Bad import STP file with creo 8

You are asking why when you are importing a STEP file into Creo it does not make solid geometry from the import feature? This happens with some files, and it can be caused by many things.  Post the STEP file here (put it in a zip file) so we can review the data and results of the import.

If you want a quick fix, open the STEP in Spaceclaim and then export it is a solid STEP and try importing this into Creo, it may resolve the problem.

If you want to learn how to deal with this inside Creo then start by reading this article.

Article - CS53903 - [Knowledge Hub] How to repair and heal imported external geometry (IGES or STEP) for solidifying in Creo Parametric

It could be as simple as an accuracy problem; you could try using the external accuracy setting on import (see above article).

There are a few things you can do to possibly improve the results. 

During the import, select Details.

• On the Model tab, set Model Accuracy to External (If you know the accuracy of the original model, set your model accuracy to that before importing)
• On the Topology tab, I always start with:
  • Join surfaces from different layers - No
  • Join surfaces from the same layer - Yes
  • Solidify closed volumes - Yes
  • Close gaps between surfaces - unchecked
  • Repair unsatisfied geometry - unchecked

The model accuracy, I feel is the most important.  The math between different accuracies rarely works well.  You can turn on the repair options but understand that surfaces will be changed.

In addition to what kdirth said, I also uncheck all options on the surface tab (G2 fix, simplify surfaces, etc).

I want the STP file to come in with as little modifications as possible. 

In my experience, the automatic fixes make things worse 99.999% of the time.