Plate Forces and Moments

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,

Technical Support Engineer

Click here to give FEEDBACK
Click here to ESCALATE the issue