[federernadal]

Just wondering, why does CFX solver need to converge the navier-stokes equations while solving Static Structural problems does not?

[JuPa]

In CFX you can turn off unneeded equations in expert parameters. It then stops solving them. Use with caution.

[federernadal]

Right, but finite element method by definition requires converging, regardless of whether it is NV equations or whatever method the structural uses? Why can we only define a particular level of convergence (1E-4 for example) in CFX not structural?

[ghorrocks]

If you use an iterative solver in a structural model it requires converging as well.

Linear structural models use constitutive models which are linear (obviously). This means that there are single step algorithms to solve these by matrix inversion and related methods - this is used by the direct solver and is why it does not need to converge.

As the N-S equations are non-linear so you cannot do "simple" matrix inversion to solve them. The standard approach is to linearise the equations, solve the linearised matrix, then re-linearise the equations with the non-linear bits updated by the most recent solution. So you have two levels of solution:

Solving the linearised equations: This could be done directly (non-iteratively) but for the large matrices CFD usually ends up giving which are very sparse direct solvers tend to be very inefficient. So iterative solvers are used, with multigrid solvers being the current state of the art for CFD.

Solving the full non-linear equations: This method is inherently iterative as you converge the non-linear components through solution of the lineared equations.

So CFX uses 2 levels of iterative solvers, a multigrid solver at the linearised equation level and a coupled solver to solve the full non-linear N-S equations.

[federernadal]

Thanks Glenn!

Quick follow up question -

So, I am working with a relatively complicated model, and each little change I make requires to rerun the convergence (the convergence takes about 6-8 hours). Any quick way to shorten this?

Also, sometimes when I interrupt the solution and open Post I see that the streamlines and other things are somewhat accurate (even though the mass-momentum lines are far from a residual of 1E-4). Can I start being lazy and interrupt convergence quickly? What are the drawbacks to doing this?

Thanks!

[ghorrocks]

If your models are similar you can use the previous model as an initial condition.

The convergence required for useful results varies depending on your case. You should do a convergence tolerance sensitivity study to determine what level of convergence is required in your case.

[federernadal]

Thanks Glenn!

Could you please direct me to a link that explains how to do either of those things?

[ghorrocks]

Initial condition - this is explained in the tutorials and documentation.

I really should write a FAQ on sensitivity studies....

The concept is simple. If you are assessing the sensitivity to convergence tolerance you run the model at one tolerance, then change it significantly. For convergence tolerance go from 10E-3 to 10E-4 to 10E-5, steps of less than a factor of ten are a little meaningless. Compare the results between the two runs using an output parameter of importance, such as drag, lift, pressure loss. If the two values are the same within a tolerance you are happy with then you have a convergence tolerance small enough that your result is not sensitive to it. If the two values are different then you need to make the convergence tolerance tighter by another factor of 10 and try again. Keep tightening until you obtain convergence.

The same concept can be used for mesh size, time step size, boundary proximity and many other tunable parameters. For mesh size there are more sophisticated approaches like Richardson extrapolation - have a look at these techniques after you have mastered the basic idea.

[federernadal]

I see the logic behind sensitivity, but what if we are working with very large models that takes hours to converge? Does it become impractical or do you know of a workaround?

Currently I am working with models that take hours to converge.

[ghorrocks]

Hours to converge? That sounds pretty quick to me. I have done runs which took 6 weeks to complete.

Your sensitivity study can be completed in a weekend. Script it all up and let it run. It will be completed when you get back. That's why they invented weekends - for CFD people to complete long simulations.