Articles tagged with Inventor Fusion

Finally got around my subscriptions update with Inventor 2010 (you need both SP1 and the Subs pack), so I’ve spent most of the day playing with Fusion Tech Preview 2.0 which was announced earlier this week and made live at the same time. What I’ve found has intrigued me, but before we get onto that, lets look at what we’re dealing with.

Fusion is about two things, in no particular order, other than it makes sense in terms of our focus. Fusion TP2 bring some changes and refinements to the user interface, which Autodesk is testing out with this project, so see what people like, what they don’t and what sticks. Some of the changes for this update include a rework of the geometry selection tools (the feature recognition for selection is still a bit flakey), but for me the work done on the triad to make aligning it to other geometry (there’s a small glyph you hit to then align the triad) makes the whole direct editing thing work, as you would expect.

While these are interesting, the big news is the introduction of the Change Management add-in for Inventor. Essentially, this enables the round tripping of data between Fusion and Inventor. You have an Inventor part, you want to edit it in Fusion, load it, edit it, directly, without recourse to geometry History. You save it. Load it back into Inventor and rationalise the changes to update the history and feature tree. It tracks what you’ve edited, what you’ve added and what you’ve deleted and updates the history and feature data accordingly.

This is the background to the Fusion name. Autodesk are attempting to fuse the ability to use both Direct Modelling in combination with History based modelling tools. The eventual goal, at present according to the powers that be, is not two separate applications, but to prove out the technology and integrate it all into core Inventor, rather than providing it as a standalone application. Hence, it’s Technology Preview, not a Product Preview.

So, let’s have a look and see what we can do.

1. Let’s start with a simple part. One of Inventor’s sample parts. As you’ll not particularly complex. The Feature tree shows a free extrudes, a few holes and that’s about it. Easy meat for Fusion to Edit.

2. Loaded up into Inventor Fusion, we started by removing this hole feature. Easy job, as you simply select the faces you want to take out, the system removes them and removes the internal boundaries of the faces and closes the surfaces out.

3. Once that counter bored hole is gone, I shifted the remaining hole along the edge and back into the part a little.

4. Next I grabbed this feature, all in all, 8 faces and shifted it a few mill up the face. The new Triad orientation thing works very nicely indeed.

5. Final move was to take these two other holes, use the Press/Pull comment to make them both 2mm larger by offsetting the internal faces. Not an accurate way to redesign a hole, but for this purpose, it’ll do.

There you have it. Four things have changed. Two things have moved in position, one has been deleted and two have been resized. It took a couple of minutes at most to effect these changes. So let’s see what happens when you read it back into Inventor Professional.

When you read the part into Inventor, the Change Management add-on kicks into gear and inspects the part you’re loading. What’s interesting is that because I was using .ipt files and Fusion saves out .dwg files, I was actually not loading the original file back into Inventor. Obviously Fusion, when making edits, stores the original feature information somewhere and the new edits alongside it. So what happens?

6. The Change Management add-on presents you with a list of edits made to the model and shows you graphically on screen on where those changes occur. It shows you the changes in blue/yellow slowing before/after for geometry changes and red showing deletes. In the image above you can clearly see the four edits we made.

You have the ability to control exactly what happens with each detected change. You can have them executed, so the feature gets rebuilt, you can ignore it, or if you encounter problems, then you can choose to have the faces extracted and the system try to patch them back into the model with the Sculpt command.

Thinking this was a reletively simple set of changes, I hit the Apply All.

It broke. and while it rebuilt one feature out of those three changes, very little else worked.

I was surprised so I did some digging.

What it boils down to is that because of the nature of whatever Autodesk is doing with Fusion and the edits it makes, there are at present, very explicit limitations in terms of what can and can’t be done when you’re moving data between Fusion and Inventor and hoping to have the history and feature tree reconciled and maintained.

Your features have to be features in their own right. There can be very little interdependency between features, no patterns, no mirrors, no nothing. If you try to edit a child of a pattern, you get an error. If you try to edit the parent, you have problems with updates. I looked into this simple part we have here.

