Welcome to the forum. There are several ways you can do this.
One way would be to create solids of each of the surfaces and then combine them.
Another way would be to perform a mutual trim on all of the surface. If the surfaces intersect the middle portion, this will result in a knitted and "watertight" (fully enclosed) surface. You can then thicken the surface and select the option to create a solid volume.
If a mutual trim wouldn't work, you could create a 3d curve at the base of the blades. You can then use the 3d curves to trim the center shaft. Then knit and create a solid volume.
You could minimize your effort by working with only one of the blades as they are axisymmetrical.
There are other ways too, but if you have surfaces that are watertight, I would start with the first option.
As Mike said, I would model just one blade and the hub as separate bodies, then pattern the blades and combine all the bodies.
If you want to have full control over the model, then you will need to rebuild it in SolidWorks. Use the imported surfaces as a scaffold to help make the SW surfaces and as a check on the accuracy of your SW model.
The hub looks simple, just a cylinder or a slightly tapered cone.
I would use Boundary Surfaces wherever possible on the blades. The center section, where the patches look fairly rectangular can probably be done as a single Boundary Surface, or four Boundary Surfaces (Top, Bottom, Leading Edge, Trailing Edge). You are probably going to end up uses Fill Surfaces at the top and bottom on the end, because Boundary Surfaces like having four edges and will have a degenerate point at the tip.
You might want to make the inner section with a Boundary Surface or Surfaces, possibly even the one that makes the center section, and then trim it back to where the transition to the Hub starts. Trim the Hub as well, and then use Boundary Surfaces to make the transition fillets.
There are other folks in this forum who can give you better advice, since they make airfoils and blades.
Thank you for the responses. If I want to rebuild the blade section, how can I trace the surface?
I would create 3d sketches and use the fit spline function.
I would put planes in places that look good for putting your profiles on. Open a sketch on the plane and use the Intersection Curve to get the existing cross section. Then make a new sketch and build a spline that matches, as best you can, the Intersection Curve. You might need to break the curve up into multiple splines, or break the sketch up into multilple sketches.
The Intersection Curve is just a reference, which you can delete when you are done with the part, so that it is completely self-contained, with no links to the imported part.
Can you provide a file of this part?
I have attached the file with partially rebuilded. I rebuilding the model by creating the multi-sections by fit spline (thanks to mike price). Then I lofted the fit spline, it start form the initial blade section. How I can improve the smoothness of the surface? Where I should add profile edges (on the blade leading and trailing edge or blade face and back)? Is there other option to close loft at the blade tip with a point?
Thanks for all the help!
Looks good. You will have to play with the model to get the surfacing to smooth out. One suggestion is to break up your loft into several lofts instead of one single loft. Another suggestion would be to add guide curves on the LE and TE apex.
Regarding closing up the tip, I would split the surface to give you a couple of short segments on the TE and LE and then create a couple of pressure side to suction side curves so you can loft through. You can then use the open surface edges as well as guide curves.
Boundary surfaces give you a lot of control too so that's something else to try to improve results. As I have had boundary surfaces fail in the models I work with, I try to start with lofts as they are more simple and also more robust. I have never had a lofted surface fail on me yet.
One more suggestion. Sometimes I find that my surface is almost "perfect", but I just can't get the final tweak out. What I will do is to use the surface I constructed as a construction surface, cut out if req'd or just use to create face curves and then delete faces, recreate surfaces. Face curves are a wonderful feature for surfacing work so if you haven't checked that out, I'd look into it.
If you need additional help regarding splitting surfs, etc. let us know.