Inventor 2009
Published Thu 5 Jun 2008
Autodesk is upgrading its flagship Manufacturing product, Inventor. Al Dean takes a look at what’s new and what it can do for you.
Image Courtesy of HTC Sweden AB
Inventor is Autodesk’s Manufacturing Solution Division’s flagship product. Its release saw the move away from an AutoCAD-based 3D design system (Mechanical Desktop) and the system has grown dramatically in both user numbers and functionality in the years since its launch. At present, Inventor covers the whole gamut of 3D modelling techniques, from part and assembly design to drawing production. In the past few years, this has expanded to include tube and pipe, cable and harness design, sheet metal, surface modelling and, most recently, design accelerators and simulation tools through various acquisitions.
Alongside the development of the product, Autodesk has developed its Digital Prototyping concept, where Inventor is used to take products through to manufacture, testing the product virtually before committing to a prototype. Autodesk is making a big noise with Inventor these days and this message about Digital Prototyping is gaining some traction and many are benefitting from its implementation. The concept of using technology to develop your products more quickly, more intelligently and more efficiently makes perfect sense – and the good news is that each release brings the user community closer to being able to achieve this in a meaningful manner.
So what does the 2009 release mean for users and organisations that have based their working practices on the product? A great place to start is with user interaction and productivity. Sources tell us that Autodesk is currently working through a project which sees the user interface and working practices standardised across a hugely disparate number of systems, not just AutoCAD and Inventor, but also Revit, 3ds Max et al.
Highlights of the new version of Inventor range from new tools to assist every user in navigating their 3D world with more intuition than keyboard gymnastics, through the updates made to the sketching tools which make the process more fluid as data is presented in a more logical and consolidated manner.
The sheet metal modelling capabilities have been overhauled, with both new sheet features added as well as intelligence which links together various processes. With the rise of outsourcing, the ability to accurately communicate your requirements and design intent is invaluable to any business.
The updates made to the assembly-modelling environment mean that users can make their use of the system more efficient with the introduction of Substitute assemblies and updates made to the automatic component placement. Interestingly, the Substitute assemblies technology also provides you with tools to protect your Intellectual property when dealing with suppliers.
For me, many of the highlights for this release are actually under the hood items; the less obvious linking of separate workflows which makes the system really work at its optimum and from that, users can gain an advantage. This can be seen in specific features like the linking of punch features in sheet metal to drawings. Manufacturing information is defined and available in those 3D features, so why not just display it in drawing views and save some time recreating it? Taking Sheet metal further, the ability to create a more accurate and manufacturable sheet metal product means the Design to Production process is more efficient with the potential to remove the real world bottleneck of manual preparation work on the shop floor.
The consolidation of various libraries in Frame design and sheet metal into the Content Center also makes a lot of sense and will provide real benefits – not only in terms of management of data (as it’s all in one, sharable place), but also that it makes standardisation easier to deploy. By ensuring that your design team is working with validated forms - forms that can be built and manufactured cost effectively - you’re giving your organisation huge benefits in terms of reduction of costs of manufacture but also rework throughout the process.
Increasing design productivity
The new Degrees of Freedom display gives you a visual view of the degrees of freedom available in the selected elements. If you’re looking to test out the parameters of a sketch, see where your sketch is under defined/constrained or if you’re working on a 2D mechanism concept, then it’s invaluable.
In terms of feature creation, sketching is something that’s always being improved - if you can make this core function more efficient, then the rest of the process benefits. Inventor 2008 introduced improved constraints management and this has continued in this release with constraints display more rationalised, more contextual and more clear. For example, coincident constraint is now displayed on the points of intersection, rather than on the geometry. Constraints are more persistent than before and many are now automatically applied. Their creation is based on your mouse movements and the manner in which you construct your sketch geometry. Essentially, the whole process is much more intuitive than before and involves less manual constraints assignment, so you spend less time fiddling with geometric relationships and more time designing.
Also related to constraints management is the new Degrees of Freedom display, available through the right click menu. This gives you a visual view of the degrees of freedom available in the selected elements. If you’re looking to test out the parameters of a sketch, see where your sketch is under defined/constrained, or if you’re working on a 2D mechanism concept, then it’s going to be invaluable.
There are a couple of other sketching-related updates worthy of note. Text can now run along an arc, which for those working on etched or stamped forms, will be a godsend. You can also run a spline through a series of points imported from a text file of co-ordinates and explore alternate solutions to trim or extend operations before applying them.
