I'm trying to determine how long it will take to heat up a flat plate (roughly 10mm thick, 1/2 meter by 1 meter) to 150°C slowly by convection and need help with the flow simulation setup.

The model is a simple insulated box with the plate floating in the middle (I'll add some kind of support later) and heated air blowing in from one side, out the opposite side.

I ran it as an internal time-dependent analysis, but after half an hour of computational time, I got about .3 seconds of real time (I'm anticipating about an hour of total real time, so this isn't acceptable). Is there a way to streamline the computation?

Also, will the solver stop when it reaches steady-state? How do I know the final amount of real-time it took to reach steady-state (can this be accomplished with a goal)?

This is my first attempt at time-dependent analysis, so any advice would be greatly appreciated.

The reason that it is taking a long time to calculate a transient analysis in Flow Simulation because the software's solver uses a conservative approach to ensure stability in the solution. This is done intentionally so that the software can be suited to a wider user base without the need for prior knowledge, although I'll admit that in this case it can lead to frustration to the user. I would not suggest a user to go barging straight into a transient analysis without greater instruction and understanding of the underlying calculation.

In short, the same way mesh size ensures a good calculation in space for a steady solution (well, it does also apply to time dependent problems too), the time step ensures accuracy in time for all the primary calculated values for a transient solution. Too large of a time step may can cause the solver to diverge. Flow Sim (being geared towards a general audience) tends to make the time step smaller, sometimes much more so than it really needs to be. The time step that can be used is dependent on the timescales of momentum, mass, energy and species, or in other words, velocity, pressure, temperature and concentration.

An estimate that can be used for determining the appropriate time step is determining how many cells a molecule of fluid can traverse in a single time step; this value is known as the Courant number. In a simplified one-D case:

Typical values for Courant number can vary anywhere from 1-10, where smaller is better, and still be acceptable, but I would recommend to keep it closer to 1, and less than one is best for stability. Knowing

a priorihow quickly your results will vary in time will also allow you to determine what time step is appropriate, but do note that just because values that you are interested in may not change that rapidly, there are other quantities being calculated simultaneously that may have a much smaller time scales, so you will need to be conscience of them as well.In the formula above for Courant number, you will notice that the element size is a limiting factor, and can be devastatingly limiting if you have very small cells. Why? Because you only have one time step, but many many calc cells, thus the time step for the calculation is based on the smallest cell in the domain.

What to do? Without prior knowledge, first

do a time dependent problem with a very coarse mesh!Solve this to figure out how the quantities are changing, and then use this information to select an appropriate time step when going about refining the mesh in space (to the geometry and flow field). As Chris Michalski noted, you can change the time step manually.For more on the Courant number, you could read about the CFL condition in any text book, or perhaps get an overview here on Wikipedia.

Message was edited by: Joe Galliera. Spelling, and added line about CFL condition with link to Wiki article.