I trying to find out the best workflow when applying a temperature distribution (solved in SOL153) to a SOL101 solution as a temperature load. I am using NX10. I struggeling to find other threads that explains in detail how use the approriate workflow.
The way I have done it now is as follows:
1. Solve thermal SOL153 to get the temperature distribution on the geometry. I plot temperature results, select all the nodes with temperature using "identify result" and export this information to a file.
2. In SOL101 I define the following:
* Temperature set - Initial/stree free (22C)
* Temperature set - Temperature load (Default temperature 22C) - This is found in subcase
In the "temperature load" I create a new temperature where I choose "new field" -> table. I choose the appropriate coordinate system and import the file created in SOL153. This will create a temperature load on all the nodes seleceted in SOL153. This works just fine in small models....
Is there any problem with this approach? There is, however, one frustrating part. When working with large models I takes very long time to use this approach. Selecting of all the nodes takes forever.....I really hope there is a better approach to apply temperature distribution as load in SOL101?
I noticed that in previous releases there was something named "temperature pre-load" as input to the subcase. I understand this is now removed? Is there someting similar in NX10?
The temperature pre-load capability was replaced with a new type to the temperature load. This new type is called "Temperature - External Time Unassigned". So in your linear statics solution you will:
1. Go to a subcase and create or drag a temperature load set into the loads container
2. Create a temperature in the temperature load set
3. Define the temperature type as Temperature - External Time Unassigned
4. Set the file type to be Nastran Temperatures
5. Select the results file from your SOL 153 analysis
You can also select other types of files such as BUN from NX Thermal, Abaqus, or Ansys results files.
Simulation Product Management
Simulation and Test Solutions
Siemens Industry Sector
Siemens Product Lifecycle Management Software Inc.
Thank you!! However, a small question
1. When using this approach, are there any limitations to different mesh sizes? For example: Using the same model (of course) for SOL153 and SOL101 but the mesh on model in SOL153 and SOL101 are not the same. In SOL101 some areas will have finer/better mesh. Anything to watch out for? Will the temperature be interpolated over the new nodes?
If the meshes are different, you have to stick with fields. Using results files assumes that the meshes are the same. That was the case with the old pre-load capability too. So, you are back where you started.
Hello Mark and Tok,
allthough it's not my thread, I have a question for that case, too and I hope, some body can answer it.
Do only elements and gridpoints have to be the same or simulation objects like contacts or gluings too?
If I am right, gluings represent some type of heat transition too, in default setting a perfect heat conductor.
Is there a problem if in SOL153 (heat transfer) the connection between two bodies is a surface-to-surface-gluing for describing a perfect conductor and in SOL101 (Linear Static) its a surface-to-surface-contact?
What about rigid elements (RBE2) and interpolation elements (RBE3), can I switch between them?
Best wishes, Michael
I gave the method a try and this a much simpler work flow. Proper planing when creating the FEM models will save time.
It was an interesting question (about RBE2 and RBE3) elements. I have an additional question about SOL153. As far as I understand there is not a "edge to surface" gluing available. I tend to use 3D shell whenever I can to reduce solving time and would like to use the same model for SOL101 and SOL153.
How can I "connect" solid and and shell in SOL153. Is it possible? For example I assign a temperature on a shell (sheet) and this will conduct temperature to get a temperature field across the sheet and solid body.
Edge-Face glue is supported in SOL 153/159. In heat transfer solutions, glue is treated as a conductance, not a stiffness.
See BGSET Remark 2 and BGPARM Remark 2, which explains how the conductances are defined.