Sheet metal
Sheet metal has seen a big boost for this release. The big ‘under the hood’ change is that Sheet Metal properties are now integrated into the Standards and Styles Editor dialog. You can standardise sheet metal parts based on the same library of options, standards and parameters that are common across the rest of Inventor. Factors such as sheet thickness and gauges, K-factors, bend radii and bend tables are incorporated into that central resource and are more manageable - as you have a single location and dialog for entry and editing.
Sheet Metal is divided into two areas – Sheet Metal Rules and Sheet Metal Unfold Rules. Sheet Metal Rules are used to define the bend and corner relief options that govern the design and behaviour (in terms of manufacturing and production) of sheet metal parts. Sheet Metal Unfold rules capture your standard unfolding methods and can be built using both linear and bend table based unfolding methods.
The new Multiple Insert option in the AutoDrop command now allows users to add instances of components into matching holes wherever they are found on planar surfaces. To add additional hole sets this just requires a quick selection, which saves a lot of manual work. The system can also automatically align inserted components in the same way.
For those actively using the existing tools, much of this information already exists and Inventor allows you to import, inspect and formalise bend tables from existing design work, then store them as best practice within the Styles and Standards Editor (they can also be exported text files if you’re maintaining older versions of the system). In terms of end use, this means that you can standardise your sheet metal design processes and maintain them across your design department, so your design team uses the same reference points, standard values and best practices, so design error can be reduced by ensuring that pre-validated parts are designed with your own manufacturing constraints and capabilities.
Moving onto more Sheet Metal modelling-related updates, this release focuses on a core area of sheet metal design – corner handling. While the ability to create a developable form has been within Inventor for years, there is always work to be done on ensuring that manufacturing processes are fully supported and that your model truly reflects your production intent. An interesting example is the ability to override how corner seams are built. The new UI methods are ’heads up’, with glyphs placed at each corner of the model which afford you precise control over how mitres are constructed. There is direct control over support overlap type, gap value, and overlap percentage in 3D and these are then reflected accurately in the flat pattern. What’s also key is that these adaptations of the default settings do not bloat out your feature tree and are maintained as a single feature or a much reduced feature set, whereas previously each would be a separate feature.
Elsewhere in Sheet Metal you now have greater control over the creation of corner seams, with the ability to precisely define and maintain the gap between them according to your welding process requirements. This release also sees the addition of large radius bend support which will be particularly useful for those working with Sheet Metal casings. What these features are all about is the creation of a clean flat pattern which goes into the production process with a greatly reduced requirement for welding prep.
Sheet metal intelligence
Working with Sheet Metal is an interesting process. It was once considered something of a black art, with drawings provided to the shop floor and the end result would just appear by magic. What the introduction and adoption of 3D tools has meant is that the designer is much more responsible for the forms that are supplied – and with the rise of outsourcing, this is never more critical. If you want parts produced accurately, you need to ensure that the data you provide to your supplier is as accurate and as unambiguous as possible. Also, what’s key is that you standardise your design work – and a way of doing that is to use standard features.
While Inventor has an increasingly rich standard punches forms library, another route is to use iPart technology and standard fasteners where appropriate – both of which have been addressed in the 2009 release.
Substitute Parts workflow
Click the thumbnail to view the images. You can navigate through the workflow steps by clicking on the left and right sides of the expanded image or by using the arrow keys.
Firstly, the system now supports PEM fasteners or, for the brand adverse, self-clinching and captive fasteners or threaded inserts. They are implemented as an extension to the Content Centre libraries and the Design Accelerator tools (Bolted Connections). Moving onto iPart support, you can create families of Sheet Metal parts with Sheet Metal-specific properties and can reference the Sheet Metal Rules and Unfold Rules we’ve already discussed, allowing you to create standard parts that support different manufacturing capabilities, whether that’s by material, by machine tool on your shop floor, or by supplier.
Frame generator
Considering that one of the biggest Inventor user groups is Custom Machinery, the introduction of Frame Generator was like manna from heaven. The good news is that this release sees some of the limitations of the tool removed and the construction of framework around existing geometry is now much more flexible. Before we onto the nitty gritty, it’s worth noting that Frame Generator is now fully integrated into the Content Centre, so you have a single, sharable source for all beam sections (more on those shortly). Frame Generator also now supports user defined section profiles and Unifast standard parts.
Moving on, for those working regularly with this type of form, you can now use more than just 2D sketches as the generating form for a framework. Elements can be multi-selected, so you can pick out a group of entities which define the framework and have the system create all those parts in a single step.
Finally for Framework design, if you’re looking to publish custom profiles and sections to the Content Center based library this is done using the Frame Shape Authoring app. This makes the process much easier, by prompting you for all the information you need to prepare a custom profile.
