Why does OptiStruct result differ greatly from those of ANSYS?
Altair EmployeeHi all,
I want to compare the result of shell and solid element for a thin plate bending analysis. So I select a thin plate with dimension 100*100*2mm, the four edge of the plate are all clamped, and a uniform pressure is applied on the top surface.
However, I got a different result from OptiStruct and Ansys with the same solid model. Both the material and the mesh are the same. The in-plane element size is 1.25*1.25mm, and there are two elements through its thickness. The maximum stress in X direction from OptiStruct and Ansys is 74.4MPa and 158.7MPa. It's so different. What's more, according to the theory, the maximum stress may be 154MPa, which makes me suspect the optistruct result.
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
The maximum stress theory for four clamped thin plate under uniform pressure loading is given in following link
http://www.roymech.co.uk/Useful_Tables/Mechanics/Plates.html
What's the reason for this strange result? I have attached my HM file.
In addition, is there any document which explain the different options meaning of stress result type and average method? See figure below
Thank you
Roy
Answers
-
Hi Roy,
Can you share the model file please?
The above post does not have any attachments.
0 -
Altair Forum User said:
Hi Roy,
Can you share the model file please?
The above post does not have any attachments.
I'm sorry. I forgot it.
0 -
Roy,
Thank you, what is the magnitude of pressure applied?
I see the result is 74Units. Also can you share the Ansys deck?
0 -
Altair Forum User said:
Roy,
Thank you, what is the magnitude of pressure applied?
The magnitude of the pressure is 0.2MPa. You can check it from my model file.
When only one element through the plate thickness, the OptiStruct result is very small. I don't know what's the reason.
What's more, In many literature mentions if the solid element was used for thin plate, there must be at least three elements through the thickness, how to understand this statements?
Thank you
Roy
0 -
Roy,
To capture bending effects it is neccessary to have more than 2 rows of elements when using solid element type.
0 -
Altair Forum User said:
Roy,
To capture bending effects it is neccessary to have more than 2 rows of elements when using solid element type.
Hi Prakash,
I have uploaded my Ansys file in my previous reply.
1. Why should more than 2 elements be used for solid? How to understand?
2. I used the same model with Ansys and OptiStruct. That is to say, in Ansys, the elements through the plate thickness is also two. Why they give so different results?
Thank you
Roy
0 -
I wonder why ansys can capture it with only 2 layers. Does it have a better elem formulation than optistruct?
0 -
In your model 'SolidCompare.hm' you do analysis with solid & shell elements at the same time?
Your solid plate has 2mm thickness and your shell has also 2mm of thickness ???
0 -
Altair Forum User said:
In your model 'SolidCompare.hm' you do analysis with solid & shell elements at the same time?
Your solid plate has 2mm thickness and your shell has also 2mm of thickness ???
Hi Q.Nguyen-Dai,
I'm sorry I didn't make it clear. I calculate the same problem with shell or solid elements. This is the different case. When using solid element, the shell element is hided and only display components is calculated. Please see the .fem file. You can run the model to validate it.
Thank you
Roy
0 -
Altair Forum User said:
I wonder why ansys can capture it with only 2 layers. Does it have a better elem formulation than optistruct?
Could be... I think Ansys supports thin solids and Roy is using the same for modelling.
The same is not supported yet in OptiStruct
0 -
Practically, you have to have at least 3-4 elements on thickness for solid meshing.
Firstly, try to compare the nodal displacements. Then try to compare the equivalent von Mises stress.
For stress tensor, be careful about local element axis.
REMEMBER: in FEA, the nodal displacement is exact solution. Whereas element stress is interpolated.
0 -
Here're SAMCEF's results for shell analysis.
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
Altair Forum User said:
Practically, you have to have at least 3-4 elements on thickness for solid meshing.
Firstly, try to compare the nodal displacements. Then try to compare the equivalent von Mises stress.
For stress tensor, be careful about local element axis.
REMEMBER: in FEA, the nodal displacement is exact solution. Whereas element stress is interpolated.
Hi Q.Nguyen-Dai,
Thank you for your reply.
I have compared the deformation and it seemed ok. However, large different results were gotten for stress with different solver by using solid element. The results were summarized in the following table. In addition, the attachment pdf file gives a more detailed summary results.
<?xml version="1.0" encoding="UTF-8"?>
In the attachment, I also listed my main doubts. Could you show your understanding? Thank you.
1. Why different stress results were gotten by solving the same solid model with OptiStruct and Ansys?
2. How to understand a saying “At least three elements must be used when simulating thin plate with solid elements”? What’s the theory in the background?
3. How to compare the FEA stress result with that of theory? I think the directional stress should be used, do you think so?
