Discussion Forum

Dear Tiago,

Have a look at following discussion:
www.ch.comsol.com/community/forums/general/thread/35375
My colleague Henrik answers your question in one of his replies.

Also, I highly recommend you to read our recent blog series on solvers and meshing:
www.comsol.com/blogs/category/all/core-functionality/

All the best,
Zoran

Hello Tiago,

I had a look at your particular model and it seems to me that it juist lacks a pressure constraint.
Your laminar flow problem has so far only by slip conditions, which just constrains the velocity (to be tangential) but is would allow solutions at any absolute pressure level. In other words: you have Neumann Boundaries only and your problem so far is non-unique, because pressure is unconstrained.
By setting the absolute pressure in one point you can add the missing gauge.

You will see that the absolute pressure difference in your system is very small 0.007 Pa, if you don't constrain the pressure, COMSOL could find a solution at any pressure level. In fact if you interrupt the solver in your original file you will find a solution at a total pressure of say 2 Pa, it is clear that the relative accuracy criterion is fulfilled, but still the solution cannot be called converged, because COMSOL tries not only to satisfy this one, but also achieve that with a damping of 1.
In our manual (search for "damped Newton methods") you find the note:

"The (automatically damped Newton) nonlinear solver only checks the convergence criterion if the damping factor for the current iteration is equal to 1. Thus, the solver continues as long as the damping factor is not equal to 1 even if the estimated error is smaller than the requested relative tolerance."
If you inspect the solver log the solver cannot achieve a damping of 1 but only 0.7.

Adding the pressure constraint, makes the problem unique and solves the issue that you encountered.
See my attached file solved.

Best regards,
Sven Friedel

here comes my model

Sven

here comes my model

Sven

Dear Sven, Zoran and Luke, Thank you very much for your input. It was indeed a lack of pressure constrain that caused the problem. Furthermore, by mistake, I was modeling the flow as compressible and that was increasing the degrees of freedom of the problem. After introducing the pressure constrain (and using incompressible flow model) the convergence problems disappeared for this geometry. Thank you.