I am currently using NX 10. I have noticed that the Nastran Temperature Pre-load feature is missing in the Solution Step as compared to older NX versions. May I know if this feature has been removed or has it been relabelled as another function?
Solved! Go to Solution.
Prior to NX 10, temperature specification was spread out over 7 different areas:
On Export, temperatures in all 3 TEMP(LOAD) are globbed into one SID. Temperatures in both TEMP(INIT) are globbed into a second SID. Temperatures in both TEMP(MATERIAL) are globbed into a third SID
This was all cleaned up in NX 10. All temperature specification is now done via a Temperature Set:
A Temperature Set definition consists of a type (Initial, Load, Material), a label, a description and a default temperature value:
The Type and Label correspond directly to the case control entry (i.e. TEMP(INIT)=1 or TEMP(LOAD)=101). The default temperature becomes the bulk data TEMPD card for that SID.
Once the set is created, multiple temperature loads can be added to the set.
All temperature loads are defined via a single Temperature Load dialog
Thanks for the explaination.
But I have a question.
In NX5 (yes long ago ) I tesedt a temperature load on a beam
clamped in both ends, so I could verify the stresses with the
coefficients with thermal expansion.
The only thing I had to do (if i recall correctly) was put on a temperature load
eg 300 degrees and define somewhere the normal temperature.
I would like to do this again in NX10 (OK first a metal and then a Laminate).
But I am confused of the possible options nowadays and the temperature
seems not to appear as a load in the navigator.
What I want is to indicate that the stress free state temperature is 20 degrees
and that the current temperature is 200 degrees.
Thanks for your time,
First, it's generally not good forum etiquette to reopen a 9 month old thread. In the future, create a new post and reference the old one if needed.
Second, I'm not sure I can post a more detailed reply now than the one posted last year. If you want to specify an isothermal temperature difference, you simply need to create a temperature set of type Initial/Stress Free and set the default temperature value of that set to T1. Then create a second temperature set of type Load and set the default temperature value of that set to T2. Your delta T will then be T2-T1.