Nonlinear Transient Heat Transfer Analysis blows up

[dstuebgen]

While conducting a nonlinear transient h.t. analysis, my results blow up and I cannot wrap my head around it. All of the loads that I have applied to this assembly are as follows:

-a linear temp ramp up from 100 to 2650°F over a 10 hour period

-an initial condition temperature of 90°F for ambient air

-and several different convection loads on my walls, roof and floor due to having separate parts of the same material to make up the walls

This same assembly worked in a nonlinear steady state analysis and got temperatures relative to what my company actually sees with this particular kiln. However, due to this analysis having proprietary material data information I cannot directly share anything. Is there anyone out there who could guide me toward an article or two that can explain the steps in trying to find out why my analysis blows up?

[John_Holtz]

Hi @dstuebgen 

Since the steady state analysis gives expected results, I suggest that you check the items that are different in the transient analysis. The transient analysis assigns Time and/or Temperature Dependence tables to the loads. Perhaps one of the tables is incorrect.

• Do the tables cover the full duration and/or temperature of the analysis? If not, the table may be extrapolated which can lead to erroneous results in some cases.
• Does the table use a multiplier or the actual value in second column? (You should do a test model to confirm that whatever the table indicates is correct.)
• If the second column of the table behaves as a multiplier (load scale factor), is your input multiplier times the assigned load correct?

John

[dstuebgen]

Morning John,

-The tables that I have cover the me entire range and then some extra just in case.
-When I was reading about the tables, I assume my load scale factor in the table would be the the actual thermal conductivity of my materials and set the k-value for my material equal to 1. Is this way the correct assumption?

[John_Holtz]

Hi,

I agree with your use of entering 1 for the thermal conductivity and entering the actual thermal conductivity in the table. The end result (the thermal conductivity) is the same whether the analysis is using the table as the thermal conductivity or if the analysis is multiplying the table by 1.

I suspect your issue is a table that is used for the loads. For example, you have a temperature load that changes over time. How was that entered? (The load type, load magnitude, and table input.) If the convection loads change over time or temperature, how is that entered?

It might be a good idea to try to duplicate the issue with a small test model that includes the loads (assuming they do not contain proprietary information) but make everything else as simple as possible (simple geometry, constant thermal conductivity, and so on). If you can reproduce the problem and provide the model, someone has a better chance of understanding what is happening in the analysis.

John

[dstuebgen]

Hi John,

-The temperature load was entered with a magnitude of 1° F with a table starting with (0 seconds, 100°F) and goes up to (36000 seconds, 2650°F) to simulate a ramp up in temperature for a simple kiln.

-The convection loads are entered as an assumed vertical, horizonal hot face up, or hot face down (depending on geometry of course) with a constant convection coefficient (accounting for radiation without directly applying a radiation load) entered at a specific film temperature.

*The convection coefficients should technically change with temperature load, but for simplicity's sake we kept the coefficient constant.

[John_Holtz]

It all sounds okay. You may need to reproduce the setup and problem in a model that you can share. Or if the model can be shared through technical support (instead of through this public forum), you can create a support case through www.autodesk.com/gethelp.

John

[dstuebgen]

Morning John,

I just sent a zip file of the assembly to technical support. Is there anything else I needed to add?

[John_Holtz · Accepted solution]

To summarize the outcome of this thread for other readers, the time step size was too large. Using the Adaptive time stepping kept the temperatures following the prescribed temperature loads.

To provide a little more detail,

• I reviewed the model that was submitted through technical support. The usual problems of a distorted mesh, contact, or excessively large thermal loads did not exist.
• I hesitated to try the Adaptive time stepping because that usually results in more calculation steps than I "think" are needed. With a simulated duration of 36000 seconds (10 hours), I wanted to minimize the number of steps. To my surprise,
  • The runtime was about the same as when using constant time step size of 720 seconds (12 minutes).
  • The adapted time step toward the end of the analysis was larger than 720 seconds. (This surprised me, but that is the advantage of adaptability.)
  • The adapted time step toward the beginning of the analysis was as small as 45 seconds.
  • I will not claim to understand why the temperatures were increasing to infinity at the end of the analysis when using the constant time step, other than to surmise that the large time steps early in the analysis was causing the result to deviate which eventually lead to the run-away temperatures later in the analysis. It was somewhat unexpected but just goes to show that numerical integration has limited accuracy based on the time step size, and how the inaccuracy at step X affects the rest of the analysis is hard to predict. (The analysis included time dependent loads and temperature dependent material properties, so the interaction of time step size, loads, and material properties is quite complex.)

John