Inventor: Everyday Tips & Tricks
Autodesk Inventor® 2012 is arguably one of the easiest software packages to learn, and possibly the easiest operating CAD platform I have ever seen. Ease of use aside, there are numerous shortcuts and new ideas that some folks just haven’t run across yet. The following is a collection of tips and tricks that I use daily, and that I hope will benefit everyone.
This panel on the Assembly tab of the ribbon is a collection of powerful assembly tools, which reduce numerous steps down to almost nothing. Here are a few of my favorites.
Ground and Root
This tool is one of the most sensible and productive tools introduced in the latter revisions. It can be found in the Assembly tab of the ribbon, under the Productivity tool panel.
When placing the initial component into the assembly environment, it is placed at the assembly origin and then grounded. Subsequent component insertions are placed freely in space.
Use Ground and Root Component to pick any ungrounded component that is already in the assembly, and have it grounded at the parent assembly’s point of origin (0,0,0), with the axes aligned similarly.
For those who utilize a lot of skeletal modeling techniques, this tool is quite useful.
Place at Component Origin
This tool uses the Place command to insert a component at the origin point of any selected component in the assembly.
After the components are inserted, they are constrained with three mate constraints on the three origin planes. This works great for anything that has been designed with a common origin point.
Level of Detail
It can’t be said enough how powerful a custom Level of Detail (LOD) can be. The best example of its use is for reducing the complexity of an assembly. LOD works by allowing you to suppress various components in an assembly, and saving the state as a LOD with whatever name you choose.
Very often when one assembly is fitted to another, minor details such as pins, some bearings, and interior components add nothing to the benefit of the user. In fact, the greater the number of components Inventor is trying to display, the poorer the performance. So why not get rid of them until you need to see them in a more detailed view?
These named LOD are passed with a placed assembly, and are available to be switched back and forth, without having to open or edit the subassembly. Additionally, you can save a LOD in the main assembly, which captures the LOD in sub-assemblies and triggers them back and forth as needed. This is referred to as a nested LOD. A good example of this is a working “Low LOD.” If you don’t want much complexity in the main assembly, then you probably don’t want complexity in the sub-assemblies either. Create a Low LOD that includes the Low LOD state in all the sub-assemblies. Then you can minimize the entire group of components from one location.
Figure 2: The Create Substitutes tool. Notice the nested LOD.
Create Substitutes takes the large number of steps to reduce the complexity of an existing assembly and reduces them to a push of a button.
In Figure 2, I have two small sub-assemblies in an overall assembly file. Let’s say we needed to reduce the weight of the overall assembly, and need to create new Substitute (LOD) for each, and replace the existing components with part files that look like the original assemblies, but with substantially reduced features. That’s a lot of file manipulation developed into one step. Here’s how to use it:
- Open every top level component assembly that is in the parent (current) assembly, and create a new LOD in each file called ‘SubstututeLevelOfDetail1’.
- Create the new LOD substitute part for each component assembly file.
- Place the substitute part into each component assembly under the substitute LOD.
- Create a new LOD in the parent assembly with the same name as was created in each sub-assembly files (Nested LOD).
At this point, every top-level sub-assembly currently active has been replaced by substitute part files, corresponding to the LOD named ‘SubstututeLevelOfDetail1’. When the Master LOD is activated, the Master LOD is activated in each of the replaced components, bringing the complete complex assembly back into existence. Returning to the reduced complexity model is as simple as activating the ‘SubstututeLevelOfDetail1’ LOD.
Reduced Component Colors in Nested View Representations
Along with various techniques to reduce the complexity of models to speed up response time in Inventor, the colors and textures of components play a role. Component colors must be calculated in order to display them as directed.
It is recommended that those who use realistic and complex colors on their Inventor components should use two sets of colors. One set has a reduced complexity and one represents the realistic color with which they wish to render. Then you can apply a separate View Representation that captures the two different color schemes in each part. Like LOD, View Representations can be nested. From the assembly, all components in all sub-assemblies can be colored realistic, or basic (or whatever you desire) from one easy location as well.
No list would be complete without some hotkey definitions. With my AutoCAD background, I’m a hotkey nut. Here are a few for the assembly environment that I use often:
- G – Rotate
- V – Move
- P – Place
- C – Constrain
- Tab – Demote
Figure 3: The Open Gesture
Inventor 2012 brought with it gestured commands. Just right click and drag to do things such as create welds, open sub-assemblies, and turn on and off visibility of planes. They can be quite powerful, as I demonstrated in Autodesk University using Publisher, which had gestures before Inventor.
The only trick is to learn them all. Each section of Inventor has a different marking menu, and so different gestures are available. While it can seem overwhelming, it’s a great thing to master.
Bill of Material
You can do numerous things with the Bill of Material (BOM) in Autodesk Inventor. I think that often it is overlooked, or at least under-valued, in many training circles.
Add a Property Column
This is a simple function, but bears mentioning, especially for those who do not get formal training. You can add any property as a column in the BOM: Simply right-click on the BOM header and a Customization dialog will appear with all the properties that can be added. Find the item that you want display and drag it to any position on the column header.
Figure 4: Dragging a new property column into place in BOM.
Modify Part Properties Remote
While you are in BOM, you can modify the properties of one of more parts without having to open them all. Simply Select them in the BOM, and pick the property field you wish to alter. The changes will be sent back to each part file automatically.
Figure 5: Changing the material properties for components through the BOM. Notice the mass properties to the left.