Assemblies
The biggest update for Assembly modelling is the introduction of substitute parts. These are used when you need to maintain the geometry of a group of parts or a sub-assembly but don’t want the full description in terms of details, geometry, or features. The first use case that springs to mind is purely performance related. If you can represent an assembly accurately with less data, then your workstation will have less to do and will run faster.
It’s also useful for protecting your intellectual property by enabling you to hide details, yet allowing you to send usable data to a supplier or customer. Then of course, there’s simply the fact that you might not want to load every single detail and this gives you a very efficient manner of combining performance with vital information.
Navigating the 3D world
While many users are now comfortable with working in 3D, the truth is that there’s always more that can be done to make view manipulation more efficient. Inventor 2009 sees the introduction of new tools for interacting with your 3D environment and these are encapsulated in the View Cube and the Steering Wheel.
The View Cube is a small graphic at the top right of the screen. It allows you to select a variety of standard views and rotate them with ease, by simply selecting your chosen view on the cube. In addition to the named faces, you can click corners and edges to get the exact presentation of the model you need. If you want to rotate the model, then the arrows appear to the top right of the curve and will rotate the model 90 degrees at a time. There’s also a Home view icon that takes you back to an isometric view by default.
The Steering Wheel is another interesting UI widget. Accessed either through the icon at the top of the screen (or CTRL+W) it pops up and presents you with a ‘heads up and at cursor’ way of interacting with your 3D model and works in several ways. One is the Object mode, where you can rotate, pan and zoom ‘around’ an object. The other is the walkthrough, which allows you to walk into your model.
The Steering Wheel also incorporates a small command with huge productivity benefits and this is called Rewind. It brings up a series of thumbnails of all the views you’ve used recently. As you slide between them, the view updates, and once you find the view you want you let go of the mouse button and the model stays in that view. It’s very productive and if you’re switching between views regularly (as most users do) then it’s going to save a lot of time. The drawbacks are that it doesn’t store component visibility details and there isn’t a hotkey to just activate this alone without the whole Steering Wheel.
Substitute parts are implemented within the Level of Detail (or LOD) tools. There are two ways in which you can use a simplified part to hide details. The reduced memory mode allows you to select an assembly to derive into a single ‘lump’ or you can use a Derived Assembly to create a more geometrically accurate representation.
There’s also been some work to assist with the placement of components, to either automate the process more, or to add more intelligence. Good examples are the new tools to assist with placing multiple components quickly and intelligently. The AutoDrop (Multiple Insert) option will place multiple bolts or screws wherever matching diameters are found and this is backed up with similar options based on iMates– both saving a potentially vast amount of time. Taking things further, the Place Component Orientation option will reference the last instance of a component within the assembly browser and reuse the same orientation. Finally, if you’re looking for a less formalised way of positioning assembly components, the new GripSnap tools allow you to do just that. These enable you to grab a component, along with all the reference geometry (work planes etc) and use precise tools to move and rotate them.
Drawings
The final major subject area we’re going to cover in this review is Drawings, an essential part of the Product Development workflow. So what’s new and updated? The answer is that there’s been a concentration on adding real meat to the draughting tools already within the system. By this, I mean providing the user with the ability to create the type of drawing view and GD and T they require and still maintain that associative link back to the 3D master model.
For example, it’s standard draughting practice to crop unwanted portions of symmetrical parts, so the new Crop View tool allows you to define how a part is cropped using rectangular, circular, and polygonal crop windows without having to use the breakout options as you would in 2008. In terms of Annotation, the benefit of working with an intelligent system like Inventor is that the drawing environment can extract information from the 3D model. 2009 sees the ability to extract centrelines (for holes, fillets, revolves, and bends), and centres of gravity. You can now have the system automatically create interference edges (by setting the Display Interference option in the View dialog) where two parts intersect, rather than having to draw them in manually.
Another interesting update is the ability to filter the parts list in Bills of Materials. Rather than having to list every part extracted from a drawing view, this allows you to filter out those components which do not need to be documented in that particular drawing – for the sake of clarity. Some filters are preset, such as Ballooned Items, Standard Content, Item Number Ranges and Purchased items. However, you can add your own filters to adapt your tabular data to your needs and have that remain associative when the assembly file updates.
On the Sheet Metal specific side of things, drawings can now include Punch notes from standard forms. This extracts the manufacturing information, such as Punch ID, Direction, Angle and Depth from the 3D punch feature, then populates your drawing automatically – saving you a lot of additional work (and just as a tip, you can also include the <QTYNOTE> token in those notes to display a count of matching punches).