4. How to output Top or Bottom stress results for shell element model in OptiStruct?
5. Is there any document which explain the different options meaning of stress result type and average method in HyperView?
Best Wishes
Roy
0 -
Altair Forum User said:
Could be... I think Ansys supports thin solids and Roy is using the same for modelling.
The same is not supported yet in OptiStruct
Hi Prakash,
I have summarized my simulation results in the following table. And a detail message you can go through the attachment.
<?xml version="1.0" encoding="UTF-8"?>
In the attachment, I also listed my main doubts. Could you show your understanding? Thank you.
1. Why different stress results were gotten by solving the same solid model with OptiStruct and Ansys?
2. How to understand a saying “At least three elements must be used when simulating thin plate with solid elements”? What’s the theory in the background?
3. How to compare the FEA stress result with that of theory? I think the directional stress should be used, do you think so?
4. How to output Top or Bottom stress results for shell element model in OptiStruct?
5. Is there any document which explain the different options meaning of stress result type and average method in HyperView?
Best Wishes
Roy
0 -
Here're my tests with SAMCEF & HEXA20 (2nd order) elements
3 elems/thickness
<?xml version="1.0" encoding="UTF-8"?>
4 elems/thickness
<?xml version="1.0" encoding="UTF-8"?>
5 elems/thickness
<?xml version="1.0" encoding="UTF-8"?>
For displacements: Good results even with few elements/thickness.
For equivalent stress:
3 elems/thickness
<?xml version="1.0" encoding="UTF-8"?>
4 elems/thickness
<?xml version="1.0" encoding="UTF-8"?>
5 elems/thickness
<?xml version="1.0" encoding="UTF-8"?>
For stress: A lot of elems/thickness to got the same result as shell model.
0 -
Hi Q.Nguyen-Dai,
Thank you for the validation.
As you concluded, the deformation result was close to the shell model even few elements through thickness was used. However, when comparing stress results, we can find that the solid model is a lot different from shell model even lots of elements through thickness and 2nd order elements was used.
(From your result, the maximum stress of solid element with 5 elems/thickness is 99MPa (2nd order element), but the maximum stress from shell model is 129.5MPa)
I think the solid model with 3 elems/thickness cannot give a good result when comparing with shell model. At first, I think may be the stress result converges when 3 or more elements is used through thickness. However, this simple example seems to deny this conclusion.
So how to understand the saying “At least three elements must be used when simulating thin plate with solid elements”? What’s the theory in the background? And why so different results were gotten with different solvers by using the same model?
Best Wishes
Roy
0 -
Hi,
My results show only the evolution of equivalent stress depending the element number over thickness.
In reality, if you would like to have good FEA results, you have to refine your mesh belong another dimensions too, not only thickness direction.
0 -
Here's another test with HEXA20 in SAMCEF: 10 elems/thickness !!!
<?xml version="1.0" encoding="UTF-8"?>
In attachment, you have also H3D () results for equivalent stress.
Remember that you can do everything with SOLID elements, but you can not do everything with SHELL elements.
When the real behavior of your structure is close to Shell theory, you get good enough results. In your current case, bigger thickness could give your 'bad' results with Shell analysis.
0 -
Altair Forum User said:
Remember that you can do everything with SOLID elements, but you can not do everything with SHELL elements.
When the real behavior of your structure is close to Shell theory, you get good enough results. In your current case, bigger thickness could give your 'bad' results with Shell analysis.
I agree. At the same time solid elements may not give better results with lesser thickness due to locking problems with bending in linear approximation. Not sure what element type is Ansys using and their formulation.
0 -
Don't we have reduced solid formulation in Optistruct? I heard it can eliminate locking.
0 -
Altair Forum User said:
Here's another test with HEXA20 in SAMCEF: 10 elems/thickness !!!
In attachment, you have also H3D () results for equivalent stress.
Remember that you can do everything with SOLID elements, but you can not do everything with SHELL elements.
When the real behavior of your structure is close to Shell theory, you get good enough results. In your current case, bigger thickness could give your 'bad' results with Shell analysis.
Hi Q.Nguyen-Dai,
I don't think I have gotten your opinion. Do you mean my example (a=b=100mm, t=2mm) is beyond the application of shell theory? However, from the theory, I think my example is in the application of shell theory because the thickness ratio is less than 10% and the deformation is also in the small displacement range.
Why we get so different result from Ansys and OptiStruct with the same model? And why is the saying “At least three elements must be used when simulating thin plate with solid elements”?
Best Wishes
Roy
0 -
Altair Forum User said:
I agree. At the same time solid elements may not give better results with lesser thickness due to locking problems with bending in linear approximation. Not sure what element type is Ansys using and their formulation.