Mass Properties of Sub-Assemblies
Review the Mass Properties of sub-assemblies easily without having to navigate to each through the Assembly Browser. Just add the Mass column to the BOM. Don’t forget the ‘Update Mass Properties’ button at the top right of the BOM dialog, if any changes are made.
Multibody Solid Creation
I have found the New Solid in the part modeling environment to be one of the most useful tools for developing mating components. Since all the solids are together in one location, references are easier to create, manage, and are less prone to failure. Give it a try if you are not yet using the functionality; just pick the New Solid button when adding solid features to the part environment.
Figure 6: Create New Solid button in the multibody solid operation.
I use this functionality continuously throughout my work. Derive creates a feature definition in the part environment from a feature in another file. This is super useful when developing objects in the multibody solid part environment, as mentioned above.
Figure 7: The Derive, Make Part, and Make Component Commands.
Once the derived features are added to the part file, any form of continued improvements can be made. You can develop unique variations easily by creating a base shape with the standard features common to all parts, and then derive it into each part file for the remaining modifications. Solids can be derived as well as numerous other features including work features and parameter, to name a few.
Figure 8: Options in the Edit Derived Parts dialog.
These update perfectly when changes to the original file are made, which makes it the best way to transfer design information in the top-down modeling strategy.
Derive a Surface
Another thing that should be noted is that solids can be derived into a part file as one of four different definitions.
Figure 9: The Derive Style Options
- As a single solid, with seams merged out.
- As a single solid, with the seams intact.
- As separate solids.
- As a representative surface.
The latter is especially useful when you need geometry in another file, but don’t want the mass.
Make Part and Component
These two commands automate the creation of derived components by packing all the options into a convenient location. Derive is used while working from within the resulting (often empty) part environment. Think of it as a wide receiver.
Make Part and Component employ the Derive command to create the derived part from within the parent (often multibody solid) part file. You might see this as the quarterback. The benefit of Make Component is that it will create an assembly file on the fly, and Ground and Root the individual new components in their correct relationship before it’s done.
This is a beautiful tool for creating most of an assembly from the comfort of your multibody solid environment, and then farming the entire component assembly out with the push of one button. Each file can be named how you see fit, and individual template and parameter options are available.
For any who have not upgraded recently, you are missing out on a whole lot of smooth operation. Great tools such as direct feature manipulation are proven and really cut down on some of the frustration that comes from repetitive workflows like Fillet and Chamfer of edges. Just pick the edge and choose from the command glyphs that appear.
Figure 10: Direct manipulation glyphs.
Numerous commands have been added to this functionality, such as picking a face and selecting the Create Sketch glyph; very fast and convenient.
Reference Work Features Whenever Possible
One of the things I can’t stand is when I reference a new sketch or component from a feature face and the feature is removed by a later edit. What happens? The references collapse.
Whenever possible, when you don’t have the luxury of multibody modeling, use work features, origin planes, and derived parameters to establish the mating surfaces and geometry of joining components
“But it’s so easy to pick a face and go!” Too bad. Don’t do it. If you take the extra time to develop solid work plane and work axis-oriented geometry, your assembly updates will run smoother and you will have more confidence in a greater complexity of designs.
Figure 11: Skeleton part file controlling four major sub-assembly regions. Notice that it is controlled from through a derived link to a master skeleton part.
We rely heavily on skeletal models. These basic sketches drive constrained work features that are derived throughout the entire design. Even if the constraints fail, you can easily re-constrain the work feature and get back on track. This is not so with failed projected geometry.
More Shortcut Keys
In the part environment, additional shortcut keys are available. Here are the ones I use often:
- F7 – Slice Graphics
- C – Circle
- D – Dimension
- E – Extrude
- F – Fillet
- H – Hole
- R – Revolve
- X – Trim
- = – Equal length constraint
Sunith Babu has a great list on the CAD Professor site if you’d like to see them all. http://www.cadprofessor.in/2010/03/autodesk-inventor-keyboard-shortcut-guide/#axzz1mBbDTIUT
Tolerance Referenced Parameters
Many companies prefer to tolerance at the paper level only, allowing technicians to keep all dimensions basic and engineers to manage these details on paper. For those who want to use tolerancing, here’s one method I use to manage my toleranced features globally.
Reference-in key parameters from a central location using the ‘Derive’ command. An alternate method, and in the case of the image below, is to model key mating features right inside the master skeleton file, using multibody solids that are derived out.
Then apply that key parameter directly to all related features, such as both the shaft and sleeve. Once the parameter is applied, it’s quite easy to tolerance the shafts and sleeves as needed, using one common overall basic dimension for all common features.
Figure 12: Toleranced mating components that make use of the same parameter.
When the shaft diameter needs to be revised, all that has to be done is to change the one key parameter in the master skeleton part file. Changes are handed down evenly and automatically to all toleranced components.
I want to mention Autodesk® Vault Professional as a tip. I know it isn’t Inventor, but it is an amazing tool for organizing your work. One thing that I love is how easy it is to move a component file that has been referenced in an assembly and saved with the wrong path. We simply move the file to the correct location in Vault, and the new referencing is all taken care of seamlessly (and without prompts and warnings) when the assembly is reopened. I honestly don’t want to work on a project without it.
John Evans is an Autodesk Certified Inventor Professional living in the Florida Panhandle, where he provides technical troubleshooting at Guston, Cothern, and Tucker, Inc. His career, through the aerospace design, manufacturing, and maintenance, spans 24 years and include a tour in the USAF. John now works as a design consultant and author from his company John Evans Design and manages the blog "Design and Motion," where he combines his passions: Autodesk Inventor, simulation and motion control. He can be reached at firstname.lastname@example.org.