If you're lucky, "Sew" will do the trick. If your sheets form a closed volume, without any gaps, the result of the sew operation of all sheets will automatically be a solid.
Also try 'extract region'. This command will make a sheet body of the solid, except for the face you pick as the 'seed face'. If you need that one also you can use 'extract face' on the original solid to get that one too.
If you can give some info as to what you want to do with the sheet body vs. the solid body we may be able to give you more and/or better suggestions.
I am importing a step file. But the model turns out to be many sheets. And there are gaps and losing surfaces. So, I couldn't sew the surfaces. Anyone can tell me how to fill the triangle gaps (tangent at least), and finally I can get a good solid? Thanks.
If STEP can't translate it into a solid and back, then you'll have a hard time doing it manually.
You'll need to repair every tiny gap and every loose end. I'm afraid that the surfaces to solid assistant in UG will not work either. You'll have to use every command available within UG. I hope you have the free form module available.
Remember that Sew is a very tricky command. If you apply to high a tolerance to bridge a gap between surfaces, they will only be sewn visually. Underlying definitions of the surfaces will still have the gap. This may cause problems later on.
It's hard, but the best option is to go to the one how sent you the STEP and tell him/her it's a mess.
First of all, knowing which version of NX you're using would really help when it comes to showing you what commands to use, as their locations can change from one version of NX to the next....or they could even be completely renamed. Regardless, please state your version of NX when posting a question.
Next, make SURE the STEP file was exported as a solid and not surfaces. Some CAD softwares allow for surfaces only in STEP files and that might be why you're looking at a surface model in NX. Also check your STEP import options in NX. Set it to import solids only unless you don't mind surfaces slipping through. If you set your STEP Import Options to solids only, then you don't have to worry about someone accidentally making a surface-only STEP file...it won't import the surfaces. Make sense?
Check your model tolerance in NX. If your modeling tolerance is tighter (smaller) than the software that exported the STEP model, then you're wasting your time trying to get a solid from the STEP file. The tolerances need to either match or NX's tolerance needs to be larger. That's just my personal opinion. Hard to convince me that a larger toleranced STEP file would import as a valid solid into a tighter tolerance in NX, but I've seen stranger things happen with CAD before.
You can use many techniques to repair the imported geometry. Some might include finding the areas with missing surfaces and using the adjacent surface edges to create a Through Curves (TC's) Through Curve Mesh (TCM's), N-Sided Surface, or any other surface command that allows you to control continuity (tangency, curvature, etc.). You might have to use Bridge Curves if the adjacent surfaces are a mess as well.
Should you find a small gap rather than missing surfaces, you can try to edit individual surfaces and untrim (Edit -> Surface -> Boundary) them back to their original shape prior to trimming then re-trim to desired boundaries. Sometimes this prior trimming information is not retained in the translation of the surfaces, other times it is.
If you can untrim, then re-trim surfaces, that will be your best option for preserving the original topology (shape), however, we don't live in a perfect world and you might have no choice other than to rebuild some of the surfaces as mentioned above. As caddict pointed out, being able to play around with the model would help us help you.
Another suggestion to add to Tim's excellent list is to enlarge surfaces and trim them back to their intersections. Many different methods may have to be employed to correct this type of file.
