How to read temperature at an integration point?

[biblo]

Hi everybody.
In my program, I need to know, at every time, the temperature’s value of every integration point of the elements. Is there a command of Ansys which enables us to read the temperature at a given integration point?
Thanks in advance
Barha

 

[bfillery]

Dear biblo

My understanding is that temperature is a degree of freedom (DOF), therefore, temperature values are output at the element nodes, not the integration points. Therefore, you should be able to request the field output from the nodal solution to view the temperatures at the nodes. If you wish to interpolate the nodal temperature to the integration points, you will need to map the nodal values to the desired points.

bfillery

 

[biblo]

Dear bfillery,
Yes the temperatures output is at the nodes but, i think that the calculation of them is done initially in the integrations points then they are extrapolated to the nodes.
Now if one uses these temperatures as loading in a structural analysis, and if for example the Young modulus (EX) depends on the temperature, calculation of the stresses, for example, is made at each integration point of the element with a different value of EX (if temperatures at each integration points are different). I would like to be able to interfere in Ansys calculation to assign the value of EX to each point of integration like i want. Is this possible??!?!

 

[bfillery]

Dear Biblo

If I understand your problem, you want to model a temperature dependent analysis where the Young's Modulus is the temperature dependent variable. If this is the case, then if you can either reconstruct the required temperature fields by a thermal analysis or if you know the temperature fields in advance, assign them as an initial field, then an input of a temperature dependent Young Modulus should do the job. Keep in mind the Youngs Modulus will be linearly interpolated between specified temperatures.

bfillery

 

[biblo]

Hi bfillery,
sorry for the delay. In fact, I make a thermal analysis to obtain the transient field of temperature. These temperatures will then be applied as load in a structural analysis for studying, for example the variation of the stresses state in the component. The mechanical properties of my material depend on the temperature. I must check, Instantaneously, the temperature of each element to assign to him the corresponding curves of the properties (for example: EX, NUXY, Sy,….). I can’t do that in advance because that is not useful.I must do that at the moment of the change. My program goes very well… except that I could improve it if I could find a means of introducing a curve for each point of integration and not for the entire element (by an average temperature). I know I am explained very badly, it is that I don’t write well English and my program is rather difficult to explain.
regards,
Barha

 

[cbrn]

Hi,
I don't understand your statement:
"I can not do it in advance because it's not useful".
If you have temperature-dependent material properties, then why not define temperature-dependent material properties in the Material Models ???
Then Ansys would give you the solution where, at each integration point, at each substep (or iteration), the mat props are exactly those needed for the temperature in this point (or, better said, caused by this temperature), without any need to directly access the calculation data...
Am I missing something?

Regards

 

[biblo]

Hi,
Look CBRN, if you can answer this question, it will be more easier for me to explain what I said before:

Suppose that:

MPTEMP,,20,100,200,300,400,500
MPDATA,EX,1,,200e9, 189e9, 170e9, 160e9, 150e9, 140e9

So, when the temperature is for example = 200, Ansys gives EX a value of 170e9. The question is: 200 is the temperature of what? Average temperature or what?
Suppose that the temperatures at the element nodes are different, does Ansys check the temperature at each integration point and then give to this point the corresponding value of EX (in this case we can have more than one value of EX for the same element at the same time!!!)

 

[cbrn]

Hi,
if I recall the foundamental "law" of dynamics used in FEM, we have [M]{x"}+[D]{x'}+[K]{x}={F} applied for every integration point. Results at nodes are always calculated based upon the Gaussian points (integration points), through the Transfer Functions (or Element Shape Functions). So, the "basis" results are always at the integration points. The Young's Modulus and Poisson Coefficient are both involved in the stiffness matrix. So, the material's constitutive laws serve to calculate [K] coefficients for all the generalized DOFS.
Based upon this, I believe that you already have what you need by defining temperature-dependent material properties. When you ask for an "element result", in fact, there is a double interpolation: gaussians to nodes, and through-nodes (that's why, for example, an "element result" showed as contours shows faceted appearance, since the value is one-and-only for each element where, instead, the value is of course different on each node and on each gaussian).
But, in order to be 100% sure, you'd better look in the Theory Manual for the element type you are using (it COULD be that, for simplicity's sake, the same MP value is applied through all the nodes of an element, though I don't think so...).

Hope this helps and that I'm not in the wrong direction...

Regards

 

[biblo]

Thank you CBRN for this very instructive answer.
I make a thermal analysis to have the temperatures at nodes. I apply these temperatures as loading in a structural analysis. I declare for example that:
MPTEMP, 20,100,200,300,400,500
MPDATA, EX, 1, 200e9, 189e9, 170e9, 160e9, 150e9, 140e9
However, this curve of EX values is valid only if the element is in the heating stage (there are other conditions which it not necessary to cited here). I must thus to check, at each step of calculation the average temperature of the element to see whether it cools or not. If it cools I assign to him, with MPCHG command, a new material which contains a different EX curve (a curve of cooling). The use of the average temperature is only an approximation. Best is to be able to check the temperature at each integration point and not the average. But according to your answer CBRN it is apparently impossible!! Do you have another idea?
Regards
Barha

 

[pja]

In your thermal analysis the temperatures are field variables and therefore are computed at the nodes only. If you know the shape functions used in your thermal analysis you can easily use the nodal values of temperature to compute the temperature at any point inside the element..ie at the integration points.