If you look a the history tree, you’ll find it’s all driven by patterns and there are three core features that are repeated throughout the part. I’ve coloured coded them above and below - the grey is the base extrude, the green features are the parents, the red features are the children. Below shows what happened when I just edited the parents. Because patterns are based on linear references, you find that the pattern tries to update too and that breaks the history tree.

Now. I don’t want you to think I got the hump, threw the toys out the pram and proclaimed “this fusion stuff doesn’t work”. I didn’t. I tried out some more parts, built some myself, tried them out and found that there are instances where the Change Management tools actually work and work well.

But these are very simple operations in very rare conditions where the feature has almost no effect or influence on other parts of your geometry. For anything else, if you want to, purely for technical reasons, try to get this to work and with this first release (that’s key to note - this is a first public showing of a new technology - NOT a product), then you have to understand exactly how your changes will effect your history tree if you want to try and reconcile even the simplest of changes.

This struck me as odd. Part of the pitch for direct modelling is that its easier to use when you either aren’t aware of how a part’s been built, have forgotten or that make a simple change you need to make is going to royally mess with your history-based part. The irony is that if you do use a technology like Fusion and unless Autodesk pull something out of the bag in terms of improving this Change Management technology, you’re going to have to be just as familiar with your part’s build history, its method of construction and the effects a seemingly small edit will have - then you might as well just do it in core Inventor.

What should also be noted is that this doesn’t change Fusion’s potential as a direct modelling technology. The user interface, although much the same, feels slicker, with a nice workflow and use model now developing and it’s power is there. The ability to open a part, make edits and get on with the job at hand, without worring about data source is a good and valid one for many - and Fusion executed all the operations I wanted to do perfectly. it seems more consistent and more robust and repeatable than the first Tech Preview - or maybe that’s just me.

But in the end, I can’t help but wonder where the Change Management technology is going and whether it’s actually worth the effort or indeed, even possible to get this to work in a reasonably functional manner. Kudos to Autodesk for trying to pull off what’s an incredibly complex thing. The good news is that this is all done, for free to the user, so they can see what it can do, try it out and feedback into the process. Autodesk Labs (as with all Labs sites) is all about trying things out. Some work and some don’t. Some make it to market, some don’t. Portions of some products get shipped while the rest gets scrapped. The good thing is that these days, we all get to try it out and see for ourselves.

Looking at the industry as a whole, there are many different approach and different ways that vendors are looking at the Direct Modelling world and this is just one avenue of experimentation. For those with an interest in how product modelling is moving forward, these are truly interesting times.

I got briefed about this last Friday (as did the rest of the press/blogger community I’m sure), but I wanted to wait till it was up and live on the Autodesk Labs web-site and I’d had a chance to play with it. When Autodesk publicly and officially announced Inventor Fusion Technology Preview, much was made of the name and the aims of the technology.

This is Autodesk’s answer to the likes of Synchronous Technology, Instant3D and all the other non-history-based modelling technologies out there. What the company has focused on, with both the messaging and the name, was the ability to rationalise together traditional feature+history-based model edits with the history-less modelling practices founds in Inventor Fusion.

Essentially you could edit a traditional Inventor model in Fusion, without using features of any kind, then pass it back to Inventor to rationalise the changes and update the history tree to integrate those changes back into the history-based model. This isn’t the history-tree appending method used by the likes of NX and SolidWorks, but something more integrated at the very core of your modelling history. The problem was, that capability wasn’t available in the first Technology Preview - which many missed. That changes today with the introduction of the Change Manager add-on for Inventor alongside Tech Preview 2.0.

Today, Tech Preview 2 has gone live and you can download it and play with it. Again, you have the ability to try Inventor Fusion if you’re from the qualifying countries. But you’ll need to be a suscriptions customer using Inventor 2010 Subscriptions release if you want to try the Change Manager. The two peices of code (fusion 2.0 and Change Manage) are delivered as separate zips/installs.

It’s also worth remember that separate applications are not the end goal of this process. This is a Technology Preview, and separating out the Fusion tech from core inventor, allows the team to play with and distribute the code and see how users like the interaction between the two different types of modeling methodology - but the end goal is that Fusion technology will be built directly into Inventor, not sold as a separate application.

