Tips for Managing Time-Dependent Thermal Analysis

If you want to do a time-dependent FEA analysis, you generally need the nonlinear solvers that are available in SOLIDWORKS Simulation Premium. The notable exception to this is the thermal study. This solver, available in Simulation Professional, treats both steady-state and time-dependent problems. In this post I’d like to get into a few of the lesser-known tricks that allow you to ask a wide variety of temperature-related questions, with fewer studies and less overall setup time.

Button Pushing

First, the basics. You change a thermal study, from steady-state, to time-dependent treatment, by right-mouse-clicking on the study name at the top of the Study Manager, and select Properties. Right at the top of the Options tab, (shown below) click on the button for Transient.

Once you’ve done this, your other thermal boundary conditions will behave differently. The temperature load will now allow an option to constrain the initial temperatures, and all the loads will allow a time-curve to control the rate at which they are applied.

Solution Type: Transient

But I’m assuming most of you are already down with this – if you need more grounding in how to apply the loads, I suggest you come into one of the CAPINC offices for one day of the Simulation Professional class.

Time Constant

The next thing you encounter in the dialog above is the settings for how long the study should run, and how many time-steps to record in the post-processing files. It’s important to know how fast (or slow!) your thermal processes will act, so that you make the study run long enough to capture the behavior of interest – but if you estimate too high, and ask for a ton of time increments, you will be waiting too long and flood your hard-drive with data files. So, it’s a balancing act.

The purist in me remembers: Way (way) back in college, we learned how to compute the ‘time constant’ of a system, to figure out (roughly) how long it will take bodies of a known mass and specific-heat capacity, to heat up by an anticipated dT, or to weep out a set quantity of heat.

I seldom take the time for that anymore – the computer tools have made me lazy. Fact is, a Thermal analysis is wonderfully linear. Instead of six vector components of stress to resolve, the system has only one degree-of-freedom – a scalar temperature. And the other boundary conditions are linear, or at least, linearized, in a Thermal study. So we can throw some pretty big darts. Whereas a time-dependent Stress study might not be accurate, (or might not even converge), unless the time-step is milliseconds (or microseconds?)… A thermal study can have very large time-steps and still produce useful results.

So, how do we abuse these facts? First, for any time-dependent study, you should also set up a steady-state study, to know what the final temperatures should look like. Then, in the Transient problem, if your initial gut feeling is that the study should run for about one minute, make the study run for five minutes. And ask for time-steps of one minute. Compare the resulting five output frames to your steady-state study, and see if you’ve already soaked-out at step one, or maybe temps are still rising at step five? In effect, aim really high, and over-estimate the settling time. The thermal problems run really, really fast, so there’s no harm in running (and then revising and re-running) this five-step study, several times, until you know you’ve bracketed the correct settling time. Once you’ve established the true time bounds, then set the duration and the time-steps to suit your final plotting/reporting needs.

Initial Temperatures

Here, I want first to reference another CAP posting, about manually assigning initial temperatures to your parts. It’ll help you avert the mistake of accidentally setting your outer surface node temps, (which would leave all the interior nodes un-initialized).

And that tip is actually all you need, if your thermal studies always start with all components at the same, zero-strain reference temperature. But what if you have an electronics package that can run at, lets say, two power states. Maybe when you first turn it ON, it ramps up slowly to some low-power wait state, and perhaps at this state you do not even turn on any internal fans yet. Then maybe there are two other power-states, depending upon functions invoked.

If your loading profile for a device looks like the graph below, then you might very well want to ask things like, “How long does it take to reach max temperatures when I switch from the low-power state, directly to the “transmitting” state? Or, if the device has been transmitting for a really long time, and then we drop back down to “receiving”, how hot will the components be after 10 seconds operating at that state?

Power Consumption at Function States

Questions like this could be pretty annoying, because, although the switching between hi- and medium-power could be a fast-acting, short-duration event, perhaps the soak-out time to get UP TO the high-power state might require a really long solution time. How, then, to simulate individual transitions, without needing to reproduce the entire loading history? This question is answered very neatly by the next option, “Initial temperatures from thermal study”.

Initial Temperatures from Thermal Study

The output from one Thermal study can be used as the initial state of another Thermal study. The ‘initial’ study can be either steady-state, or a particular time-step of a Transient run.

Thermal Stress

This mechanism of feeding one study’s output, as the input to another study, is used In SOLIDWORKS Simulation to also get the stresses and strains associated with the state from a Thermal study. The dialog below, taken from the Properties of a Static study, shows how you can link to the output temperatures of a particular Thermal study, and especially, at a particular time-increment.

Temperature for Thermal Study - Slow Cool

There are a couple of important logistics that go into making these two studies work together. The first is, they must have the same mesh. There has to be a correspondence of the finite-elements. But also, you find that the meshing requirements for Thermal are pretty low – the accurate reporting of stress and strain, requires a lot finer mesh, than does temperatures. So you should create the Stress study first, apply your choice of mesh settings and local mesh refinements – mesh, but don’t run it yet. Then, with the Stress study active, you can drag-n-drop the Mesh folder, onto the tab for the thermal study.

This copies the settings, mesh controls, and also the resulting mesh, to the thermal study. Now, on the thermal study side, you might very well apply additional controls, such as a Contact resistance. If so, then you will need to re-mesh the thermal before running, and then that would mean that you must drag-n-drop the mesh to copy it back to the Stress study, before you can finally run it. The final Stress mesh should always be copied from the Thermal study.

OK, finally, let’s say you have a time-dependent thermal analysis, of a part growing (or shrinking) due to temperature, that has, say, 10 time-steps. And now what if you want to animate a 10-frame movie of the stress or displacement caused by the temperature changes?

This is fairly easy to do also, providing that you set up the stress study, not as a Static study but as nonlinear. (Note! This now means that you must have a license to SOLIDWORKS Simulation Premium). In the nonlinear study properties, you change the solution time to be the same as the thermal, and you override the time-stepper to create manual time-steps, the same number as in the thermal study.

In the vast majority of cases, a system’s stress and strain components react very fast (milliseconds) compared to the flow of heat, so this changing of the time-step to be huge leaps, will not affect your accuracy. So the assumption we are really making here is that the Stress solution is quasi-static, each time-step is effectively a static-equilibrium solution, with mass-dynamics not taken into account. For this reason, when you are first creating the nonlinear study, you want to choose the study sub-type as STATIC.

Nonlinear, but Static

Then, when you go into the Study Properties, and define the Thermal Effects, just as we’ve done before, you notice that a nonlinear study has an additional option for how/where to reference the temperatures.

Nonlinear - Static. For each nonlinear time step, use temperature from corresponding time of transient thermal analysis.

Of course, this checkbox will work as desired because we made sure two studies share the same duration and time-steps. Effectively, we are ‘meshing’ time – and the two studies must have matching granularity, exactly as the thermal/stress study geometry must have the same spatial mesh.

I hope these tips will save you some time, next time you’re feeling the heat.

CAPINC was founded on one core principle: Provide the best solutions and services to assist our customers in designing and developing better products. CAPINC provides premier solutions and services in New England to assist our customers in accelerating their design and development process for better mechanical products. Our award winning technical support team is comprised of industry experts with hundreds of years of combined practical experience in mechanical design, design validation and analysis, product data management, and technical communication. We are the award winning 3D solutions partner offering SolidWorks software and training, and the entire Stratasys line of 3D printers and production systems. For more tech tips and blog tutorials check out CAPINC's blog and videos.