Before sewing the sheet bodies, I would suggest that you run the 'Heal Geometry' utility to clean-up of the model. You can do that by going to...
File -> Export -> Heal Geometry...
...which will result, as it implies, in the creation of a NEW part file where the topology of the model as been 'repaired' (your original file will be unchanged). Now this new file will have had any features removed and the results will be a non-parametric model but it should be 'cleaner'. Anyway, give that a try.
As for what you're seeing now, that's how something called 'Tolerant Modeling' works in NX. Tolerant Modeling allows you to sew together sheet bodies where their edges do NOT line-up exactly. What happens is that if the edges of two sheet bodies do not exactly line-up but they are within the tolerance distance of each other as set in the Sew dialog, then they are sewn together. However the shape and edges of the sheet bodies are NOT modified in any way, but rather the systm uses ONE of the edges as the 'seam' between what are now 'faces' on a single sheet body, and hides the other one. For all intents and purposes the APPEARANCE of the faces is such that it looks like there really is only a single edge which would indicate that the edges really did line-up. Now this was done so as to NOT modify the original sheet bodies since they are what are for some reason and we're not going to change them just to get them to sew together. Now this situation will NOT cause any problems with ANY NX application since all of the downstream tools know how to work with these so-called 'tolerant edges'. This includes other modeling operations, manufacturing applications like generating tool paths on these bodies, creating finite element meshes, performing measurements, etc. Also custom applications written in NX Open will work with these 'tolerant models' AS IF THEY WERE PERFECT.
That being said, when you do something like extract a face from a sewn sheet body with Tolerant Edges, the face created will be exactly like the original sheet body including any misalignments and gaps, but that's the way it's supposed to work and has worked for over 20 years. However, the Heal Geometry utility mentioned before actually does TRY to clean-up the models and can fix some of these misalignments and gaps, but not necessarily all of them, but it can help if you really need to have better aligned edgss. However, NX will work no problems when using these 'tolerant models' because that's how we designed NX to work and it was worked like that, as I jsu mentioned for over 20 years and very few people have ever had a problem with it as long as you didn't use really large tolerances to get a 'result'.
Anyway, give it try and see how NX works with what you have. Most other people have been doing it for years with very few problems.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
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