Basics for New Inventor Users
In today’s global market, as manufacturers work to reduce design cycles and cost margins, industry experts are championing digital prototyping as a way to cost effectively validate design ideas and accelerate the development of competitive products.
The Autodesk® Suites include numerous tools to help in the design cycle. Autodesk Inventor® is the central component in two of these suites (Factory Design and Product Design) and a supplementary component of another suite (Building Suite Ultimate).
Autodesk Inventor takes engineers beyond 3D to digital prototyping by giving them a comprehensive set of tools for 3D mechanical design that enables them to design, visualize, and simulate products before they are ever built. Digital prototyping with Inventor helps companies design better products, reduce development costs, and get to market faster.
Because the Inventor model is an accurate 3D digital prototype, it helps users to check design and engineering data as they work, minimize the need for physical prototypes, and reduce costly engineering changes discovered after the design has been sent to manufacturing.
Autodesk Inventor has several types of files that you must understand before getting started. These include basic modeling file types as well as project files. Unlike AutoCAD® where there are only two files types to manage (DWT and DWG), Inventor uses separate files for reference management, part, assembly, presentation, and drawing design.
Project Files (.ipj)
As you create designs in Autodesk Inventor, file dependencies are created between files of different types. For example, when you create a 3D assembly, a file dependency between the assembly and its part models is created. As your designs grow in complexity, these dependencies can become more complicated. Inventor utilizes project files to locate the required files as they are needed. As a result of using the information contained in the project file, when you open that 3D assembly, Inventor can locate the 3D part files and display them properly.
In the context of an introduction to Autodesk Inventor, all that is important to realize is that you must have an active project before you create any files. This is why the project file is listed in the New and Open dialog boxes. Inventor installs several sample project files, but the default project is initially active. Depending on your particular usage of Inventor, it may be pertinent only to have one project or you could have many based on your file system and design needs.
Part Files (.ipt)
This environment is where all part modeling, sketching, and complex design takes place on individual components. Specific tools exist here for sheet metal, plastics, electrical connectors, complex surfacing, editing non-native parts, and more. Several styles of part modeling techniques are used here depending on company guidelines for required output and 3D modeling standards.
Parts are traditionally started with a sketch and then features are created from those sketches (extrusions, revolves, sweeps, lofts, coils, and so on), but geometry can also be added from selecting already placed geometry (holes, fillets, drafts, chamfers, and so on).
Assembly Files (.iam)
Parts are added to assemblies to position and constrain together to form the completed design. Parts are not copied into the assembly when placed (50, 1MB part files do not make a 50MB assembly file); instead, their relative location is hyperlinked into the assembly for referencing.
Part modification can still be accomplished inside the assembly to visualize how the change will affect other components when modified. When you make a change to a part, the change is evident in each assembly or drawing that references that part. Assembly files can be referenced by other assembly files (creating subassemblies), presentation files, and drawing files.
Presentation Files (.ipn)
This file type is used for two purposes. First and foremost, it is used to create explosions that will be used for disassembled views in drawings for easy documentation. Second, it is used for animation tasks for quick visualization of assembly or movement for internal review to different stakeholders. Inventor has a rendering Studio environment and the Design Suites have Showcase and 3Ds Max for more intricate stills or animations.
Drawing Files (.dwg or .idw)
This file type is responsible for creating orthographic views and annotations for designs. IDW and DWG files are also interchangeable. Depending on your workflow and need for use in downstream applications, you can create your production drawings with either file format, but DWG allows more collaborative and functional uses.
As changes are made to parts, assemblies, and presentation files, their updates will update other files in which they are referenced—whether that it is just a drawing file or numerous other assemblies or subassemblies. For instance if a part is used in 50 different assemblies, a change made to that part will update how it appears in 50 different assembly files simply by changing it in the part file.
As some of these relationships get more advanced or more components are reused, data management software such as Autodesk® Vault (free with Inventor) becomes important to design to aid in managing relationships and associations of files to each other. Tools that copy entire designs and sever links to the original files are extremely valuable for iterative designs that you don’t want tied to an original file from another job. Data management systems can resolve links that reside within modeling files to new path locations and file names without manually relinking files to their correct references.
History-Based Feature Modeling
Inventor is a feature-based modeling program, which means that a part evolves by creating features one by one until the design is complete. To start a design, there are several base features to choose from. Below is an example of four, but there are more.
There are primarily two types of features you can create with Inventor’s modeling environment, those which require 2D profiles to create (Sketched Features) and those that require only existing geometry (Pick and Place).
Sketched Features are created by sketching its shape or profile and can be any shape or size. To create a sketched feature, you must sketch a 2D cross section on the placement surface or plane and add dimensions and constraints to define and locate the sketched geometry with respect to the model.
Pick and Place features are those for which a shape has been predefined. To create a pick and place feature you must define the location of the feature and the references required to locate it with respect to existing geometry. Examples of some pick and place features are fillets, drafts, chamfers, shell, and some holes.
The history of these features—whether they are sketched or pick and place—is stored in the model browser of the modeling file. Consider the following set of features and their order.
From this model the tree on the right is automatically created for this history. Modifications can be made to the earlier features to affect changes to the latter features in the history. Any change to Extrusion 1 will affect change to the entire part, because it is the Base feature, as well as positioning of latter features, depending on how they were created.