We’ll be trying it out later on today, once we’ve updated Inventor to the latest release (without which the change manager won’t work). There are also some new additions and changes to the core Inventor Fusion tools as well, so stayed tuned for more. In the meantime, here’s some video fun for you.

#3: Looking at this initial Tech Preview, Inventor Fusion has some legs to it. Yes, there are things missing or that it doesn’t do in comparison to other direct modelling systems – in fact, the system is installed with a list of things it can’t do, so if you have problems, check that first (it’s in the README_INV_FUSION.htm file).

But perhaps the real thing to consider is in the title, the word Preview. After all, this is a formative release of a new technology. So, to get an idea of where this is headed, I got on the phone to Kevin Schneider who heads up the Emerging Products and Technology Group at Autodesk, the man heading things up and pushing the system forward.

Al Dean: For me, the big question is the round tripping between Inventor and Fusion that you showed at launch. That’s not in this release is it and have you got any idea when it’ll be available?

Kevin Schneider: That is not in technology preview 1. We intend to let customers look that later this summer in an update to the Technology Preview. Not in the first Tech Preview but making it clear that we’re going to keep refining the ideas over the year, with customer feedback. As a result, the round trip with Inventor is not in this preview but we will get a chance to have customers try that soon. When we announced it, we should have been a little clearer that this wasn’t going to be there in the first release.

AD: How many releases are you looking at? Is there a specific lifetime you have for this thing on labs or are you looking at when it might ship?

KS: The technology preview you’re working with will go on to the end of the year. I can’t predict future releases or much about that but what I can specifically say is that we’re going to continue to update the Technology Preview releases as frequently as soon as we can implement ideas that come from customers. As to when it ships, that’s a bit more of a complicated question. Just like we did with Plastic Parts and the Advanced Simulation preview, ultimately the destination for these capabilities is core Inventor. What I would say is that customers need to tell us when they think what we’re previewing is ready and then we’ll move it to Inventor. That’s the whole point of doing a technology preview.

AD: It’s never going to a standalone application as it is at the minute, it’s always going to be an integral part of Inventor?

KS: I think the most wide reaching impact of the technology you see here will be when it goes into core Inventor. Whether the tool you’re using has a future – we have no comment or no commitment at this time. I think you’ll agree that if this capability was in Inventor, that would be big. Really Big.

I think the thing that’s important but is sometimes a little confusing, is the reason that we do these Technology Previews as a separate application is that customers are very reluctant to use Beta software because they have to uninstall production software, the data doesn’t migrate, they accidentally overwrite production files – all these things can be really dangerous in a production environment.

But by doing these as separate executables, you can side-by-side install, you can install it at home. We’ve found a much larger number of customers are using these things when we take the risk away from production software and we get way more feedback earlier in our ideas. It’s better for our customers, better for us, better for the industry.

AD: The one thing I’ve been thinking about is that you guys use your Labs web-site and resource a lot more than many other vendors. It’s a nice thing that you put these things out and you seem to engage with your users a lot more. is that something you’ve thought about? I’m curious about the mix up, when you’re developing something new like Fusion, do the customers that use it throw you things you didn’t expect or do you have a good idea where things are headed?

KS: I can give you some examples. We thought that some of the progressive shelling we’d done (Editor’s Note: this is found in the Plastic Part design tools) and as you know, work I’ve been doing for years. When we went to the technology preview and we got customers working with it everyday, we learned a lot and a lot of it about being not as easy to use as the benchmark we have set with Inventor. And that’s why it didn’t show up until Inventor 2010, because we needed to do more work.

In the past, that would have gone into Beta, people would have looked at it and it would have shown up in the release and users would look at it and think “What the heck is this?” – it would have been another hacked piece of functionality that customers get annoyed with. We’ve eliminated that problem by using Labs get quick feedback.

