I am trying to create a temperature load with NX Nastran solver - Sol101 Linear statics in NX10. The procedure I took to create the temperature load was as followed:
Loads >> New Load Set >> Temperature Set (Default temperature: 20°C) >> New >> temperature (500°C) >> "Click on surface A (Please refer to the attached "Temperature set.JPG)
I am able to solve this and obtain the stress results. However, when I try to create another temperature load under the temperature set for Surface B, the error "The file D:/......op2 is not found." appears after solving and no results are generated from the solver. May I know if it is possible to create two temperature load from the same temperature set?
I have also tried solving with various solution type such as SOL106, SOL601-106, SOL601-129 and SOL701 to no avail. Furthermore, SOL106, SOL601-129 and SOL701 cannot even provide any solutions for a single temperature load under a temperature set.
May I know if there are any major steps that I have overlooked?
Thank you in advance!
Solved! Go to Solution.
"Result file is in wrong format" is a generic error that post issues when it cannot read a results file cleanly. The root cause is a NX Nastran fatal error that caused the run to terminate (when the run terminated, the .op2 file was not closed cleanly):
*** USER FATAL MESSAGE 4228 (GP3B) TEMPERATURE SET 1 CONTAINS DUPLICATE GRID ID ( 1420 ). *** USER FATAL MESSAGE 4228 (GP3B) TEMPERATURE SET 1 CONTAINS DUPLICATE GRID ID ( 1421 ). *** USER FATAL MESSAGE 4228 (GP3B) TEMPERATURE SET 1 CONTAINS DUPLICATE GRID ID ( 1422 ). *** USER FATAL MESSAGE 4228 (GP3B) TEMPERATURE SET 1 CONTAINS DUPLICATE GRID ID ( 1429 ). *** USER FATAL MESSAGE 4228 (GP3B) TEMPERATURE SET 1 CONTAINS DUPLICATE GRID ID ( 1430 ).
Back to your problem, you cen create multiple temperature loads in a temperature load set, bujt those loads cannot overlap. That is, as long as each temperature load defines temperatures on a unique set of nodes, they can be unioned in the solver. If the temperature on a node is defined in multiple temperature loads, the solver cannot combine the loads.
In your model, the "Tip" load defines a temperature of 500C on one face of the block. The "Side" load defines a temperature of 250C on an adjacent face. The solver cannot determine what you want the temperature load on the shared edge (highlighted orange in the image below) to be - 500 or 250??
To resolve this, edit one or both temperature loads and select the shared edge into the excluded target set so no temperatures will be assigned to the grids on that edge by the temperature load set.
Updated files are attached.
Thank you for providing a solution to my problem.
However, I'm interested to find out more if it is possible to assign different temperature loads to the same elements for solving. The specific problem that I have encountered is that I am unable to assign an additional temperature load to the model in the Mapping Nastran solution. For clarity, this is the procedure I took with the end objective of creating a desired thermal stress profile in mind:
• Transient Thermal analysis via NX Thermal/Flow - Thermal
• Temperature mapping with Output format - " Create Nastran Solution"
• Mapping Nastran
At this Mapping Nastran stage, there will be an temperature set with temperature load created that mapped the temperature distribution obtained from NX Thermal/Flow. From here onwards, I am required to create another temperature load on the same set of elements (i.e. there will be 2 temperature loads assigned to the same element) to obtain my desired stress values. Is it possible to perform this task?
I have chanced upon the case control commands "SUBCOM" and "SYMCOM" that I think may be possible for this scenario. If so, how do I create this command automatically in the preprocessor NX Advanced Simulation?
Thank you in advance!
Multiple structural loads can be applied to nodes and elements because a linear combination of these loads makes physical sense. For example, if you apply a 100N force and a 200N force to a node in the X direction, the resultant is a 300N force in the X direction.
On the other hand, temperatures cannot be linearly combined. What does it mean to apply separate 100C and 200C temperatures on a node? Linearly combining them to get a 300C temperature makes no sense. This is analagous to applying multiple displacement constraints on a grid in a structural analysis. If you place a fixed displacement SPC of 1mm on a grid, then create a second that fixes the same dof at 5mm, what does that mean? What displacement is the solver suppossed to assign to that dof?
If you have multiple different heat sources, boundary conditions (convections, ratiation, etc.), then you need to run a heat transfer analysis first. The results of this analysis will be a temperature field with a single temperature value at each node.