I haven't looked into confirming your theoretical calcs and what assumptions are made for them but I would recommend posting your references here. I would also recommend doing some research on how close those calcs come to actual tests.
regarding your flow simulation setup a few comments:
1. what is partial vs complete? i'm not sure I understand
2. when doing 2D simulation, you want the thickness to be as thin as possible. even if the default is 0.2inches, I would go even smaller than that. the solver is still solving a full 3d problem, just with one cell thickness, so you want to minimize the chance of any flow out of the 2d plane from having to be calculated. in general I try to keep it's width so that it correlates with the smallest element size so that I have as close to cubic cells as possible.
3. with respect to your comparison, make sure that your theoretical calcs aren't including any edge/end effects since 2d simulation is assuming it is infinitely long. I would also recommend working with lift force/length so that you're not converting the 2d thickness to 3d.
4. for your mesh, and your comp domain, I would say the size of the cells is still too big and your comp domain is too small. but without a plot of what the flow looks like it is hard to say on the comp domain. for the cell size, it may take 50hrs, but you're going to have to do a mesh convergence check to know if you have an appropriate element size. and you're going to also have to consider convergence criteria and the convergence graphs.
5. I also believe the developers recommend turning the flow rather than turning the components. check the soliworks kb on this.
6. regarding plotting, i'm assuming you are choosing all faces when plotting. if not, you will get incorrect results. I would also recommend creating global and surface goals to make export easy.
overall, this is a really good thing to do before you move onto more complicated problems. it really shows how big the comp domain needs to be, how many cells you need and what level of complexity is reasonable for cfd and whether it is practical or not. there is a good article about this in the kb as well.
I would also recommend you take a look at the validation example of a flow over a sphere. it will comment on all the things I have mentioned here in addition to whether a steady state solution is correct or not. also, it should give you more confidence that the issue you are running into is not necessarily that flow is solving the problem incorrectly but rather it is just a bump in the road from gaining experience in using the software. at hawk ridge we spend a lot of time with customers working through these bumps with our mentoring service.
The lift coefficient for a flat plate is something that I was taught in my aerodynamics course a couple of years back. Here is a good 3 page summary outlining the theory. The lift coefficient is proved on the middle of page 3 to be 2*pi*alpha. This value is for a 2D section, or a wing with infinite span.
I will look into your other suggestions
did a quick look at your reference and don't really see much discussion about the assumptions those calculations make or how they match to physical.
a couple assumptions it looks like it makes:
1. the angle of attack is very small
2. that the plate is very very thin
you'll need to take that into consideration because without considering that, comparing what you get out of flow to a straight hand calculation may be flawed. CFD will likely be closer to reality within the assumptions made by the setup of the analysis. for example there are some limitations to the KE turbulence models that will affect a physical simulation but won't in either CFD or hand calcs.