To specifically answer your question, there was a quite lengthy discussion at the last Paris press event between Roopinder, Martyn and a couple of others about how Autodesk doesn’t do enough to preview new technology, engage customers more early. “To lead” was the challenge they were giving us. Now the group I work, emerging products and technology, was a direct response to that can Autodesk do to use Labs better than any other company we’ve seen so far to get ideas and technology into customer’s hands early enough so we have solid ideas about how these need to go into our production tools.

First thoughts on the Technology Preview 1

I’m in two minds about what to write in the way of a conclusion. After all, this is very early stage software, nowhere near production ready. Autodesk has built a set of technologies (delivered as a standalone application) that’s clearly being used to knock the rough spots off the technology and usability before it gets anywhere near integration into core Inventor (which is the eventual goal). So let’s strip it back to basics and look at what Fusion represents.

The most immediate thing is that it brings a number of direct modelling tools that allow you to work with geometry in an effective manner, regardless of source. Yes, the tools available follow the conventions of other systems operating in the same, direct modelling manner and as a first pass at getting the technology out there, it’s clear there’s potential here. Great potential indeed. Direct modelling, despite what some vendors claim, is a technology that’s very nicely suited to specific tasks. Not in terms of industry or market sector, but pure, hardcore modelling operations where history-based systems fail. Whether that’s working with imported, dumb, data or whether that’s making design changes at late stages where the history of the part or assembly becomes unwieldy and prone to breakdown. It also provides an interesting way for the non-expert CAD user (but I’d stress the experienced engineer or designer) to get ideas down, play with geometry and to think, in true three dimensions and document those ideas and concepts – but without the knowledge overhead traditionally associated with history-based modelling techniques.

These have been the sweet spots for direct modelling for the last two decades and I suspect might always remain so. What’s changed is that there are larger vendors now jumping into the space that’s formerly been occupied by the likes of CoCreate, IronCAD. If you have bigger players discussing a technology, there’s a perception that something new has been discovered. Facts are that direct modelling isn’t a particularly new concept. What’s changed is market awareness, increased development resources across the industry and yes, more powerful hardware to enable those direct edits to be made with less chunking of a processor set.

But alongside the direct modelling, there’s something else afoot here and that’s an intriguing experiment or testing of waters with regards the Inventor user interface. Inventor often gets a bad name for itself amongst users moving to it from other modern systems (in all honesty, usually, SolidWorks), claiming it’s not as easy to use and my personal thoughts are that there’s one or two very fundamental sticking points that back it up – nothing major, but things that jar if you’re used to other systems. Looking at Fusion and separating the modelling technology from the user experience, it’s clear that Autodesk is testing out how users react to the new marking menu system, a much more interactive heads up way of working than is currently implemented in core, shipping Inventor. What I find intriguing is that Autodesk are doing this by release code into the public realm and letting users (whether they’re customers or not) play with it and see what it can do. That can’t do anything other than assist with making a better product.

So the two in combination makes for an interesting thing. Some new technology that’s at a very formative stage, still awaiting some of the core components (the round tripping) and which is going to extend well beyond this calendar year with updates and such, then Tech Preview 2. Let’s see where it goes.

If you fancy a play, then its there to have a go with. www.inventorfusion.com

#2: While the tools we’ve discussed are predominantly targeting 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 providing such interest is that with history-based design tools comes an issue of knowledge and recalculation as we’ve already discussed, but also of knowledge. History-based design relies on a linear of recipe of features, built on top of features, on top of even more features. Editing that geometry can be painful, purely for the lag that editing early features can cause and the inherent problems with subsequent features breaking.

Alongside this purely technical hurdle to effective editing, there’s also an issue with regarding knowledge. Because you have a very granular and lengthy recipe for even the simplest of parts, to make edits, to reconfigure geometry to make a design change requires some serious knowledge. Not only of the system in question and its eccentricities, but also of how it 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 – and bad ones at that.

