Learning Forum

[helen.durand]

Hello, I am currently working on a one-way transient thermal and transient structural simulation. I am defining temperature dependent material properties in a command object inserted in transient thermal and structural using the MPTEMP and MPDATA commands. 

In transient thermal, when I define the enthalpy (ENTH) material property as the following, I get warnings saying the temperature exceeds the maximum defined temperature, though the simulation still runs:

However, if I add an additional enthalpy data point of 8.4766e+09 for 5000°C, which is the same value as I had for 1600°C, I get the following error:

 *** ERROR ***                           CP =       0.594   TIME= 17:08:12
 Material property ENTH must be input with increasing values as the     
 temperature increases.  The MPDATA command is ignored.       

If ANSYS was just using the enthalpy value of 8.4766e+09 corresponding to 1600°C for all temperatures above 1600°C, it seems like I would not get this error. 

What happens to the enthalpy in the case where I get a warning but the simulation still runs? 

 

ALSO: For thermal conductivity (KXX) I defined a value of 30.5 at 1600°C, and warnings again occur if I go above 1600°C. However, if a I add another thermal conductivity data point of 30.5 at 5000°C, I do not get an error like I do with the enthalpy. It seems like thermal conductivity and enthalpy are being treated differerently.

If I do not include the 5000°C data point, what does ANSYS do for the thermal conductivity? 

 

 

Thank you!

[Gary_S]

We have a Knowledge Material entry for this question:

When temperature-dependent material properties are defined, how does ANSYS determine the material property if the calculated temperature is greater than the maximum temperature defined on the material curve? - Ansys Knowledge

[helen.durand]

Thank you, yes I saw this previously. I guess I was asking for clarification on this issue. 

The reply in that link states: "If the calculated temperature exceeds the highest defined temperature for a temperature dependent material curve, ANSYS uses the maximum defined temperature to determine the material property." 

Say my highest defined enthalpy is 8.4766e+09 corresponding to 1600°C. Is this statement saying that the value of 8.4766e+09 continues to be used for all temperatures above 1600°C?

If so, how come when I enter an additional data point of 8.4766e+09 at 5000°C, I get an error about the enthalpy needing to increase? It seems like the simulation would run the same as before in this case. 

Thank you!

 

 

 

 

[Gary_S]

Hi 

 

Yes, the value of 8.4766e+09 continues to be used for all temperatures above 1600°C?

 

The error is triggered by an identical value. 

Try increasing the last value just a little bit like: 

8.4767e+09 for 5000°C

 

Gary

[helen.durand]

 

Thank you for the suggestion. I have tried doing this in several different simulations using values of enthalpy of 8.47661e+09 or 8.47660001e+09, and I have found that this seems to create convergence issues and results in a different solution (when compared to the case where I do not specify a value for the higher-temperature enthalpy).

Do you know why this might be the case?

Thank you! 

 

[Gary_S]

Can you confirm the material properties are correct by using a single part test model / confirm thermal reactions? 

Also, Is there a reason for defining material data in a Commands object rather than in the Engineering Data GUI?

[helen.durand]

 

The material properties come from other sources, but I think the behavior is independent of the values being used for material properties.

 

I am trying to understand why the following two cases cause different outcomes when running the simulation:

CASE 1: A range of temperature-dependent material properties are defined up to 1600°C. The simulation exceeds 1600°C. Based on a previous reply, the material property value corresponding to 1600°C continues to be used for all higher temperatures. 

CASE 2: The same range of temperature-dependent material properties are defined, except an additional data point is included at 5000°C (the value of the material property at 5000°C is the same or nearly the same as the value used at 1600°C). The simulation has odd behavior when the temperature exceeds 1600°C, including convergence issues and different temperature results.

 

Why is the simulation different between these two cases?

 

I am using command objects to define material properties because it is easier to make changes to material properties (I can just copy and paste a single block of text generated by another code). The GUI can be combersome to change material property data in some cases.

