Plate Forces and Moments

Question:

Sir,

I would like to ask something regarding the results of Plate elements.
I have two Midas model for our discussion and comparison

MODEL 1 :

Using Automesh by clicking the 4 points only ( 4 nodes of the footing)

MODEL 2 :

Using Automesh but I assigned nodes in which I can get almost equal to 0.3m plate size. ( I used 0.3m as division for the plate elements using Automesh command).

Both MODEL 1 and MODEL 2 have the same support reactions as shown below :



After getting the Support Reaction, I checked again the Plate forces Shear and Moments.

For our discussion purposes, I checked the shear Vyy.

When I checked the Plate Shear using load combination 7 there is a difference in the value as shown below :



In this sample diagram, Shear Vyy of model 1 is 149 kN while MODEL 2 is 140 kN

I expect that the result should be the same because there is no difference in the loadings and reactions.

May I know what is the reason why the result is different.?
Is there something wrong with my model ?

I will attach also the sample Midas gen for the MODEL 1 and MODEL 2

I hope for your reply soon.

Thank you very much.

MRS














Answer:

Thank you very much sir

Hi Ray Oliver ,

Thanks for waiting, the answers to all the questions are been given below

Question 1 : Is there any command in Midas gen in which I can check if the plate element that I create have a correct skew angle, warpage and taper?

Answer: no, there is no option available in Midas Gen which can directly shows you the values of Aspect ratios, skew Angle, warpage, and taper of meshing.

If the user needs to check that, he/she needs to verify manually.


Question 2 : Usually manual creation of plate element is suitable if you want to get the fine mesh because you can control it by copying the nodes in any distance that you want then assign the plate manually but there is an instance that you have an irregular shape like octagon or pentagon that is why we want to use the Auto mesh command to make the modelling easier. 


Using auto mesh, I expect that Midas gen will automatically give the correct ratio for fine mesh, skew angle, warpage, and taper.

In auto mesh command we can control the divisions of plate as shown below :

But there is instance that assigning divisions it will create some irregular shapes.


Answer: yes, it will create an irregular mesh, but it is due to meshing of irregular shape of geometry that is to be meshed. Midas gen Will not automatically provide the optimum/correct aspect ratio, skew angle warpage, and taper.

Question 3 Is Midas gen automatically give the correct fine mesh ratio, skew angle, warped and taper ?

Answer: no, In Auto Mesh function, Midas gen provides the meshing according to Mesh size provided by the users and other parameters shown in Dialogue box. It will not account aspect ratio, skew angle, warped and taper while providing meshing.

For demonstration purpose I have shown three meshed model to demonstrate how meshing is done.

Size of geometry opted is 8mX3m.

Model 1: input length as 2m create a mesh of 2mX1.5m which has the aspect ratio of 1.33.


Model 2: input length as 1m create a mesh of 1mX1m which has the aspect ratio of 1.



Model 3: input length as 3m create a mesh of 2.67mX3m which has the aspect ratio of 0.89.


We can clearly see that mesh is dependent of mesh size input from the above figures.

Note: here you can see that in model 3 input for length was 3m but it creates the mesh of 2.67mX3m, this is because if it creates the mesh size of 3mX3m the total length in longitudinal will be 9m which is not possible therefore Midas gen automatically resizes the mesh according to geometry.

Question 4 : What is the difference between checking the length and divisions in mesh size.?

I understand the division part it means that midas gen will automatically divide the length into the value of division part. How about if I checked the length ?

Answer: 


Length function will be defining length of mesh elements. For example, if you have 4mX4m geometry and 1m is gives as length, so it will be creating mesh elements of 1mX1m.

Division function will be directly dividing your given area into number of divisions provided. For example, if you have 4mx4m geometry and 2 division is given as division, so it will be creating mesh elements 2mx2m.

Question 6 :  What is the difference between Average nodal and Average Nodal Active only because there is a different value.?


                        Which one is the correct value to use?


Question 7 : Element nodal value is more closely to the value of Average Nodal Active only.

                       Why is that the value of Average nodal is not close with the element nodal ?

                        What does it means ? 



I have been using the Element Nodal in designing plate element. 


Answer: In the given model, the results for Myy for Element nodal will show the contour for the active elements it will not show the results for Pedestal area.

Now, Avg. nodal gives the results at node by averaging the nodal forces due to surrounding elements sharing same boundary. It will average the forces of all elements sharing same boundary whether active or not active (Pedestal area results will be accounted).

If we check on the Avg. nodal active only, in the given model it will not accounts the forces due deactivated elements (pedestal area) for averaging the forces.


Therefor, the results for different in element, average nodal and avg. nodal active . 

Question 5 :  Which one is suitable to used in designing plate element. Is it Element nodal or Average Nodal ?



Question 8 : Is this the best option in designing plate element rather than average nodal values?

Answer: This totally depends on Structure, mesh quality and Loadings.

For better understanding of this we have done mesh convergence study for which we have made four different Mesh containing plate elements. It contains slab geometry of size (8mX8m) but different mesh sizes in each of them. Studies have been done for Mxx plate moments. In this study two loadings type has been consider for comparison.

1- Pressure Load (UDL)

2- Point load on the node at 2m from Left- bottom.


The geometries have been shown below. 


All the study has been done on the node which is 3m from Left and 2m from bottom in each mesh as shown by red circles.


The results of all the models for both loadings have been shown below.



Conclusion drawn from the above study:

· Finer the mesh, the more is the accuracy.

· Good quality element mesh needs to be generated and we do not have any recommended value of mesh size. It depends on the problem statement.

