I have done a static analysis of the quick opening of a pressure vessel using two different material approach.
in the first one all the material properties are set at the design temperature (250 °C): i.e. Youngs modulus and expansion coefficient are set at the appropriate values;
in the second one I have used functions vs. temperature to define Youngs modulus and expansion coefficient, and I have add a body load activated at the default temperature (250 °C).
I think the results have to be quite similar, but with great surprise they are different!
In the second analysis Femap stop (without errors) in a few time after 1 or 2 iteration and don't seems to keep togeter the parts glued (the teeth of the mating flanges are meshed with different approach hex and tetra);
In the first Femac required a lot of iteration and hours for the result, but I don't unterstand why, if it is my error or Femap limit. Many thank in advance for any help!
I have changed the function to define Youngs modulus from "vs. Temperature (2)" to "vs. Temp (TABLEM1 Linear, Linear) (19)" and I have put constant the expansion coefficient to semplify the problem, but again results are different from those obtained from the first solution where all the material properties are set at the design temperature (250 °C)
Nobody can help me?
I think the problem is to set Femap to translate correctly the material properties to Nastran
I suggest to prepare a pilot study using a simply model with a few elements that replicate the real problem, and post here the FEMAP model, this way we will be able to help you for sure!.
This is the simplified model with connections contact and glued types, glued connections are used to joint tetra and hex parts (in the true model I cannot Hexmesh all parts). In this case Femap do a lot iterations but the result is very strange and the glued parts do not seem joined together. In this case Joungs modulus of the material are "vs. Temp (TABLEM1 Linear, Linear) (19)" .
The next picture are results from the same model, load, scale, etc., but with Joungs modulus of the material set at the proper value at 250 °C.
Many thank in advance and if is needed a more semplified model tell me.
When enter a function ID#1 for Young module where ID#1 is a temperature dependant function then GLUE/CONTACT is not working properly, a value of 1.0 is used to derive the stiffness of GLUE/CONTACT connection instead the derived value from the temperature dependent property data.
Workaround: in the GENERAL tab of the material property enter the nominal value for Youngs module, ie, 210e3 MPa, and associate data under FUNCTION REFERENCE tab to a function vs. Temperature where a relative valued is used, not absolute.
I have modified the temperature dependant function and run again my model, but without results! It take a lot of time and don't seem to converge (more than 20 hours for only 13 iterations).
So I have ran the test model I have done, again it not converge after 40 iteration even if it was near to converge, but results are without significance. The only good news is that now glued and contact parts seems to work properly. A few minutes ago my Femap support said my that this is a software bug and that will be resolved in a next patch.
Best Regards and many thanks also