Questions about Thermal Analysis Inputs

[ccassino]

Hi All, 

I have what I hope are a few simple questions. I'm having no luck finding answers to them in the documentation. For Autodesk Inventor Nastran 2023, when performing a nonlinear transient heat transfer analysis:

1) What does the thermal constraint do?

2) How does the applied heat flux condition work? If I'm applying it using a table of heat flux magnitudes that change over time, do I need to put an initial value of magnitude in the entries, or is completing the table sufficient? I'm getting values of heat added to the model that don't make sense relative to what I think I'm applying.

3) How does the initial temperature condition relate to other applied heat loads? Does it create an initial uniform temperature for all bodies in the analysis and then permit the temperature in the materials to go to zero over time unless they receive another heat input? Or does the initial temperature condition set the floor for the temperature in the model?

4) Is there a way to plot the temperature through a wall in a model as a function of distance?

Thanks in advance for any help.

 Best Regards,

 Chris

[ccassino]

Sharing this graphic so that the heat flux question is better understood. Do I need to put something in the box for Load Magnitude, or do I just need to enter details in the table? I know for a transient heat transfer analysis, I need to have the table with the heat flux as a function of time. But I'm not sure what the original input does. Because the output I get when the 80 is in the load magnitude box is different than expected from following the table input. As in, when I put a value of 10 in, I get different result when there's an 80 in there, despite the table inputs not changing. For this example, I put in values that are all the same. I want it to vary with time. But I want to understand what this applied condition really does before I do that. And before anyone asks, yes, I'm using all linear elements in this model. Thanks.  

[ccassino]

As for the other questions, I have a very simple model I'm running as a test case. It has an applied heat flux and an initial condition. The initial condition is 60 F. The applied heat flux is shown in the reply above. I'm getting cooling in the model as time progresses. I need to set a floor so that the temperature can increase from a minimum, over time, using nonlinear effects. Thanks.

[ccassino]

OK... since no one else is biting, I'll share what I think is happening based on some testing I did last night. It appears the magnitude is acting as a multiplier effect. So, 80 x 80 = 6400 W/m^2. If I put 1 in the initial magnitude slot, and change the table data to a constant 6400, I get the same final temperature gradients and heat added as if I keep the table inputs at 80 and have the magnitude at 80. Since it's a consistent result I can proceed with my analysis. If there's any documentation that contradicts what I just said, please let me know. 

[ccassino]

Regarding initial conditions...the issue appears to have been that if the reference temp is above the initial condition then the model doesn't know what to do. If you set the reference temp to the initial condition temperature, then it doesn't let the temp fall through the floor to zero. Again, if anyone has different information or experience, please let me know.

[John_Holtz]

Hi @ccassino 

It would be helpful if you would attach your test model. That way, we would have a better understanding of how you are entering things such as "initial condition", "reference temperature" and so on. 

Here's some details on your original questions:

1. Thermal constraints force the temperature to be a constant. (Similar to a mechanical constraint that forces the displacement to be a constant value, usually 0.)
2. All loads need a magnitude. The column "Load Scale Factor" in the table means that it multiplies the entered load magnitude by the value. (In general, all tables use the second column as a multiplier for the corresponding input, whether it is a load magnitude or material property.)
3. The "Load > Initial Conditions > Temperature" set the temperature of the entire model at time 0. What happens after time 0 depends on the applied loads and conduction.
4. You should be able to plot the temperature as a function of distance for a selected edge of the model. Therefore, you may need to split the model or face to have an edge where you want the temperature distribution "through the wall". Otherwise, there is no means of getting a precise plot. (An approximate method would be to determine what nodes are close to the "line through the wall", extract the temperature of those nodes, and create the plot in Excel.)

John