· Point loads create stress concentration areas.

· When we have point loads, the mesh should be fine to get correct result.

· When we have point loads, do not take Avg. nodal if you are not sure of mesh quality.

· It is an engineering judgement based on the importance of project. If you need more accuracy, then fine mesh with element results shall be used.

· In an important project where accuracy is needed, element result, and average nodal result should not vary much even when UDL and point loads exist.


· If element result and average nodal result are varying much, then mesh must be refined.

For your reference the model file and the excel files has been attached.


I think I was able to answer all the questions, kindly let us know if any further assistance needed.

Regards,

Anmol Saxena
Technical Support Engineer

Click here to give FEEDBACK
Click here to ESCALATE the issue


Hi Ray Oliver ,

Thanks for getting in touch, We are working on query and we will get back to you shortly.


Regards,
Anmol Saxena
Technical Support Engineer

Click here to give FEEDBACK
Click here to ESCALATE the issue


Sir,

Thank you very much for your reply and for the article that you have sent to me.

Regarding the article that I have read, one of the most important part is to check the mesh size.

The fine mesh will give the accurate result and there are some rules to be check like the ratio of longer span / shorter span of plate element should be at least close to 1. Other need to check are the skew angle, warpage and taper.

Question 1 : Is there any command in Midas gen in which I can check if the plate element that I create have a correct skew angle, warpage and taper?
Question 2 : Usually manual creation of plate element is suitable if you want to get the fine mesh because you can control it by copying the nodes in any distance that you want then assign the plate manually but there is an instance that you have an irregular shape like octagon or pentagon that is why we want to use the Auto mesh command to make the modelling easier. 

Using auto mesh, I expect that Midas gen will automatically give the correct ratio for fine mesh, skew angle, warpage and taper.
In automesh command we can control the divisions of plate as shown below :



But there is instance that assigning divisions it will create some irregular shapes.
Question 3 : Is Midas gen automatically give the correct fine mesh ratio, skew angle, warped and taper ?
Question 4 : What is the difference between checking the length and divisions in mesh size.?
                       I understand the division part it means that midas gen will automatically divide the length into the value of division part.
                       How about if I checked the length ?

Regarding Average Nodal and Element nodal comparison :

Based on the article it says that you can check if the plate element is accurate by comparing the diagram of element nodal and Average nodal.
I created sample Myy and Vyy result based on MODEL 2 for our discussion purposes.

For Myy Result :



For Vyy result :





I present the three option based on Midas gen :

1. Element Nodal 
2. Average Nodal
3. Average Nodal ( with checked the Avg. Nodal Active only box)

Based on the Plate diagram there are almost same but different values.
Usually in designing the plate, I am using the element nodal because I always assigned the local axis :

X  - parallel to the global +X axis
Y  - parallel to the global +Y axis
Z  - parallel to the global +Z axis

Question 5 :  Which one is suitable to used in designing plate element. Is it Element nodal or Average Nodal ?
Question 6 :  What is the difference between Average nodal and Average Nodal Active only because there is a different value.?
                        Which on is the correct value to use?
Question 7 : Element nodal value is more closely to the value of Average Nodal Active only.
                       Why is that the value of Average nodal is not close with the element nodal ?
                        What does it means ? 

I have been using the Element Nodal in designing plate element. 
Question 8 : Is this the best option in designing plate element rather than average nodal values?


I have an urgent work that need this clarification.
I hope for your reply soon .
It means a lot to me.

Thank you very much for your help.












Hi Ray Oliver ,

Thanks for waiting 
Here are the explanations for your questions 

Q1)  I expect that the result should be the same because there is no difference in the loadings and reactions

Reactions will be same because equilibrium must be established.

Q2) May I know what is the reason why the result is different.?

       Is there something wrong with my model?


There will be difference in results based on mesh size if it is coarse or fine. In your case, model 1 and model 2 mesh size is different. Model 1 has coarser mesh than Model 2 thereby the results will be different. To compare the results, do the following:


1) Make a fine mesh between two models

2) Ignore the stress concentration areas of the two models for comparison.

3) Compare the Average Nodal Results



Please go through this article:

https://www.midasoft.com/bridge-library/ensuring-element-quality-for-mesh-size-transition


https://www.midasbridge.com/en/blog/bridgeinsight/meshing-its-significance-to-structural-engineers



Regards,
Anmol Saxena
Technical Support Engineer

Click here to give FEEDBACK
Click here to ESCALATE the issue


Hi Ray Oliver ,

Thanks for writing to us, We are working on your query and we shall get back to you shortly.


Regards,
Anmol Saxena
Technical Support Engineer

Click here to give FEEDBACK
Click here to ESCALATE the issue
Creation date: 3/10/2023 4:08 PM      Updated: 3/14/2023 1:04 PM
Files   
DataImage22.png
139 KB
DataImage3.png
52 KB
DataImage33.png
128 KB
DataImage34.png
159 KB
DataImage35.jpg
76 KB
DataImage35.png
51 KB
DataImage36.png
138 KB
DataImage55.png
121 KB
DataImage56.jpg
98 KB
DataImage69.png
42 KB
DataImage72.png
128 KB
DataImage82.jpg
87 KB
DataImage84.png
14 KB
DataImage93.png
134 KB
DataImage93.png
22 KB
Mesh Sensitivity Study.mgb
2 MB
Mesh Sensitivity Study.xlsx
28 KB
MODEL 1.mgb
671 KB
MODEL 2.mgb
789 KB