Warnings on shape violation: influnce on simulation results?

[Patyuchenko]

Hello,

I am performing a thermal simulation of a microchip model. The model was splitted into many simple blocks by vsbw command in order to simplify the meshing process. Each block consists of maximum 3 volumes.

With the meshing of an each following block it becomes much more difficult to mesh it since the model becomes "heavier" (with a lot of elements) and it takes a lot of time to remesh each block several times with different variables of lesize command applied to the lines of a block´s volumes to obtain a mesh with no warnings.

Therefore I am leaving some volumes meshing of which was performed with some warnings and proceed with the next ones. These warnings are mainly as follows:

Tetrahedron element Nr. ... has an angle between adjacent edges of 167 (or less) degrees, which exceeds the warning limit of 165 degrees.

As a rule there are about 70000 elements in each block. I try to obtain not more than 5 warnings per block then I continue with the next one.

What do you think can it have some significant influence on the simulation results?
To which warnings should one pay attention to according to your experience?

Thank you very much.

Best regards

 

[cbrn]

Hi,
unfortunately the reply is not univoque: you may accept or discard strongly-distorted elements, based upon IF they are in a relevant position for your analysis, or not. Since I have an idea of what your model is, I guess that a great part of these elements are near the transition between the chip and the "surrounding", thus they would be "important" for your analysis. On the other hand, I also believe that T dof is less sensitive to elem distorsion (but I may be wrong: I'm not a "thermo-expert").
Have you already tried to adjust "pitch" in LESIZE, so that the lines themselves serve as transition?

Regards

 

[ansysfreak]

Hi

Your element shape are all Tetrahedron?
Why don't you try mesh sweeping the block's?

Grtz
Garry

 

[Patyuchenko]

Thank you very cbrn for your answer.

I am sorry but I did not understand what "pitch" in LESIZE is. What did you mean by "pitch"?

(I use SOLID90 element for the mesh and apply LESIZE in order to define the number of elements for all the lines belonging to a volume.)

Anyway, the thing I am thinking of is can the wrong nodal solution in a nonrelevant part of the model result in a wrong solution in a relevant part? If ANSYS performs calculation of a temperature at each node on the basis of the results obtained for the nodes located in adjacent regions then it can give completely wrong result in a relevant part of the model even if a good mesh is performed there.

Could you give me some advise on the following problem:
the geometry of the model is quite big and it is almost impossible to mesh it directly without subdivision on simple blocks, this is what I did. Each block is easy to mesh. But now I encountered a real problem of lack of physical memory. I know there are many possibilities in ANSYS to optimize calculation process (in my case, I am still meshing my model, therefore I need only temporary memory). Each time I mesh a new block separately, of course all of them are interconnected, but each time I consider only one. When ANSYS creates a mesh for each subsequent block (which is quite fast) after that it tries to process all the meshes of all the previously meshed blocks and this realy takes a lot of time. Do you know is it possible to stop ANSYS doing this each time I mesh a new block of a model? I tried to select everything under the selected volume but it did not help, it still "sees" other meshes and tries to process them.

Thanky you very much.

Regards

 

[Patyuchenko]

I cannot sweep the volumes since they are not homogeneous and their meshes are interdependent.

There are three volumes in each block: the one on the top, the one at the bottom connected with the upper one and the one inside of one of them which is very thin. All of them are glued therefore their meshes depend on each other.

 

[ansysfreak]

Hi

Not if you use contact between the volumes.
Then you can mesh them separate.
Disadvantage: more contact elements.
Can't you use a shell element for the very thin volume?

Gtrz
Garry

 

[Patyuchenko]

Hi,

Thank you Garry for your answer.

By "Not" you meant that it is possible to stop ANSYS "seeing" the previous meshes only if I use contact elements between the volumes or the result for each block will be influenced by the results calculated for the adjacent blocks only if I use contact elements? Sorry for misunderstanding.

I do not use contact elements. Different volumes representing different materials are just glued since it is physicaly a solid semiconductor structure.

Yes, I just used SOLID90 trying to mesh everything with it since it did not seem too complex. I will try to use a SHELL element also. I hope it helps.

Thank you

Regards

Anton

 

[cbrn]

Hi,
1- error propagation: the error due to bad geometry should be local. Anyway, the principal disturb that distortion gives is to the displacement DOFs because of the transfer functions: I do think that for T DOF the bad influence would be limited. Of course, if you're approaching your interest zone with a continuous succession of bad elements, this could be a problem.

2- modeling technique: yeah, very good point Ansysfreak !! Should be the right way: shells for the thin component, solids for the surrounding

3- modeling technique part 2: using "contacts" in order to "join" several volumes: yes, it works, but with some strong issues: the analysis will become non-linear, and the contact elements btw uncoherent meshes will generate results' irregularities at the interface

Regards

 

[Patyuchenko]

Thank you very much cbrn for the detailed answer.

Regards

 

[cbrn]

Hi,
sorry, I forgot to answer to one question of yours: I refered to "pitch" in LESIZE but I mixed up the terms: Ansys calls that "spacing ratio": LESIZE,NL1,SIZE,ANGSIZE,NDIV,SPACE,
where "SPACE" is what I refered to: if >0, it's the ratio btw last division size and first division size; if <0, it's the ratio btw central division size and extremities division size.

Regards

 

[Patyuchenko]

Thank you cbrn. It is clear now.

Regards