# Continuity Convergence Problem in CFX

 Register Blogs Members List Search Today's Posts Mark Forums Read

July 2, 2015, 03:57
Continuity Convergence Problem in CFX
#1
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 18
Hello

I am simulating a relatively simple case in CFX. A flow in the inlet duct of a compressor is being modelled to study the total pressure loss. I am using the following settings:

- Air as Ideal gas, Reference Pressure 0 Pa, Heat Transfer as Total Energy and Turbulence as SST Model with wall y+ around 1(I am using good quality Structured Mesh with wall y+ around 1)
- At Inlet Total Pressure is used as Bounday condition with 34667 Pa and Total temperature 243k.
-At Outlet Static Pressure is used with 28000 Pa.
-Advection and Turbulence Numerics with High Resolution and Convergence criteria is set as 0.00005 for all the equations.

Initially a run was performed at Physical Time Scale of 0.001 for 350 iterations and I was expecting a good convergence considering the simplicity of flow and good quality of mesh but the convergence of Continuity Equation is not so good as shown by Residuals in the pic1.

Then I considered to perform Time Scale study for this case while doubling and reducing the time scale half(1/2) i.e 0.002 and 0.0005 but that didn't seem to help much. These cases are only performed for just 100 iterations. Residuals for continuity equation are not going beyond 10-4 as shown in the pic2 and pic3.

Then I further considered increasing the Time scale(as increase in time scale helps in faster convergence) to 0.01. This was the biggest Time scale at was solution was stable, further increment resulted in the divergence of the solution but even this big time scale does not aid in acheiving the good convergence for continuity residuals as shown in pic4. This case was also performed for 100 iterations.

So time scale of 0.01 give me a starting guess(as this was the biggest time scale at which solution was stable) to perform further simulations using Step Function for time scale study. 0.01 time scale was used for 1st 20 iterations and then it was increased using step function with some factor and at the end for last 20 iterations time scale was 0.12 was reached(step function). A similar 2nd step function was used with 0.01 for 1st 20 iterations and increment was such that for the last 20 iterations a time scale of 0.2 was used. In these 2 cases atleast I was expecting some better convergence but only to my fustration, not much was acheived. The pics for these two cases are pic5 and pic6.

Can anybody tell me what can be the reason behined this. Large time scales are not helping to acheiving the good convergence(let's leave the accuracy for time being aside). Even step functions with large time scales at the end of iterations didn't help. I am open to any suggestions and will share the further details if somebody needs in helping.

Any help is appreciated.
Attached Images
 t_0.001.jpg (46.1 KB, 39 views) t_0.002.jpg (33.5 KB, 27 views) t_0.0005.jpg (46.5 KB, 24 views) t_0.01.jpg (44.5 KB, 23 views) st_fn1.jpg (44.9 KB, 23 views)

July 2, 2015, 03:58
#2
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 18
pic6 for 2nd step function.
Attached Images
 st_fn2.jpg (44.8 KB, 21 views)

 July 2, 2015, 11:12 #3 Senior Member   Join Date: Jun 2009 Posts: 1,543 Rep Power: 27 I am a bit confused about your interpretation of the physical timescale: A value of 0.001 [s] means nothing if not compared to the residence time, or other scales in the flow. For example, what is the automatic timescale computed by the software ? That will give you a ballpark idea. The automatic timescale includes physics such as residence time, viscous scales, rotating velocity, etc. Is your flow subsonic or transonic ? There is no such thing as an easy transonic flow compressor. Not sure why you mix accuracy with physical timescale. The accuracy of a steady state simulation is based on the mesh used and the active models. Once it converges, the timescale used to reach such solution is no longer relevant As an advice to understand convergence issues, please do the following:Return to first order turbulence numerics. Get a converged solution first, then make it more difficult if you find it worth your time. Write backup files including the Equation Residuals for all equations. Post process a backup file, and locate the region where the maximum residual for continuity. Study the mesh around that section: aspect ratio, skewness, etc. Study flow regime: separated, aligned, etc Hope the above helps,