The same power that grants this highly functional type of design can also be a pitfall for new users. For instance, what if one of the features were deleted? What would happen to the above model if the Shell in step 4 or Extrusion in step 5 were deleted from the history? Anything dependent upon those features such as steps 6 through 9 would either become sick or destroyed.
These types of relationships that are created by referencing already created geometry or features is known as Parent-Child relationships. For Example, Hole1 is parent to Mirror1. Modification of Hole1 directly affects Mirror1, but modification of Fillet2 does not directly affect Hole1 or Mirror1 since it was not referenced for either subsequent feature.
The majority of the features you create on your parametric part models start with constrained 2D sketches. Intelligent and predictable part designs require a thorough understanding of how to create 2D sketches and how to capture design intent by applying geometric and dimensional constraints. Precise sketches created with AutoCAD, by default have no parametric intelligence. A change in a dimension does not force the geometry to update to reflect the new dimension value.
Parametric sketches in Inventor enable you to click and drag the geometry in directions allowed by the existing constraints while all conditions controlled by the constraints are maintained. For example, if you drag the outer arc to a different size, the horizontal lines remain tangent, horizontal, and their defined length. This is called flexing the degrees of freedom of a sketch.
A parametric sketch consists of 2D geometry on which constraints are applied to control the size and potential behavior of the 2D geometry. The two types of constraints are geometric constraints and dimensional constraints. As you create geometry in Autodesk Inventor, some geometric constraints are applied automatically.
The symbols next to the geometry in the above illustrations are known as "constraint glyphs" and represent 2D constraints. The use of 2D constraints is one way in which design intent is automatically captured as you are creating your sketch geometry.
Dimensional constraints, on the other hand, control the size of the objects. The diameter dimension controls the size of the circle, while the linear dimension controls the length of the horizontal line. There is only one command to create many different types of dimensions based on the user selection. Dimensions will control the size of the geometry; the geometry does not control the value of the dimension.
Dimensional constraints used later in design on secondary features really show off the ability to change values to have features move based on the intent of the user.
As Dimensional constraints and inputted values are added to a model, their values are stored in the Parameters box for equations and management. Unique identifiers are given to each dimension used in sketches or feature creation (d0, d1, d2, etc). These values can be renamed and formed into equations for which to drive design variation and relationships in modeling files. Modification of the values here can also change the model directly.
Models built in part mode can be used as components in an assembly file. Assemblies are created by constraining components with respect to one another. The addition of constraints creates feature relationships between components and builds intelligent assemblies. Similar to features in part mode, constraints in assembly mode are assigned a unique identification value for their offset values (d0, d1, d2, etc) to be used in equations if desired.
Initially when a part or subassembly is added to a new assembly file, the first component placement will be grounded in place and will not move around.
Components added after the first one will have six degrees of freedom (DOF) of movement (three translational, three rotational). In order to restrict that movement, assembly constraints are used to lock down any undesired movement. Either Constrain or Assemble can be used to create assembly constraints.
Examine the example below with the base component (letters) and the secondary component (numbers).
Open degrees of freedom will allow users to check desired motion in designs before locking them down. In the example below, the yellow linkage piece is too short to allow the red link to go a full 360 degrees (1 and 2). But activating the part in the assembly and changing the length of the yellow link to allow for full rotation can be done without ever leaving the assembly (3).
Once components are assembled they can also be checked for interference in design. In the following figure, the red shows a PCB board (green) overlapping into the plastic walls of this part. Corrective measures for design flaws can be taken care of before parts every hit the mold or the physical prototype stage. In traditional 2D drafting these types of interferences could be very hard to see and often times missed before a prototype is created.
The Automatic Bills of Material tracking for designs makes sure all components are accounted for and that the design criteria for each part is being correctly populated for data tracking. If not, changes can be made here to enact change to the part files material selection, BOM structure, and other tracking data known as iProperties.
Autodesk Inventor has numerous tools for showcasing designs. While it is true that some of the ancillary products in the Design Suites as well as other products such as Inventor Publisher do a much better job for direct marketing of consumer data, the Inventor tools are quite useful for internal company discussion and training. For instance, Drive Constraint in assemblies and standalone presentation files are great for showcasing movement, while Inventor’s realistic visual styles and material library with Studio are great for higher end work.
Drive Constraint or Presentation (*.ipn) files can be used to create videos (AVI or WMV) of what is on the screen. Drive Constraint will capture offset values as they change and animations in the presentation environment (*.ipn) will capture steps to assemble or disassemble a design. The videos can be shared internally for discussion or externally for clarification of design intent in the supply chain.
When it comes to higher quality visualization, Inventor has a few tools that have performed quite well in the past: Inventor Studio for high-quality, photorealistic stills and animations as well as fanciful technical sketches, and the Realistic Color Styles and Environments (IBL) for faster still imagery. Both of these images are taken from the Inventor interface.
The tools available in the drawing environment enable you to quickly create production-ready drawings for manufacturing. Drawings are created from part, assembly, and presentation models. The shape, dimensions, and orientation of the parts or assemblies have already been defined in the part or assembly mode. Inventor uses this information to create the required views in a drawing file very quickly without the need for manual orthographic projection techniques.
Drawing models are not actually self-contained in a drawing file. There is a link between the drawing file and the source model. If a change is made to the source model, all drawing views that reference it automatically update. The reverse is also true—a change made to a modeling dimension in the drawing also reflects change in the model.
Adding details and annotations to your drawings enables you to communicate additional information to other designers working on a project. You can also apply styles and standards to control the appearance of your model and drawing annotations.