Inventor 2015: Body Integrity Check

Posted on September 4, 2014 by Mark Lancaster, Synergis Solutions Product Specialist:
Back in July, I hosted a Synergis60 (our monthly free) webcast regarding Inventor Tips and Tricks.  For those who were able to attend, hopefully you learned something new and were able to apply these items into your modeling workflow.  If you were unable to attend the webcast, you can still access the recording.
In wrapping up my presentation, I informed everyone that Inventor 2015 has a secret.  A secret, you ask?
Yes, in Inventor 2015 there is a new (undocumented) feature called the “Body Integrity Check”.  This utility analyzes your model for geometry errors and is useful in determining which modeling feature could be causing the issue.  However, at the time of my presentation, I was unable to demonstrate this utility due to not having any failed modeling examples on hand.
Since then, I received a case where a customer was having failures when trying to extrude a couple of sketches.  Though the model was done in release 2014, I instantly thought of this tool and in the end I felt it was a time saver in finding a starting place in resolving the overall issue.  I would like to take this opportunity and share how this tool can be useful in determining failures in your model.
For this case, the customer was unable to extrude Sketch 44 and 46 using the extrude settings they required.

So in previous versions of Inventor how would you actually determine what was causing the failure?
For Inventor 2015, I would simply launch the utility by using the <CTRL>+<F7> key combo and presto: a dialog appears stating there is a “surface irregular” issue in the model.

Okay so there’s a surface irregular issue in the model. Not much to go on based on that information. Which modeling feature has the issue then?
To determine where the problem is, we first need to break down our model into smaller chunks by manipulating the browser tree. To do this, we will start by relocate the “end of part” marker to the halfway point in our tree (above the Loft 8 feature) and rerun the utility.
At this point the information came back clean and now I know at least the problem lies somewhere below the ”end of part” marker.

Again we need to break it down into smaller chunks, so I moved the marker halfway between the current location and the end of the browser tree. This time I relocated it between the Extrusion 2 /Hole 2 features and ran the utility to see if the issue was somewhere in this part of the model structure.
                   
Once again the surface irregular message appeared and now I know one of these features (Loft 8, Loft 9, Extrusion 1, Hole 1, or Extrusion 2) is causing the issue.
Now that I have narrowed down the list of culprits, I will now move the end of part maker between each feature to determine which one is actually causing the issue. In the end, Loft 8 was the feature causing the problem. With that and a couple of other modifications within their model, the extrude failure was able to be resolved.
As you can see we were able to pinpoint the issue and start addressing it immediately without spending a lot of time researching the model.

As indicated in my presentation, the “Body Integrity Check” utility can only function if the following are present:

• Must have a C:\Temp directory prior to use
• Must have read & write privileges to C:\Temp

However in certain cases, this tool may fail to launch for you in Inventor 2015. Autodesk is current investigating the reason behind this, however, there is a work around for it.
“Body Integrity Check” work around:

• Caution: This work around requires your Inventor profile to be reset as though you just installed Inventor 2015 on your machine. Proceed at your own risk.
• Please review and fully understand this link prior to you running the Inventor reset utility: http://knowledge.autodesk.com/support/inventor-products/troubleshooting/caas/sfdcarticles/sfdcarticles/How-to-use-Inventor-Reset-Utility-to-reset-the-local-environment-for-a-Windows-User-Account-Inventor.html
• Exit Inventor and launch the Inventor Reset Utility.

Until next time…
Mark L.
Mark Lancaster is the newest member to our Synergis technical team, having just joined us a year ago.  His most previous experience is as the CAD Design Manager of Pall Corporation, one of our long time customers.  In that position, he was responsible for workstation optimization and design management, established uniform standards for the local and global offices, and developed global systems to control and manage their design data.
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