 

[Gary_S]

Hi Helen

Can you rule out an error in the Command object material definition?
Please enter the data above into the Engineering Data application. 

[helen.durand]

 

Thank you for the reply

After some testing, the results are the same regardless of whether the data is entered in Engineering Data or as a command object. 

Adding the extra enthalpy data point still makes a difference. In this case, the highest temperature data point for enthalpy is (temp,enth) = (1600°C , 8.4766e9). If I add another data point of (temp,enth) = (10,000°C , 8.47660000001e9), the results are different (see plot below for an example).

It seems like adding an extra point for the other material properties (C, KXX, or DENS) does not change the results. The issue only occurs with ENTH.

Any thoughts about what is going on? Thanks again for the help!

 

 

ADDITIONAL INFORMATION: a plot of some results from the test simulation. The extra ENTH data point changes the results.

where:

RED: Material properties added using a command object; extra enthalpy data point of (temp,enth) = (10,000°C , 8.47660000001e9) 

BLUE: Material properties added using engineering data; extra enthalpy data point of (temp,enth) = (10,000°C , 8.47660000001e9) 

GREEN: Material properties added using a command object; no extra data point included for the enthalpy data

MAGENTA: Material properties added using engineering data; no extra data point included for the enthalpy data

 

[Gary_S]

 

Hi Helen

For “It seems like adding an extra point for the other material properties (C, KXX, or DENS) does not change the results. The issue only occurs with ENTH.”

I found this in the help which may explain why C seems to have no effect in transient thermal.

3.7. Specific Heat
You can input specific heat effects using either the C (specific heat) or ENTH (enthalpy) property. Enthalpy has units of heat/volume and is the integral of C x DENS over temperature. If both C and ENTH are specified, the program uses ENTH. ENTH should be used only in a transient thermal analysis. For phase-change problems, you must input ENTH as a function of temperature using the MP family of commands (MP, MPTEMP, MPTGEN, and MPDATA).

=====================

Can you try these adjustments and see if you get a converged solution 

Mesh >  Element Order > Set to Linear

Analysis Setings > Nonliner Controls > Line Search > On

 

[helen.durand]

Thank you for the reply! 

I deleted the data for the specific heat (C) and the simulation results are unchanged, so this is in agreement with the statement you included from the ANSYS help. The plot below shows the results for a case with and without the C data. This is useful information but does not seem to be the problem.

The results discussed in the previous post (i.e., the plot of temperature vs time), as well as the plot above in this post, are from converged simulations. Sorry if this was not clear. I was previously having issues with convergence, but I had already enabled line search (as you suggest). I was able to get convergence with quadratic elements.

The issue that remains: The results are different when I include the additional enthalpy data point. Could you please help me understand why this is occurring? 

[Gary_S]

 

According to my colleague, enthalpy is a special case.  For temperatures above the last input temperature, we extrapolate the enthalpy curve at the final slope.  

 

[helen.durand]

Thank you, this is really helpful! I ran a simulation where I extrapolated the enthalpy data point and it is in agreement with you colleague's statement. 

ONE LAST QUESTION: Do you happen to know if there are other material properties that have an exception? 

Specifically:
Instantaneous coefficient of thermal expansion CTEX
Poissons ratio NUXY
When using a temperature-dependent multilinear model TB,PLASTIC,...,...,...,MISO

 

[Gary_S]

Hi Helen

 

Enthalpy is the only quantity that is the integral of a material property.  

The only documention regarding extrapolation and enthalpy is here: 

Considerations for Enthalpy (TBOPT = ENTH)
To ensure correct results, you must define enthalpy over a large enough temperature range to span all computed temperatures during the solution. The TB command does not extrapolate enthalpy values beyond the specified temp range like the MP command does.

If both the TB and MP commands are used to specify enthalpy values, enthalpy values defined via the TB command are used and those defined via the MP command are ignored.