Inventor Fusion Technology Preview 2 – Part 6

In Part 5 of this series, I wondered whether the Fusion technology involved secretly keeping track of the direct modeling operations and then using this data to cook up the changes and treatments in order to modify the original history based feature tree. Or does it involve comparing the changed dumb model with the original feature tree and doing the next to impossible task of editing the features, parameters, constraints, etc. of the feature tree. In this post I will attempt to answer this question.

As I mentioned earlier I do not have access to any inside information about the technology. All I have is Inventor 2010 with the Change Manager add-in and the standalone Inventor Fusion application. I know I could use low level system tools that scan memory and track file I/O to sniff out what the Fusion application is doing internally while the user carries out direct modeling operations. But using that approach would be more like a hit and miss. So, I decided to use an approach that was borderline crazy but completely foolproof. I decided to carry out the direct modeling operations in a software other than Fusion. If the Change Manager could come up with the changes and treatments without me using Fusion’s direct modeling tools, then I would know for sure that Fusion had nothing to do the Change Manager’s ability to cook up the changes and treatments.

But there was a problem. The Change Manager can understand only Fusion-flavored DWG files. So how was I to create a DWG file that was Fusion-flavored and yet not use Fusion’s direct modeling tools? As you will read below I actually managed to pull it off.

I started by creating a 3″ x 2″ x 1″ box in Inventor 2010 by extruding a 3″ x  2″ rectangle by 1″.

My aim was to convert this box into a 3″ x 3″ x 3″ cube. This meant that the sketch would have to be modified to be a 3″ x 3″ square and the extrusion distance would need to be increased by 2″. That’s two changes. I saved this model as an IPT file and opened it in Fusion. I immediately saved the model to a DWG file and closed the document. I did not use any of Fusion’s direct modeling tools. A simple File->Open and File->Save which ended up giving me a Fusion-flavored DWG file.

I opened the Fusion-flavored DWG file in AutoCAD 2010. Yes, AutoCAD 2010, not Inventor 2010. Not surprisingly it contained the 3″ x “2 x 1″ box. And this where things started to become a bit messy. As it turns out, you cannot simply edit the model in AutoCAD, save the DWG file and open it in Inventor 2010. If you do so the Fusion-specific information will be lost. By digging deeper, I figured that a Fusion-flavored DWG file contains a single block called ACAD_FREEWAY_COMPONENT_1 which contains a single AutoCAD 3D solid. At least for this experiment this was how it was set up. I somehow needed to maintain this structure so that Inventor 2010 would think that this was a Fusion-flavored DWG file. So I exploded the block in AutoCAD to expose the 3D solid. I then used AutoCAD’s Move Face tool to move a side face and the top face of the box so as to get a cube. I then redefined the AutoCAD block to contain this cube and not the original 3″ x 2″ x 1” box and then saved the DWG file.

So basically I did the equivalent of what Fusion would have done if I had pulled the box faces using Fusion’s direct model tools. Just that I did it in AutoCAD and maintained the Fusion-specific information in the DWG file. So now was the time to check if Inventor 2010 still recognized the DWG file saved from AutoCAD as an Fusion-flavored DWG file and kicked in the Change Manager. It did! I opened the DWG file in Inventor 2010 and the Change Manager started.

As you can see from the image above the Change Manager recognized two changes and recommended two treatments both of which involved editing a feature. The changes were highlighted in the model view.

As you can see from the image above, I was going to end up with a cube. But the real question is how this cube will be created. Will the 3″ x 2″ rectangle in the sketch be modified to 3″ x 3″ square? Will the 1″ extrusion distance be increased by 2″? To find out I clicked the Apply All button and both the Edit Feature treatments were applied. I quit the Change Manager and observed the sketch and feature tree. As you can see from the figure below the rectangle in the sketch is now a square.

And the extrusion distance has been increased by 2″ and now stands at 3″.

So this simple experiment proves without a shadow of a doubt that Fusion does not secretly keep track of direct modeling changes which could be then used to guide the Change Manager. In this experiment the direct modeling changes were not done using Fusion at all. For further confirmation you can try out the things Kevin Schneider from Autodesk mentioned in this comment to Part 5 of this series.

Like I said earlier, my purpose for writing this series is not to see how well Inventor Fusion can create a cube from a box. Rather it is to get a better understanding of how this technology works. I understand that users are more interested in knowing whether a software can do something and not how it does it. That’s why I urged you earlier not to take this series as a review of Inventor Fusion. This is more like a technology review, not a product review.

In the next part we will see what happens when the Change Manager fails to come up with a solution. What options does the user have? Stay tuned.

  • R. Paul Waddington

    Thanks for this series of post Deelip.

    As an aside, I have said it before and I say it again, put Fusion into AutoCAD to extend what we can already do; I’ll be quite happy and so will many others.

  • R. Paul Waddington

    Thanks for this series of post Deelip.

    As an aside, I have said it before and I say it again, put Fusion into AutoCAD to extend what we can already do; I’ll be quite happy and so will many others.