Inventor Fusion technology preview: Part two

Written by Al Dean

Published Mon 29 Jun 2009

Part 2 - existing geometry, assemblies and annotation

While the tools we've discussed so far predominantly focus on the creation of geometry from scratch, one of the reasons that there's been a groundswell of interest in direct modelling technologies is the inherent ability to work with existing geometry. The reason this is attracting such interest is that with history-based design tools there's a big issue of history recalculation and knowledge. History-based design relies on a linear recipe of features, built on top of features, on top of even more features. Editing that geometry can be painful, mainly because editing early features can can have a big knock on effect causing subsequent features to break.

Alongside this purely technical hurdle,there's also an issue of knowledge. Because you have a very granular and lengthy recipe for even the simplest of parts, making edits and reconfiguring geometry to make a design change, requires some serious knowledge - not only of the system in question but also of how the component was designed in the first place. It's bad enough diving into a complex part you have designed yourself, but editing someone else's work can be the stuff of nightmares.

Importing data

In its current incarnation, Inventor Fusion allows users to read the native Inventor and AutoCAD format data directly - note that the system will only import solid geometry (not wires, surfaces or points). It's also worth pointing out that when importing Inventor data the system will not work with assembly features (typically used for weldment design). In terms of third party data, Fusion supports the import of SAT files (between version 4.0 and 7.0) and STEP files (supporting the AP214 and AP203E formats). In terms of export, it will save out to the Inventor format but the other formats are limited to SAT (7.0 only) and STEP using the AP203E standard.

Feature recognition

As we discussed in Part one, Inventor Fusion is a non-history-based application but still takes advantage of feature-based working methods. When creating specific native features (holes and fillets in this technology preview), these are stored and remain editable. But what about imported data which typically won't have this feature data? To get over this and to add some intelligence to the system, Inventor Fusion has basic feature recognition tools built into it. Once your geometry is imported, the Recognize Features tool can be run from the Home panel. This will interrogate selected geometry (it only works with one part at a time) and will find any hole, fillet or pattern features and store them in a browser.

It should be noted that with imported data this doesn't replicate the features used to build that part originally, but rather uses recognition technology to find features that Fusion can work with. The same is true of Inventor parts too. As you'll see from the pictures that accompany this article, the system doesn't replicate the traditional Inventor feature tree, instead using a series of mirror patterns, holes and fillets to recreate the cycle fork crown part.

The Fork Crown part (from the suspension fork dataset in the Samples folder). This has a multi-item feature and history tree detailing each operation used to build the part.

Importing the same component into Inventor Fusion give you a dumb solid which you can edit. The Recognize Features command will interrogate the part and find features that Inventor Fusion can replicate, such as fillets, holes and patterns.

Making edits 

When it comes to making changes to parts I've found it's best to work with the data directly using a combination of the Press/Pull and Move commands to edit the geometry, shift it and work with it. When working with direct modelling tools such as this it is important to realise that all systems (without exception) have quite specific limitations in terms of topology. While you can move, push and pull faces seemingly at will, the model must remain watertight and closed and the geometry/topology must solve. When you see faces disappearing, this is usually in the area of fillets and such, where the underlying modelling engine can't handle the removal of those faces to patch the surfaces back. If you try to make too drastic changes to complex geometry, perhaps to move features across faces and boundaries (particularly when those faces are non-planar), you'll run into trouble and the operation will fail. The good news is that Fusion gives you good feedback about what it can and can't do and will clearly flag up problems.

Working with Assemblies

The Constrain panel gives access to assemble both parts and multiple bodies within a single part file.

Alongside the part modelling and editing tools, Fusion also allows users to create assemblies using some basic mating tools. As the system is capable of handling multi-body in a single part users can work with both explicit separate parts or use the same alignment and mating tools to build up an assembly using mulitiple bodies. The basic commands are found when clicking the Constrain icon in the Home panel and these are Align, Center, Angle and Tangent, all with offsets where appropriate. One thing to note is that the order in which the mating geometry is selected is important. As Fusion doesn't have a Fix or Anchor command to lock the first part down, your first selection is automatically locked and the second selection moves to it.

The Anchor glyph denotes that the first selection is locked and your next selection will move to it.

Annotating data

While the name of the game with Fusion is direct editing of geometry, there are also a range of dimensioning tools, either for creating precise geometry or for annotating models. For the former, the system allows users to create dimensions to position geometry precisely using traditional modelling methods. When it comes to annotation of a model the system follows the new 3D annotation methods that are being introduced across the industry.

 
Dimensions are added directly to the model (rather that to a drawing) and users have the ability to add dimensions to specific work-planes. These can be specified directly or dynamically. As there could be a complex set of annotations users can switch between existing annotation planes (using the tab key) which helps keep order in their dimensioning schemes. Users can also toggle between ANSI and ISO methods of dimensioning in this technology preview.

Next up we're going to speak with Kevin Schneider at Autodesk about the launch of Inventor Fusion, to find out what Autodesk's plans are and where all of this new technology is headed.