Inventor Fusion Technology Preview 2 – Part 7
As in the case of any new technology, people are more interested in what happens when it fails as opposed to when it works. More so when the technology claims to do something that everyone thinks is impossible. In my opinion, it takes a lot of guts to go down that kind of a path and I commend Autodesk for doing what they have done. I believe that the Fusion technology is in its infancy and there is still a lot of work that needs to be done.
The purpose of this part of this series is to determine how useful this technology is when it fails. I know this sounds like an oxymoron and maybe it is. But I believe that any new technology should not have any show stoppers. By show stoppers I mean, things that prevent you from going forward. Show stoppers in new technologies have the capacity to put people off, more so when people are already skeptical about the technology to begin with.
In this part we will see what happens when the Change Manager fails to do its magic. Does it leave the user stranded? Lets us start with the simple 3″ x 2″ x 1″ box that I used in Part 6. I open the Inventor 2010 model in Inventor Fusion and make what seems to be a very simple change. I rotate the top face by 20 degrees using Fusion’s triad.
That’s it. Just the one change. I save the DWG file, open it in Inventor 2010 and sure enough, the Change Manager kicks in.
As expected, the Change Manager detects the single change and recommends an Edit Feature treatment. I can see the change highlighted in the graphics window.
So I click the Apply All button and expect the treatment to be applied. But nothing happens. So I click the Apply Treatment button and get this error message.
I think this message should have popped up when I hit Apply All. Maybe its a bug. Anyways, the point is that the Edit Feature treatment failed and I am being asked to either choose a different treatment of ignore the change. I don’t want to ignore this change because I know I need it. So I proceed to select another treatment. I drop down the list of treatments and find one called Extract Faces.
The Extract Faces treatment is like your last lifeline. When all else fails you can use this treatment to continue working. So what exactly does the Extract Faces treatment do? To put is simply, it compares the original geometry with the new changed geometry and adds sculpt features to the feature tree so that the preferred treatment that failed is accommodated in the feature tree. You can get more information on sculpting here.
So I select the Extract Faces treatment and click the Apply Treatment button. This time it works. I quit the Change Manager and proceed to see what happened to the feature tree.
Two Sculpt features were added to the feature tree which have been highlighted in the following image in cyan.
As you can see the extrusion feature remain unchanged but two sculpt features were added further down the tree. One of them added a prism to the extrusion while the other removed a prism from the extrusion. One can argue that this is not very different from how other MCAD systems offering direct editing tools add features to the bottom of the feature tree. The difference is that in Fusion this is the last option, and not the only option.
Another thing, the two sculpt features added are independent of each other. This means that for whatever reason I can delete one of them if I want to, as can be see in the following image.
I believe as the technology improves, the need for using the Extract Faces treatment will be reduced. Obviously the aim is to eliminate the need for it completely. But till Autodesk gets there, the Extract Faces treatment will be crucial in helping users test the technology.
I am now going to subject Inventor Fusion to some stress tests and see how well it holds up.