I am new on NX nastran Thermal analysis.
I try to analyze a HEA beam (testing the solution type) and have problem with getting results (See picture "No Results").
In .f06 file; I get messages with nr. 3057 og 3007:
*** USER WARNING MESSAGE 3057 (NLITER)
MATRIX IS NOT POSITIVE DEFINITE.
*** SYSTEM FATAL MESSAGE 3007 (NLITER)
ILLEGAL INPUT TO SUBROUTINE NLINIT
The solution is set up like (See picture "Solution-view"):
I chose the material and created mesh for the beam.
Hope you can help me.
Solved! Go to Solution.
Hello Betül Arikan,
first of all, I can't see your picture inside the text.
Here my points to check:
1. What kind of solver and solution did you select?
- NX NASTRAN - SOL 153 Steady State Nonlinear Heat Transfer
- NX NASTRAN - SOL 159 Transient Nonlinear Heat Transfer
- NX Thermal / FLOW
2. Does your material contain all parameters required for heat transfer?
- specific heat,
3. Does your constraints/loads fit to your solution?
I'm not sure, but I think flux does not fit to steady state without another thermal flow constraint like convection or radiation.
4. Do you think you need initial temperature definitions for our part and did you define it?
- I think in transient solution you need initial temperatures.
May be, it helps al little bit to find a solution for your problem.
With best regards
Thanks for your reply!
I do not know why it does not displayed the pictures, but it is same pictures as posted.
1. I used:
Solver: NX Nastran
Analysis type: Thermal
Solution type: SOL 153
2. I chose AISI_310_SS.
Do I need to give the parameters (density, condictivity, specific heat,) for the beam in addition?
3. I changed/reduced the heat flux value (to 0.05 W/mm2) and I get results now.
4. I did not defined initial temperature for my part .
Do you think I need to define the initial temperature in this case?
Hello Betül Arikan,
as you select a steady - state solution I think you don't need initial temperatures if you use constant material parameters.
As you built a solid model with solid elements you have to assign the material in the specific SOLID connector property, as you probably already now.
You use with AISI_310_SS temperature dependent material values which are not defined in the temperature area you have to expect with heavy negative temperature constraints. I think this could be important.
Maybe you should use as a test a manually created material with constant parameters for thermal conductivity as it is the only parameter in AISI_310_SS with temperature dependend values which are important for temperature field analysis.
Additionally you need density and specific heat.
Otherwise you could try to check out the effects of your different loads and constraints in defining
- only temperature constraints with a gradient through component,
- temperature + convection without flux,
Additionally as you have a nonlinear solution slected you could imporve the solution process with nonlinear solution parameters. But if you have constant material values, there is no nonlinearity in model.
That's all for now...
Try and check the influences...
Thank you for the help. It works now.
Now I have some other problems.
Can you answer those, if it is OK for you?
I have tried to drag the temperature under the solution/Loads, but it does not help.
In the solution step is existing force pre-load, not temperatue pre-load.
I think here is a little confusion about temperature load and temperature constraints.
In an Thermal analysis as in "NX NASTRAN => Thermal => SOL 153 Steady State Nonlinear Heat Transfer" the aim is to calculate nodal temperatures and the derived temerature field and gradients across the structure influenced by convection radiation and boundary temperatures. The temperatures values are here the primary solution variables like displacements in a static solution.
Therefore defining temperature values in this case means setting constraints for nodal temperatures. Here you have to define a constraint to fix a special temperature at an certain node.
In a Structural analysis as in "NX NASTRAN => Structural => SOL 101 linear statics" termperature values only descibe temperature differences in comparison to each other and initial values to introduce thermal strains as a result of thermal linear expansion. Here the temperature distribution is a load because the primary solution variable are the nodal displacements. Here you have to define a load set with temperatures to get thermal strains and resulting displacements and by ostruction of them stresses and reaction forces.
Therefore the question is: Where do you try to use temperatures as a load ?
a) in your thermal analysis or
b) in your static analysis?
It does not work in a) but it works in b).
Remember to get thermal strains made of temperature differences in comparison to each other and initial temperature you have to define the thermal expansion coefficient for the desired material.
To get nodal temperatures from a thermal analysis into a static analysis I can describe you my way oing it, I do not know if its best best way, but I know its working (I use NX 8.5.2).
After solving the thermal solution, export all nodal temperatures of your desired Subcase into an ascii file in post processor.
Then switch into your satic solution and import that file as temperature distribution node ID table.
After that your load contains a appropriate temperature value corresponding to your thermal analysis load set for every node of your model .
In comparison to the initial temperature of your static solution and your thermal expansion coefficient in your static solution you will get thermal induced strains, displacements and finally stresses if you obstruct these strains or there are temperature gradients in your nodal load values.
Keep in mind using temperature-dependent material values can make it more dificult to understand your static results.
May be there is a more comfortable way without using "static" ascii files, but I can't say so.
May be you find that better way then tell me.
Try it and tell me your results. Best wishes.
Yes, I am comfused.
I do not understand, if it is not possible to make temperature load in thermal analysis, why we have the feature/option.
Can you explain in detail how you put/mapp result from thermal analysis into static analysis (would like with picture)
Thank you very much!
first short answer.
The opportunity to have both temperature loads ans constraints is founded in the capability of NX CAE to define very different solutions which are defined for most different physical phenomenoms. Thermal analysis and structural analysis are classified in that way differently. And NX CAE is grown over many years. That often means (not only in NX but also in many other computer programs) not everything must be logically :-)
You only have to understand, that temperature constraints are usable in heat transfer solutions (thermal analyses) and temperature loads are for structural analyses.
To define termal results as a load set first try read documentation. i.g.
I've found this from another user dealing with temperature preloads in NX10.