Need help with creating surfaces from multiple sketch lines.

I will get to the curves question. It looks like you are attempting to build a surface that is 3 sided, that is not a good idea. You should build a 4 sided surface and trim it to achieve the 3 side shape shown in your pictures. It also appear you are using 2 boundary curves with an internal curve in your last picture which is not a good way to create this geometry. If you get it to regenerate successfully it will almost certainly not offset to a thickness if needed downstream. Look at the Guassian curvature if you do create it and look at the pointy vertex corner of the surface. Connecting anything to that boundary will also likely be problematic.

For style curves you should directly build the 4 external boundary curves and then add internal curves if needed to control topology inside the boundary. These curves can be built with core Creo features or Style curves and can be mixed in surface construction within style features. When selecting the curves you can use the selection paradigms (chains, loops etc.) to combine/trim curves to define the boundaries. If you are not familiar with this refer to the Creo quick reference card for selection tips.

In the picture immediately below a concept for a curve network to create your geometry is shown. Red represent the 4 boundary curves, green are internal curves should they be needed and the white shows the curve to trim after the 4 sided surface is built. In your case it looks like the flange is planar so you can trim the surface with a plane to get your 3 sided surface quilt and you would not need to create the white curve. I do not think you need the green ones either for you geometry. You also need to pay attention to curve connection and continuity in anticipation of joining other surfaces needed to create solid geometry and thicken it. Take this as a general approach to get a 3 sided surface as matching the opening in the flange is probably not going to work using a single 4 side surface because of the fillet in the corner.

Trim 4 side surf to get 3 side surf

I am speculating the this is a gear differential case design that will be machined or cast based on the file name. Unless you are trying to learn to use style features I would suggest using core Creo features to get the case geometry. I have designed machined and cast gearboxes and would not choose style features as a preferred tool to create the general form for that type of design. If you can get the geometry with core features it is usually more straightforward and easier to control the design intent in the model without style features. You can parametrically control style features but it requires more construction geometry and planning of the design intent to make it useful to modify models.

The picture below is a simple example of a cast & machined cylinder design that is water cooled and has internal water passages as well as the porting passages for combustion, all built without using style features. You can get pretty complex topology using the core feature set.

Cast/machined cylinder with liner