Importing data

Inventor Fusion, at this release, allows you to read the native Inventor and AutoCAD format data directly – note that the system will only import solid geometry (not wires, surfaces or points in this release) – if you’re also working with non-English speaking colleagues, then you need to ensure there are no non-English characters in the file names. Also, when importing Inventor data, the system again will only import solid data (not surfaces) and also will not work with assembly features (typically used for weldment design). In terms of third party data, Fusion supports the importing of SAT files (between version 4.0 and 7.0) and STEP files (supporting the AP214 and AP203E formats). In terms of Export, it’ll 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’ve discussed already, Inventor Fusion is a non-history-based application but still takes advantage of feature-based working methods. When you create specific native features (such as holes, fillets in this release), these are stored and remain editable. But what about imported data which typically won’t have this feature date? To get over this and to add some intelligence to the system, Inventor Fusion has basic feature recognition tools built into it. Once you have your geometry imported, you can then run the Recognize Features from the Home panel. This will interrogate the geometry you have selected (it only works with one part at a time) and will find any hole, fillet or pattern features and store them in browser. It should be noted that when 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, 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). As you can see, it 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. Using the Recognize Features command will interogate 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 dive in and work with the data directly, using a combination of the Press/Pull and Move command to edit the geometry, shift it and work with it. When working with direct modelling tools such as this, it is important that you realise that all these 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 handle the removal of those faces and patch the surfaces back it. 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, as with many similar systems, Fusion gives you good feedback about what the system can do and will clearly flag up problems.

Working with Assemblies

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

Alongside the part modelling and editing tools, Fusion also allows you to create assemblies using some basic mating tools. As the system is multi-body in a single part capable, you can work with both explicit seperate parts or use the same alignment and mating tools to build up an assembly using mulitiple bodies. Found when clicking the Constrain icon in the Home panel, the basic commands are Align, Center, Angle and Tangent, all with offsets where appropriate. One thing to note is the order in which you select your mating geometry is key. As Fusion doesn’t have a fix or Anchor command to lock the first part down, you need to remember that 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 your data

Now, while the name of the Fusion game is direct editing of geometry, you do have a range of dimensioning tools, either for creating precise geometry or for annotating your model. In the former, the system allows you to create dimensions to position geometry exactly using the usual methods – but the system isn’t really geared up for that yet. 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 you 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, you can switch between existing annotation planes (using the tab key), which lets you keep order in your dimensioning schemes. You can also toggle between ANSI and ISO methods of dimensioning in this release.

Next up we’re going to have a little chat with Kevin Schneider at Autodesk about the launch of Inventor Fusion, what Autodesk’s plans are and where this is all headed. Look out for more later in the week.

Perhaps the most eagerly awaited bit of technology in the last few months has been Inventor Fusion. This is Autodesk’s first foray into the world of direct editing of 3D geometry, which has been one of the most talked about technologies of the past 12 months with products like Solid Edge with Synchronous Technology, SpaceClaim and CoCreate creating much of the buzz. Yesterday saw the application launch, so we thought we’d give you a guide to the functionality you’ll find on the web-site.

Unlike Inventor 2010, Inventor Fusion doesn’t rely on history. Features are still very much an intrinsic part of the application, but it doesn’t carry with it the headache of history recalculation when features are edited.

Autodesk first showed off Inventor Fusion at its annual user event, Autodesk University, in December 2008 and we got the scoop on DEVELOP3D.com with some rather shaky videos. Seven months on and the technology has just been made available for download from the Autodesk Labs web-site. Out of all the CAD vendors, Autodesk has one of the most impressive Labs sites and many technologies that started out in Autodesk Labs have been refined over the past couple of years and now form a key part of Inventor and its associated extensions, such as simulation and tooling. Inventor Fusion is likely to remain in Autodesk Labs for some time as each successive public release is put out for all to see, play with and give feedback to help drive its development.

I’ve been lucky enough to have access to the software for the past couple of weeks prior to it going live on the Labs site and have spent some time playing with the application. Over the next few days I’m going to share my experiences and conclusions of Inventor Fusion, kicking off with the minimal User Interface (UI).

The Inventor Fusion UI. Dynamic. Very.

User Interface

The Inventor Fusion UI is minimal to say the least and because it has a small set of commands (which actually do a lot more than might immediately be obvious) there are just two panels and tabs. Let’s look at the basics of view manipulation first.

