Learning Forum

[Thamanna Iqbal]

As part of my project I had performed an analysis of a circular fabric plate. I had conducted the analysis by providing horizontal, vertical and cross slits at the centre of the plate with varying geometry. So when I checked the results, as the width of slit increases the stress is reduced for the horizontal and vertical slits and in case of cross slits initially the stress increases with increase in slit size, then stress decreases with increase in slit size. Why does it happen like this?

Also, instead of slit when providing hole in the centre with varying diameter, the stress value shows initial increase in stress with decrease in hole dia and changes the pattern for small diameter. What could be the reason for this?

[Thamanna Iqbal]

In case of cross slits, initially the stress decreases with decrease in slit size and then increases and again decreases.

[peteroznewman]

Please show the Engineering Data entry for this material.

Please show some images of the slits.

Please show the loads and supports on this plate.

Please show charts of the change in result as a function of slit width or hole diameter.

For the hole, show the contour plot for the large and small hole to illustrate your comment that the pattern changes.

[Thamanna Iqbal]

 

The mass density provided is 4.6e-10 and E value is 300 MPa with Poisson ratio equal to 0.4. The slits are provided at centre symmetrically. The length of slit is kept constant with varying width. The edges of the plate is free for z translation only. An initial velocity in downward direction is provided. FSI analysis is carried out for thr study. 

 

 

 

 

 

[peteroznewman]

What is the diameter of the plate?

What is the orientation of the plate relative to the coordinate system? 

You said the edges are free in Z translation only. Is Z in the plane of the plate or normal to the plate? 

You said this is an FSI analysis, what is the load on the plate?

Show the mesh on the plate because element size has a large effect on stress. Where is the highest stress?  Is it in a sharp interior corner?  Do you know what a Stress Singularity is?

[Thamanna Iqbal]

Plate diameter is 600 mm. The centre of plate is at (0,0,0). Z plane is normal to the plate. Other than air pressure simulated by EOS no other load is applied. Auto mesh is used with element size 12mm. Highest stress occurs aroud the edges of slit. It is having sharp corner.

Sorry, I dont know about stress singularity.

[peteroznewman]

If the corner of the slit is a sharp corner, that is a stress singularity. That means the stress in the model is a strong function of element size. If the model is remeshed and the element edge length is cut in half, the stress will approximately double, even though there was no change in geometry, loads or supports!  That means as you changed slit widths and remeshed, it is likely that the element edge length was varying at the corner so most of the change in stress could be coming from changes in element edge length at the corner and little from the change in slit width.

Make the ends of the slit a semicircle and ensure there are many elements around that semicircle, say 12 elements or more. The stress singularity would be removed from the model and the change in stress when the slit width is changed would be almost entirely due to the slit width with almost no stress change due to remeshing.