are often frustrated that the generator will not continue after the respective settings are added. Make sure you check the Shaft/Hub feature creation option (see item 6 on Figure 10). This is set to both shaft and hub by default. If you are only creating a shaft spline, Inventor will still be waiting for the hub. Check the hub option off and Inventor will create the feature.
Figure 11: Creating Hub Splines – note the shaft creation option is off and Inventor is using the splines from the existing shaft to size the hub splines.
Once the settings have been applied and OK is picked, the features are created as subassembly components and added in the Assembly Browser, just like the Shaft components mentioned earlier. In the event that users need to edit these, simply pick the component and select “Edit Using Design Accelerator,” or conversely “Delete Using Design Accelerator.”
Figure 12: Editing Design Accelerator features.
Users can edit these generated components directly without this option. For example, if you needed to add some faces and geometry to a Design Accelerator shaft, users can add those features and it will not affect the Design Accelerated features. However, I encourage users to use the “Edit” and “Delete using Design Accelerator” option whenever the Accelerator-specific features, such as a different standard, need to be adjusted or simply removed. Inventor will clean up its tracks, deleting components and features or adjusting part extrusions and parameters automatically.
In some cases, the Design Accelerator features being loaded through assemblies can begin to crowd your browser a bit and create additional complexity. It is a small price to pay for automation like this. Could it be better automated, like better positional automation within mating components, like maintaining bearing and mating journal alignment? Possibly. Can the complexity of the file and assembly structure be simplified? Perhaps. However, considering how well the existing feature set works, it’s a small price to pay, and not something I am overly concerned about.
Having the standards in one place, selectable and automated, is a dream. And being able to edit these later in the design without concern that the components will have to be recreated is a real comfort. It is one of my favorite things that Inventor offers. Let’s face it, calculating involute spline profiles once is bad enough. Repeating the process in the assembly is not an an option.