The View tab and panel gives access to the view controls for view and display. Like Inventor 2010, there’s a View Cube at the top right of the UI, then the display toolbar below gives access to the rest of the view controls.

In terms of navigation, all of the controls for pan (middle mouse button or F2), zoom (scroll wheel or F3) and rotate (F4) are there, with the exception of the shift + middle mouse button combo for rotate (a little tip for Inventor 2010 users courtesy of Steve Bedder). There’s also control over the display of grids, shadows, View Cube, navigation bar, and browser. As in Inventor 2010, it is worth noting that there is a toggle for orthographic or perspective display, but I encountered some display issues when in perspective mode, so be warned (I’m told this is to be fixed very shortly indeed).

There is also a material definition and texturing control for parts, so the visual appearance can be set to help put models in context. The familiar browser – now integrated into the user interface, rather than as a separate panel – gives access to named views, origins, work geometry, annotation planes and a feature list (Note: no history).

The final command for this panel is the ShowMotion tool. This is new for Inventor-related products and it sees cross-pollination of technology from Autodesk’s Showcase product. Showcase excels at helping users quickly create presentations to show off product models, and allows view positions and display states to be captured and animated – think a 3D PowerPoint for design review and presentation.

ShowMotion enables users to create a shot for a view and add the animation details so it can be stored for reuse and presentations. Simply bring up the little panel in the UI, flick between views, and run simple animations. It’s very slick.

Modelling from scratch

There are several things you need to familiarise yourself with before digging into Fusion. Firstly, the user experience is much more dynamic than Inventor (and many other applications, for that matter) and there is much less reliance on toolbars and icons. While all of the modelling and editing operations are available on the Home toolbar, once you get the hang of things, you’ll find you don’t use this much. This is a heads up interface to the extreme.

Fusion Tip #1: Fusion defaults to Inches. If you want to switch units, look at the dimension indicator at the bottom right corner of the screen. Click Inches and select from a number of unit displays (mm, cm, ft, metres are supported). The rule to the left gives you control over snap distances for the Press/Pull, dynamic manipulation controls. You’ll also see the toggle icons for grid, snapping and ground shadows at the very bottom of the UI

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Much of Fusion is driven from marking menus, something that was introduced into the Alias products many years ago and which has been adopted by many modelling packages as a replacement for the context sensitive right hand mouse button menu. Fusion combines the two. To begin, hover your cursor in the middle of screen. Now, hit the RMB (Right mouse button). You’ll see a radial marking menu pop up and a more traditional menu. The radial commands give you access to the following:

The Marking Menu’s give you access to the most commonly used command around the cursor and a secondary, more comprehensive list of commands in the more traditional menu.

For modelling. To begin, select Draw. This brings up the usual plane selection triad and you can either select a working plane or one from the browser. Once that’s done, the view presents the plane normal to the screen, starts a sketch and switches on the grid if you’ve turned it on (either from the View Panel or from the small icon at the bottom right of the screen).

Inventor Fusion’s sketching tools dynamically add ad-hoc dimensions that allow you to eye-in values (the grid helps greatly) or to tap in values to lock length and angle.

Immediately the line, circle, arc drawing tool starts and you can create a sketch. Sketching within Fusion is pretty slick. Hit the start point, add the first line and immediately the dimensions are displayed, for length and angle. While you can eye these in, it’s much more powerful when tapping in known values. The tab key switches between the length and angle, and you can tap in one and eye in the other – or indeed, tap in both.

To create an arc, you drag from the end point of your last line and add the arc, again eyeing in or tapping values as you go. This process can be used to create a lot of geometry, but for more complex forms there is a pretty comprehensive range of additional sketching tools, including splines, circles, rectangles, filleting, other methods of arc construction and extending and trimming. These are available either from the Home Panel or the marking menus. To assist with geometry creation there is also the usual range of work-plane, axis and point tools to create references. These are simple to set-up and use the same dynamic movement and positioning tools as every other command.

Automatic closed loop profile detection gives you the ability to create geometry very quickly. Model glyphs give you access to operation options, such as direction of pull, and draft angle.

