I am new on NX CAE Thermal cases. I have the next case, I want to study thermal expansion
of a part, is a convection case (air) and the temperature goes from 20 Celsius to 50 Celsius.
The parts is standart steel.
Which kind of boundaries, must be used on NX CAE for this case?
Thanks, in advance.
Solved! Go to Solution.
You will need to do this in 2 parts. First, the thermal boundary conditions (convections and temperature constraints) are applied an a thermal solution is run. this can be NX Nastran SOL 153, 159 or NX Thermal. The output of this solution is a temperature distribution.
This temperature distribution is then applied as a load in a structural solution (i.e. NX Nastran SOL 101). The structural solution then calculates the thermal strains.
I am currently dealing with the same issue here and my problem is that even the simplest example in SOL 153 does not work. What I did: I made a box, mesh it with tetra elements (I tried tet4 and tet10 with same result) Applied database material Steel, Added fixed temperature (50 deg) on one face and heat flux (10 W/mm2) on the oposite one. The model is saying it is using SOL 153, NX Nastran in thermal setting. It has by default the inicialization temperature of 20 deg predefined
But the result is 13 WARNINGS and 1 FATAL
With the first warning message:
TABLE LOOK-UP ON TABLE ID 1 FOR MATERIAL ID 2 RESULTS IN A
NEGATIVE VALUE OF A MATERIAL PROPERTY FOR ELEMENT ID = 12 .
THIS MATERIAL PROPERTY WILL BE SET TO 0.0 .
USER ACTION: MAKE SURE THE TABLE CANNOT RETURN NEGATIVE VALUES BY INTERPOLATION OR BY EXTRAPOLATION.
And first error:
*** STOPPED PROBLEM DUE TO FAILED CONVERGENCE
What could be wrong here? Any ideas? Thanks a lot for any hint,
A pro po,
that means that this calculation also includes using result of one analysis as an input for another one... is there a tutorial, or a discussion thread dealig with this?
Your material has temperature dependent modulus data as shown below. The blue portion of the curve is the data defined in your input deck for temperatures between 20 and 704. In NXN 8.5 and prior, Nastran always extrapolates table data if a lookup value falls outside of the domain of the table. The red portion of the curve shows the extrapolation out to T=2000:
In NXN 9, an option was added to table definitions to disable the extrapolation and simply use the last defined value for any points outside of the table. Setting this option and running in NXN 10 yields the following results:
Your heat load on that face is set to a (very large) 10 W/mm^2. This results in a temperature of almost 2900 degrees on the loaded face. This is way past the point where the extrapolated modulus becomes 0 (which is at approximately 1600 degrees).
Your choices include:
I was not thinking about the logic of the applied loads... now even the Warning mesage make sence.
Now to the second part I found a video tutorial in the NX documentation, how to map the result of one simulation as a BC to another one:
In the NX library in your installation: UGDOC\html_files\nx_help\en_US\graphics\graphicLib
I found it putting this to the "search line" of the html manual: "Base model on results".
Note that the mapping is only required if your structural mesh is different than your thermal mesh. If the same mesh is used, you can specify THERMAL(PUNCH)=ALL in the SOL 153 run and Nastran will write the appropriate TEMP cards to the punch file.
In NX 8.5, these temperatures can be applied using the Temperature Preload option on the subcase:
I want to create a case study on NX CAE like this one first case as you say. I have to use NX Thermal or (SOL 153) afther this run, I have to use static case (SOL 101). How can I put two temperatures between 20 Celsius and 50 Celsius. Attached an example case video, about my case. I am using NX9.0.2