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Often Asked, General

What is 'examine geometry' and why should I use it? by cowski
Posted: 30 Nov 20

The 'examine geometry' command will inspect your model for errors in the topology (for example: a self-intersecting face). Such errors in the model can lead to problems downstream such as modeling commands not completing successfully, drafting views reporting errors, CAM toolpath generation errors, CAE mesh generation errors, etc etc.

Start the examine geometry command and turn on all the checks that you want to run. In my opinion, the checks that every model must pass include:
Body checks:
  • Data Structures
  • Consistency
  • Face Intersections
Face checks:
  • Self-intersection
Other checks may be important depending on your intended use, but every model must pass the above checks.

Once the checks are set, set the selection filter to "no selection filter" and window select around the entire model; this will ensure that all the faces and edges are selected along with the body. If you simply single click on the body, only the body will be selected and only the body checks will be run; we want to be sure that the face checks (and the optional edge checks) are also run. Finally, press the "examine geometry" button to run the selected checks on the selected geometry. The dialog will remain open and information will appear to the right of the selected checks (not run, pass, or highlight). The 'highlight' option means that this particular test failed and NX will highlight the general area where the fault occurs.

My model failed a check, now what?
If you are starting with imported data (a STEP file, a parasolid from another system, etc) you will only have "body" features in the part navigator (no features or parameters); whenever you import CAD data, I suggest running "optimize face" and/or "heal geometry" before doing anything else. These commands will help clean up the model and can fix minor errors. Run examine geometry on the results. If it still fails a check, there are few options:
  • ask the originator for clean data or data in another format (warning: this usually results in a wild goose chase)
  • use synchronous modeling commands to delete and/or remodel the offending faces
  • trim off the offending part of the model and remodel it
If you are working with a native NX file (parametric file with full feature history), you need to find out which feature is causing the problem and tweak its parameters or try a different modeling technique. To find the offending feature, I suggest the "divide and conquer" strategy. Let's say your model has 1000 features and it fails a test. Make feature 500 current (cut the features in 1/2) and run the test again. If it passes the test, you know the offending feature is somewhere between 500 and 1000. Let's cut that in 1/2 again and make feature 750 current; if it fails, we know the offending feature is somewhere between 500 and 750. Repeat this process a few times and you will soon narrow it down to a few features. Use "make current feature" one by one and run the test to see where things go wrong. Tweak the parameters of the offending feature slightly and retest. For example: sometimes a 10mm blend works but a 12mm blend causes problems. Continue fixing and checking until your model is problem free.

I posted a journal here to help automate the searching process:
thread561-336862: Examine Geometry Journal

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