Once you have a closed profile (Note: Fusion only supports closed profiles at the moment for feature creation, as there’s no surfacing), you’ll find that the profile automatically becomes shaded indicating that it’s ready for feature construction. To exit the sketch, you can either hit the small icon at the bottom right of the sketch plane or hit the marking menu and choose the modelling operation. Now, this is where things get interesting so let’s look at the various commands available in this first Labs release.

The major modelling operation is the Press/Pull command, found in the marking menu or the panels. This can be used to create extrusions, either to add material or cut it away. Hit the command, select the profile you want to work with and the display brings up a preview and a small arrow. This lets the geometry to be dragged out to the desired depth (again, you can key in or eye in values). There are two additional controls you need to be aware of. Firstly, with the small glyph near the feature (by default it shows a plane and an arrow), you can either define the extrusion as running from one side of the sketch-plane, from both (to different values) or symmetrically about that plane. Secondly, below the length arrow, you’ll see a small ball. Dragging this will create the required draft angle. Of course, you can also tap the values into the panel that pops up at the top of the screen.

Adding addition sketches allows you to quickly sketch, pull/push new features into your model.

The Press/Pull command is a multi-purpose tool, in that it allows you to create extrudes and fillets depending on your selection. Select a profile and you have a cut/add extrusion. Select an edge or set of edges and you have filleting to hand. Filleting allows you to work with single edges and multiple selections and you simply press the fillet into place. There is also a handy “match radius” glyph that allows a numerical reference to be taken from another existing fillet radius.

The Press/Pull command can create extrusions, offsets and fillets depending on your selection.

Move

While the Press/Pull command will be used in most instances when modifying and adding geometry, the Move command lets you work with existing geometry and shift it – simply grab the geometry and use a triad to move or rotate sets of faces. There’s also a very handy ‘Select Other’ tool from the marking menu. This gives a heads up way to find geometry related to your current selection, either by topological neighbour (edges or faces which are connected directly to your current selection), by Z depth (which allows you to select obscured or hidden faces behind your current selection), or using the feature selection tool (to find extrude, fillets and such from your selection). The options are displayed on-screen with dynamic previews that show exactly what you’re working with. These allow you to grab the feature or face you want to work with, and then hitting the move command brings up the familiar Triad. This gives you several things to do with your geometry selection. Each axis on the triad allows you to move the geometry in that direction. There’s also a visual reference for rotating geometry about an axis and a free move option using the sphere at the origin.

Using the Move Triad and the F5 key allows you to grab geometry, align the triad to the direction you want to move that geometry and pull it into position.

These small black arrows animate to you show you how your geometry selection can be manipulated.

More traditional features

Alongside the Press/Pull command, there are familiar commands for sweeps, revolves, fillets, chamfers and shell. There’s also a Delete Face operation, but it’s worth noting that the system will only allow you to delete a face if the removal of that face results in a watertight model, once the boundaries have been filled in.

The hole command epitomises Inventor Fusion’s dynamic way of working. When you create a hole, you have a number of options for a straight bore, counter bore or counter sunk holes. These are not standards-based yet (I’d expect that’s coming at some point, as Autodesk already has a wealth of data for that within Inventor 2010), but you simply drag and drop the handles into place to create the feature. That feature is then stored in the browser and can be copied/pasted into another position when required.

Hole creation isn’t yet standard-based, but uses the same dynamic interaction methods to define the various constituent parts of simple bores, counter sunk and counter bored holes.

Alongside standard features, there are patterning tools (radial and linear), mirror of features and part splitting. Because these are maintained as features and remain intelligent, modifications to one mirrored face will result in updates to others within that Mirror set.

Reference geometry is available to assist creating reference with accurate references.

While this might sound complex, in reality, it’s a very easy way to work. When you build successive features, you follow the same, sketch, model, preview, build workflow. Sketching is much more fluid than in Inventor 2010. If you create a sketch on an existing face, the system uses the boundaries that already exist and you can simply drag that profile loop into shape, without all that messy face splitting business.

