4/11/2008
Optimum mesh. Decided to solve the turbulence viscous layer by refining the mesh until we get yplus less than 5 at the wall. (cell of about 30,000 is good enough to resolve the layer)
Decided on the single bend. Use h = 1.5w and compare with h = 1w
w = baffle spacing
For h = 1.5:
Get Pressure coefficient loss of 3 across the bend
Lots of stagnant flow at the bottom corner
Yplus at wall less than 5
For h = 1;
Pressure coefficient loss of 3.21 across the bend
Yplus less than 5
Explanations:
Lower h has higher pressure coefficient loss. The fluid need to flow through constricted region which increase the frictional losses as compared with the flow through bigger h?
Evaluate the current progress
1. Model and validate a simple 180 degree turn over two baffles:
Create fully second order accurate model (done)
Perform mesh sensitivity analysis (using coarse, medium and fine meshes) (done)
Model the baffles using alternate Turbulence models (K-e Standard, K-e Realizable, K-w)
Analyze the effects of changing the baffle clearance height (done. increase height = decrease in pressure drop)
Understand and analyze the relationship between Strain Rate, Energy Dissipation and Kinematic Viscosity
Create a flexible mesh that uses parametrization to easily change geometry dimensions
Analyze the effect of the Reynolds Number on the results
Analyze the sensitivity of the model to convergence residuals (done)
Change the velocity inlet to 0.5 m/s to check the Reynold's number effect. We see that the pressure difference is about the same delCp = 3.04;
3/7/2008
Boundary layer
first row = 0.0015
growth factor = 1.13
rows = 6
Depth = 0.0124841
Third boundary layer
first row = 0.003
growth = 1.025
rows = 4
depth = 0.0124575
3/3/2008
Create boundary layer at the wall. Assume the BL thickness is 0.012 m from the previous results.
File name: sharp bend medium boundary layer.dbs
Goal: Create 15000 elements mesh with special treatment to the mesh at the wall.
First row = 0.0005
Growth factor = 1.19
Rows = 10
Depth = 0.0123544
With the boundary layer, use edge mesh of 0.005
Mesh the faces.
Export as mesh to be solved in fluent
2/20/2008
Mesh for 180 pipe using the baffle spacing of pilot plant: 0.1 x 1 m Mesh vertical (first length = 0.001, interval count = 100) Horizontal (successive ratio = 1.1, inverval count = 20)
Now solve in fluent (Using parameter from pilot plant)
vol flow rate = 109 L/min = 1.82e-3 m^3/s
pipe diameter = 3in = 0.0762m
area = 0.018m^2
velocity = Q/A = 0.1m/s
2/18/2008
Mesh for 180 pipe bend done for both sharp turn and smooth turn. Mesh criteria: successive ration 1.1. Interval size = 0.1 for vertical line and 0.05 for horizontal line.
2/15/2008
Tutorial of flow over mixing elbow.
Used own mesh. Use the tutorial method. Obtained the solution (with back flow warning). Result not quite the same. Maybe due to different mesh. They used unstructured mesh, I used structured mesh.
Good thing to note:
#
When setting boundary conditions of the inlet and outlet, they use
Turbulence Specification Method: Intensity and Hydraulic Diameter. (Turbulence intensity, hydraulic diameter)
Use pressure outlet for the outlet boundary condition.
Use adapt --> Gradient > deselect coarsen >compute > enter value for refine threshold > mark >manage.
#
Create a mesh with more elements. Following the same steps, still not quite the same as the tutorial solution.
Ok, after this, I will try using hydraulic diameter to our pipe bend problem and see whether the result changes.
Remember to use 3ddp when open fluent for the previous file.
2/7/2008
3D 90 degree elbow
First mesh face using Quad, Submap, then mesh volume.
Interval size: 0.001
Take too much time.
Fail, only mesh the faces
2nd mesh face using Quad, Submap (interval size 0.005), only Stair steps option are available for mesh volume (interval size 0.001).
Workable. Maybe not... still too long...
Use Quad Submap 0.005, use stair steps 0.005. Get result.
In Fluent:
Use K-e model. Use liquid water. Set inlet = -39.9 in x direction
Got the mesh. Now need to compare.
Mesh 5 is the good one! The velocity vector compares ok with the data. The difference might be due to our mesh not refine enough causes truncation error.