1. leave the solver as laminar and turbulent, more info on why in the kb.
2. don't worry about the turbulence parameters, more info on why in the kb.
one issue with your description is that you gave us the expected results but not what you got out of flow simulation. you said higher, but how much higher? what about the mass flow rate? what happened to your water?
in my opinion, the issue you ran into is expected. your virtual model doesn't match physical. in the virtual you have a straight tube, in the physical your turbulators.
is your goal to exactly match the 2 and correlate them so you can do future testing?
in the end, you need to find a way to model the outer tube to match physical. 3 ways I can think of:
1. model the actual geometry. did you try a sample to see how bad the solve time is?
2. don't model the turbulators and replace with porous medium. will get tricky.
3. don't include the outer tube at all and fake it with a convection coefficient.
I'm curious to see what the kb says on these, but it appears to be down at the moment. I selected "turbulent only" because I'm worried that the simulator will calculate the flow in the tubes to reach a laminar state, which it would not with turbulators. The water side fluid domain is set to use laminar and turbulent. The tubes are 1.38" I.D. and 79" long.
The resulting gas outlet temperature in my simulation was 480 F, considerably higher than the expected 120 F that was measured on a prototype.
The water behaved more or less as expected in the simulation except that the outlet temperature was about 10-15 F lower than expected and measured on the prototype. I have the water side boundary conditions set up using volume flow rates of 37.5 gpm for both, and 80 F inlet temperature. The 37.5 gpm flow rate is based on testing procedures.
I have not actually tried modeling the turbulators to see what it does to calculation time. There are over 100 tubes in the heat exchanger, and the turbulators run almost the full length of the tubes. I just assumed it would be too great a load on the calculations.
I haven't tried anything with porous mediums yet, but that might be a good way to simulate the turbulators with less calculation load. I'll look into that idea.
I'm not sure what you mean by "fake it with a convection current," but I have considered trying to make the tubes into generic heat sources rather than modeling the gas flow through them. I don't actually know how to do that yet. Is it possible to create a long cylindrical heat source that decreases in heat output as you go down the length?
Are you really using only 1 inch of water as a pressure driver? I wouldn't have thought that would be enough to move an appreciable amount of gas through thin, baffled tubes.
In the actual boiler, the pressure is driven by the blower on the burner. The 1" pressure drop through the tubes is mostly created by the turbulators.
For my simulation, I am only modeling half of the total boiler, and using data measured between the combustion chamber and heat exchanger sections as my inlet pressure condition to the heat exchanger tubes. The tubes are 1.38" I.D., so they are not that thin.
The turbulators are altering both the pressure drop and the turbulence which makes it tougher. I doubt you're going to get a similar effect from something that isn't mesh intensive. Adding a uniform cross-section feature to split flow into 2 would increase drag to get your pressure differential right but you don't have the mixing turbulence of the Brock. The lack of turbulence is going to dramatically reduce the heat transfer to the tubes so you'll still be off. What kind of Reynolds numbers do you get without the turbulators in the model?
Have you tried adding the turbulators to see how much it increases simulation time? Even if you dumb down that portion of the mesh so it's all partial cells and not solid cells it might induce the swirl you need. Or at least give you an idea of the HTC to force the wall condition without them in the full model.
Are the turbulators floating? i.e. not good conductors to the wall (welded/soldered) such that the extra surface area transfers heat along the ribbon to the wall and into the water? If they only affect pressure and turbulence then dumbing down the mesh will still be accurate.
Otherwise, as Jared said, you might need to look at adding a porous medium to replace the turbulator. But while that gets the backpressure that may not be good for the heat transfer because it would affect the cross-sectional uniformity of the air temperature because it's not tumbling.
If it were me I'd mock up a single tube to include the turbulators and tweak the local mesh so you can see a swirl in the partial cells to make sure it actually swirls the flow, then step up to the full model and bite the bullet and run it over the weekend.
The turbulators are floating and don't contribute any significant conduction to the tube walls and water. They have only small points of contact with the tube wall.
An additional note: in the simulation that gave me 480 F outlet temperatures where 120 F was expected, I left the turbulence intensity setting at its default 2%. I also ran a different simulation (same gas tubes, but different baffling of the water side) using 100% for the turbulence intensity. Using 100% intensity gave me lower gas outlet temperatures, in the 200-250 F range.
Since then I have roughly calculated an intensity of 86% based on the u'/U calculation and the changes to the flow area withing the tube caused by the turbulator.
It may be possible to break this down into simpler simulations. If you could accurately model your heat flux coefficient between the tube walls and the water (using experimental data or a detailed simulation of a fixed tube) then you could implement a larger scale simulation with solid bodies representing your tubes inside the shell.