That’s it for Part One. We’ll be back at you soon with Part II looking at working with existing geometry, assembly creation and model annotation. Before we go, no post would be complete with some video.

Autodesk has officially launched Inventor Fusion (we reported on it at AU late last year). The company has finally come out from the cloud of secrecy surrounding Inventor Fusion and talked to the press/media about it openly. While there’s not been a great deal new learned in the last few days (as it’s still a while away from becoming available) it’s worth answering the major questions that cropped up. We’ve also got some better quality video showing how the system works in different use cases, so let’s mix up the two.

#1: Why?

Fusion #1: Here you’ll see how the system is configured to model from scratch. Things to look out for are the stripped back UI, how the majority of commands and operations are both highly context sensitive, and present in a radial manner around the cursor.

This one is easy. Inventor is currently a history-based parametric modeling system. Quite a number of Autodesk’s competitors have been developing systems which are not. These systems allow you to dynamically edit geometry without recourse to parametric design, without recourse to history – no regeneration, not flipping hourglass. Due to the nature of these systems, they allow you to work with geometry from other systems nicely.

And those other vendors have been making quite a lot of noise about it. Hence, Autodesk’s response. Yes, I’m sure everyone’s been working on something similar. Facts of the matter are that workstations of the last 20 years (since the release of Pro/E) have not had enough power to carry out these types of calculation in one go.

As a result, each model’s construction was split up into chunks (features) and executed in linear order (history). But we’re now at a stage where the compute power in your average workstation is sufficient enough to allow to do both, simultaneously. While the development of this technology was inevitable, the release of SpaceClaim and the subsequent acquisition of CoCreate by PTC, all brought things to a head and provided the catalyst. Here we are.

#2: Is it the new Inventor?

No. Not yet. It’s a technology preview. As such, its a system that you’ll be able to download and play with. Essentially, Autodesk want users to knock the rough bits off it, kick it into shape and see where it goes.

#3: Will it be the new Inventor?

No. Well. Sort of. The name is the clue. Fusion is about bringing in a new technology into the Autodesk offering. Eventually, I would imagine and it was confirmed during the launch web-conference, that all of this technology (in whatever form it ends up once the Technology Preview is over) will become part of standard Inventor – unless users want otherwise.

#4: What’s the difference between this and SpaceClaim, CoCreate, and Siemens’ Synchronous Technology et al?

The modeling technology is not particularly unique. Whatever system you work with, if you’re working with basic, prismatic and well translated parts, then it’ll work like a dream. Step outside of that, and it won’t. Basic topology changes will be OK, dramatic ones will not.

Inventor Fusion does have some very nice User Interface details, radial menus at cursor (rather than menu), stripped back dialogs, context sensitivity – it’s all there. It’s very NX like in fact. For me, that’s a 100% good thing.

Fusion Video #2: Here you’ll see how the system works with existing geometry, making design changes and editing patterns/array. While you’ll see a feature tree to the bottom left of the UI, that’s feature only – not a history tree. So updates are made instantly.

#5: So, it looks like other systems, works like them, what’s the Big Deal?

The Big Deal is this. Now, this is only demo-ware at the moment, but the potential is huge. You can take a history+parametric+feature-based part from standard inventor into Inventor Fusion. In Fusion, you can edit the geometry of the part, delete faces, move specific instances from a pattern.

Fusion Video#3: Edits are being made to this transmission housing, using the direct modelling tools. Note how the system is pulling, dragging and droppping non-native data.

You can then read it back into Inventor, have the system interrogate the part and reconfigure the history and feature tree to accommodate those changes. Whizz bang, your part has been round-tripped successfully, edits made without recourse to history.

Now, the quick amongst you (or the cynics) will say – surely that shows that you’re lacking tools in standard Inventor. Absolutely. but consider that eventually, this technology will be one and the same system. that’s intriguing. That’s mix and matching direct editing with parametric and history-based design and maintaining that history. Creating a Fusion. That, my friends, is very interesting indeed. See, I told you it’s all in a name.

Register your interest at www.inventorfusion.com