Hi Prakash,
I still have not understand the following questions.
What is locking problem? Why we get so different result from Ansys and OptiStruct with the same model? And why is the saying “At least three elements must be used when simulating thin plate with solid elements”?
Best Wishes
Roy
0 -
Altair Forum User said:
Hi Q.Nguyen-Dai,
I don't think I have gotten your opinion. Do you mean my example (a=b=100mm, t=2mm) is beyond the application of shell theory? However, from the theory, I think my example is in the application of shell theory because the thickness ratio is less than 10% and the deformation is also in the small displacement range.
Why we get so different result from Ansys and OptiStruct with the same model? And why is the saying “At least three elements must be used when simulating thin plate with solid elements”?
Best Wishes
Roy
No, I don't say your example is 'bad' for SHELL analysis. But I'm sure that another plate 100x100x1 will give better results with Shell.
We are in 'approximate world' with FEA. Only you can judge about accuracy of your work.
0 -
Altair Forum User said:
Don't we have reduced solid formulation in Optistruct? I heard it can eliminate locking.
Hi tinh,
How do you understand my doubts in the following attachment?
Best Wishes
Roy
0 -
Altair Forum User said:
No, I don't say your example is 'bad' for SHELL analysis. But I'm sure that another plate 100x100x1 will give better results with Shell.
We are in 'approximate world' with FEA. Only you can judge about accuracy of your work.
Hi Q.Nguyen-Dai,
Yes I agree. We are in 'approximate word' with FEA. My simple example have theory solutions. You can look for the result in any book or paper about theory of plate. The following link also give the theory solution. (the theory max stress is 154MPa)
http://www.roymech.co.uk/Useful_Tables/Mechanics/Plates.html
So what's your understanding of the following questions:
Why we get so different result from Ansys and OptiStruct with the same model?
And why is the saying “At least three elements must be used when simulating thin plate with solid elements”?
Thank you
Roy
0 -
Altair Forum User said:
Don't we have reduced solid formulation in Optistruct? I heard it can eliminate locking.
TInh,
I need to check if there a way to eleminate locking with 2 layers
Maybe Ansys is using a different element formulation which OptiStruct does not support yet. If I can have the Ansys .cdb file for the same model I can check with experts
0 -
Altair Forum User said:
Hi tinh,
How do you understand my doubts in the following attachment?
Best Wishes
Roy
I saw the displacement results are similar, just stress is different. I think it is because stress is not output at outer position.
Enter panel analysis>control cards>GLOBAL OUTPUT REQUEST, slide down to activate 'STRESS' and select 'LOCATION' as 'ALL'
Run anaylysis again and open Hyperview>Contour> select stress result and activate 'Use corner data'
The max stress values are 133 and 143(XX) , I think they are comparable with ansys
0 -
Altair Forum User said:
I saw the displacement results are similar, just stress is different. I think it is because stress is not output at outer position.
Enter panel analysis>control cards>GLOBAL OUTPUT REQUEST, slide down to activate 'STRESS' and select 'LOCATION' as 'ALL'
Run anaylysis again and open Hyperview>Contour> select stress result and activate 'Use corner data'
The max stress values are 133 and 143(XX) , I think they are comparable with ansys
<?xml version="1.0" encoding="UTF-8"?>
I didn't think about this
/emoticons/default_smile.png' srcset='/emoticons/smile@2x.png 2x' title=':)' width='20'>
Still I am curious to know the element type used in Ansys.
0 -
Altair Forum User said:
I saw the displacement results are similar, just stress is different. I think it is because stress is not output at outer position.
Enter panel analysis>control cards>GLOBAL OUTPUT REQUEST, slide down to activate 'STRESS' and select 'LOCATION' as 'ALL'
Run anaylysis again and open Hyperview>Contour> select stress result and activate 'Use corner data'
The max stress values are 133 and 143(XX) , I think they are comparable with ansys
Hi tinh and Prakash,
What's the meaning of 'Use Corner Data'? If the Global output request is default, which stress output, element stress in the integration points or node stress or average stress?
I also have doubts about stress output meaning in HyperView. For shell model, I think maybe top or bottom stress can be output, however it seems this can not be done in the HyperView. Is there any help manual about the meaning of this results options?
Best Wishes
Roy
0 -
Altair Forum User said:
I didn't think about this
Still I am curious to know the element type used in Ansys.
Hi Prakash,
Maybe we can output APDL input file from workbench by using Tools--Write input file. I have output from my model, and please check it in the attachment.
From the dat file, the element in workbench solid model is SOLID186 and full integration is used.
I think this element type is a very common second order solid elements. Does OptiStruct have this type elements? How to define it?
Best Wishes
Roy
0
