hi, i have completed the incompressible flow simulation at 0.3 Mach. Now i want to do the compressible flow simulation with 0.7 mach.

What steps should i take?

i have done the following:

selected density based with node gradient implicit solver.

boundary conditions are: pressure inlet, pressure far field, pressure outlet, wall and interior.

k-epsilon model. It is not converging?

Thanks

u need to apply ur fluid material as Ideal Gas.

i am using Ideal Gas. please tell any other solution Thanks

i also have this question.if i want to do the compressible flow simulation with water ,i may select idea-gas?

yes, you may have to select ideal gas. selecting ideal gas means varying density. but do you really want to do the compressible flow simulation for water, because water will be more or less incompressible over a large range of reynolds number.

as i know the node gradient is harder to converge.

or maybe u can try to create a finer mesh for your model.

u using k-e standard model? maybe can try realizable.

Compressible analysis requires a careful approach as it is very prone to divergence.

My recommendation would be:

1. Do the Mach 0.3 flow simulation with ideal gas flow and use the pressure based solver. (Don't use the density based solver...it will give a whole lot of problems) 2. Increase the speed to Mach 0.5, and use the mach 0.3 flow results as the initial condition. 3. Once converged, increase the speed to Mach0.6 using results from Mach0.5 as initial conditions. 4. Continue to Mach0.7, with mach0.6 as initial conditions.

Also try the following: 1. Use pressure far field instead of pressure inlet for the inlet. 2. Reduce under relaxation factors accordingly.

The trick is to be patient and increase your speed slowly for best convergence and results.

Hope that helps

i hope this will work. i will try this. can you tell me what is difference in density based and pressure based because you are telling density based will give whole lot of problems. And can i use pressure based only for 0.7 mach. I dont have to go more than that, however i am expecting that in some places i may get mach number more than 1 due to the geometry.

Thanks in advance.

It is very difficult to explain the difference between pressure based and density based solvers, I would suggest going through the users guide. But pressure based solvers can handle even supersonic flows, so you should be able to get decent results using them. You only need to use the density based solver should you want to do simulate complex highly coupled density and flow conditions, such supersonic simulation with multicomponent flow and combustion (like when you want to simulate the ramjet effect). Otherwise, pressure based should be OK.

If you are expecting local mach number to reach supersonic speeds, you will need to ensure that your mesh is fine enough to accurately predict any shocks that might appear. Your best bet would be to use mesh adaption, you can use the pressure gradient as your adaption characteristic.

Also, remember to include viscous heating with your turbulence model, as the high speeds will cause an increase in temperature, which will affect your local flow conditions.

Hope that helps.

yes!i want to make an simulation of piston-pump,so i must consider the compressible of water. if the media is water,we just select ideal gas or we will write a UDF for it?

[TeddyNguyen]

simulation credit


Thanks for sharing this useful information. It's great.