Jump to content
Sign in to follow this  
Roy Duan

Why does OptiStruct result differ greatly from those of ANSYS?

Recommended Posts

Hi 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.

59ba6ad00c4a8_OptiStructStaticResult.thumb.JPG.a49dc9cde93873ad670f26569d59b608.JPG59ba6ad6372bb_AnsysStaticResult.thumb.JPG.4ea8bce2a64f798d9bcf5c93c1983b10.JPG

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

2017-09-14_195741.png.54828a59e3a5717fbd08cd3573849c10.png

 

Thank you

Roy

Shell_Solid.zip

ShellSolidCompare.hm

ShellSolidCompare.fem

Edited by Roy Duan

Share this post


Link to post
Share on other sites
Guest

Roy,

 

Thank you, what is the magnitude of pressure applied?

 

I see the result is 74Units. Also can you share the Ansys deck?

 

Share this post


Link to post
Share on other sites
8 minutes ago, Prakash Pagadala 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

Shell_Solid.zip

Edited by Roy Duan

Share this post


Link to post
Share on other sites
Guest

Roy,

 

To capture bending effects it is neccessary to have more than 2 rows of elements when using solid element type.

Share this post


Link to post
Share on other sites
10 minutes ago, Prakash Pagadala 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

Share this post


Link to post
Share on other sites
12 minutes ago, Q.Nguyen-Dai 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

Edited by Roy Duan

Share this post


Link to post
Share on other sites
Guest
1 hour ago, tinh 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

Share this post


Link to post
Share on other sites

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.

tinh likes this

Share this post


Link to post
Share on other sites
On 2017/9/14 at 10:27 PM, Q.Nguyen-Dai 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.

59bc86978f618_ResultsCompareTable.thumb.png.bc30cc6e07a09d61205b304e07e120b2.png

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

Shell Solid Compare results summary.pdf

Share this post


Link to post
Share on other sites
On 2017/9/14 at 10:25 PM, Prakash Pagadala 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.

59bc885fe3204_ResultsCompareTable.thumb.png.3f327d4027cad5645de7f774172ff2fa.png

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

Shell Solid Compare results summary.pdf

Share this post


Link to post
Share on other sites

Here're my tests with SAMCEF & HEXA20 (2nd order) elements

3 elems/thickness

solid_3elems_displacements_mag.thumb.png.225df38a4c8822b4ba178c3714f2563a.png

 

4 elems/thickness

solid_4elems_displacements_mag.thumb.png.c7b85a80e96525aa393b25452e914bb8.png

 

5 elems/thickness

solid_5elems_displacements_mag.thumb.png.4c7bfc29f56a2a4849c217c2e4664497.png

 

For displacements: Good results even with few elements/thickness.

 

For equivalent stress:

3 elems/thickness

solid_3elems_equivalent_stress.thumb.png.f8c724946cb2607ad0b10c694f386089.png

 

4 elems/thickness

solid_4elems_equivalent_stress.thumb.png.08f88b3d5192a672c68399c1fe1ab706.png

 

5 elems/thickness

solid_5elems_equivalent_stress.thumb.png.16dbed95c8f95bc6de13412e6f1bf23e.png

 

For stress: A lot of elems/thickness to got the same result as shell model.

 

Share this post


Link to post
Share on other sites

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

 

Share this post


Link to post
Share on other sites

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.

Share this post


Link to post
Share on other sites

Here's another test with HEXA20 in SAMCEF: 10 elems/thickness !!!

solid_10elems_equivalent_stress.thumb.png.eb9f8dcb4234efbac274b72908163a02.png

In attachment, you have also H3D (SAMCEF_solid_10elems.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.

 

 

 

 

 

 

Share this post


Link to post
Share on other sites
Guest
On 9/16/2017 at 8:39 PM, Q.Nguyen-Dai 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. 

Share this post


Link to post
Share on other sites
On 2017/9/16 at 11:09 PM, Q.Nguyen-Dai said:

Here's another test with HEXA20 in SAMCEF: 10 elems/thickness !!!

 

In attachment, you have also H3D (SAMCEF_solid_10elems.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

Share this post


Link to post
Share on other sites
9 hours ago, Prakash Pagadala 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

Share this post


Link to post
Share on other sites
3 minutes ago, Roy Duan 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.

 

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

Sign in to follow this  

×
×
  • Create New...