For example if your element uses bi-linear interpolation to find the temperature at the point x1,y1 you would do
T(x1,y1)= T1*N1(x1,y1)+T2*N2(x1,y1)+T3*N3(x1,y1)+T4*N4(x1,y1)
where N1-N1 are the bilinear shape functions and T1-T4 are the nodal values of temperature.

 

[cbrn]

Hi,
yes, pja's method is great and this is what, implicitly, ANSYS' manual suggests.
However, there are also two other possibilities:
- have ANSYS report values at the integration points (report listings only), via the KEYOPTs of the element (if available)
- force ANSYS to copy the gaussian resulta to the nodes, without interpolation: ERESX,NO

Regards

 

[pja]

If temperature are the element dof, then results for them at the integration points are not available..this is equivalent to asking for displacements at integration points for a structural element..can't do it. The only way to do this is to postprocess the nodal results. ERESX has an effect on derived results(stresses,strains,etc) only..same for any KEYOPTS an element might have.

 

[cbrn]

Hi,
Pja, you're right. I made a mistake...

So, it shouldn't be so difficult to achieve the goal, although not very immediate, since Ansys Theory Manual reports the theory underlying every element type, so for example if you find that an elem is a Lagrangian hex, in any FEM book (or perhaps even in the A.T.M.) you can find the shape functions...

Regards

 

[biblo]

Thank you CBRN and PJA for this great informations… I try to use them in this moment….but the second part of my question remains unanswered!!. If I can read the temperature at a node (or at a point of integration) and that its value implies the use of material 2 how to force Ansys to use material 2 instead of 1 in this point.

Barha

 

[cbrn]

Hi,
1- nodal results vs integration points results: I thought again about this and perhaps we have "a bit" deviated: in fact, as the generalized DOFs are computed at the nodes and temperature is a generalized DOF for thermo-structural elements, as Pja points out, then the correct point where to compute the temperature-dependent material properties seems the node and not the integration point !!! In fact, both structural DOFs (displacements) and thermal one (temperature) are evaluated there; Afterwards, the derived results will be determined at the integration points (these are stresses, strains, thermal gradients, fluxes...) and re-transfered to the nodes (or not, depending on the ERESX setting) by the program itself... I presume this is the overall-correct way to interprete all the calculation process
2- Ah, yes, we forgot that... It's a problem, since a same element can't have different material properties at each node! It woul be like saying that a 1x1 sq.in. piece of material is rubber at one corner, steel at one other, paper at the third and wood at the fourth...
So the moral would most probably be: the way you used to compute was foundamentally correct: average on the element; if you aren't satisfied of the results in one area (for ex. because there are strong thermal gradients), then simply... refine the mesh !!! ;-)

Regards

 

[biblo]

Hi,
It is what I do CBRN, I refine the mesh....but I cannot go very far because the computing time should not be also very big!! Also if I use a variable mesh I encounter problems of convergences.....
We still don’t know what do ANSYS when the temperatures at the nodes (or the points of integrations) are different. Does it take the average temperature to assign the value of EX (for example) to the element? Or it assigns at each point a different EX according to its temperature!!!!!!!!!!

 

[cbrn]

it assigns a different EX according to the temperature. But it will always be the EX-vs-TEMP law of the material the element has been given.

Your problem is when the temperature "slope" changes its sign, i.e. when you have to shift from one MP law to another, because two laws are not allowed for the same MatProp of the same MatType.

I don't really know how to get out from this problem...

 

[biblo]

I believe that the best solution for the moment remains that which I do: to apply at nodes the same temperature (which is their average temperature) and if it proves that the element cools in comparison with the preceding step, then to assign to him a new material (with MPCHG). To have a better approximation I have to make a more fine mesh. Thanks’ CBRN and PJA for your invaluable help and your very instructive information.

Regardsssssssssssssssssssss
Barha

 

[SKJoe]

Hi,

I have one experience with integration points as follows :
I tried to include initial stresses to my nolin static analyse. Obvious procedure is that first you solve thermal analyse and in solution phase you turn on to write initial stresses. ansys create a file with IST suffix. The file.ist is used subsequently in static analyse. I tried to open the file.ist in text editor and realized that there were written 12 values for each element. It means one value for each integation point of each element (I used shell181 full integation - it means 4 points over element and 3 points through the thickness of shell. 4*3=12).

So if it is true that you can aplly dof only to nodes, why the file.ist contains values for integration points ?

Regards,
Lubo

 

[pja]

Once again, DERIVED RESULTS are computed at integration points. I believe the main reason for this is that in the course of integrating the element stiffness matrices, the B matrices, which directly relate strains to displacements, are computed at integration points, hence strains(and therefore stresses) are available at these points.

I doubt the IST file had the element FIELD VARIABLES reported at integration points.