(FEM) 2D mesh interprets curve incorrectly. 2

[5H4D0W]

Im trying to mesh and simulate stress in a simple 2d example.
This represents a 1x20x100mm flat piece of steel under stress.
There is a stress concentration (notch) in the middle, with diameter 2mm.

I have been reducing the element size gradually to find a convergence value for maximal stress at the notch. But when I get down to element size 0.003mm, this happens:

Now, clearly the curve of the notch (radius 1mm) has not been interpreted as a curve, but as a many-sided polygon. The elements are smaller than the sides of this polygon, so the error is in the curve itself, or in the mesh interpretation of the curve.

So, how do I get the curve to act as an actual curve, or at least up the rezolution?

 

[cowski]

Now, clearly the curve of the notch (radius 1mm) has not been interpreted as a curve, but as a many-sided polygon.

Welcome to the world of FEA. The meshing step breaks your model into small elements, all of which have straight sides; this is the nature of finite element analysis. It is the job of the analyst to pick a mesh size and type, refine it (globally or locally as needed), and interpret the results. Since you know that your real model doesn't have those small discontinuities, ~38MPa is a good estimate of the stress in that area.

Edit: Also, you might look into a result type that averages the stress over the element to help smooth out the results.

www.nxjournaling.com

 

[5H4D0W]

cowski,

Yes, this is true. But as I mentioned, the percieved "sides" on the curve are much bigger than the element size.

Sides of curve: roughly 0.1mm <-- why so large?
Element size: 0.003mm

Thus, there should be more sides to the circle (i.e. "higher resolution").

 

[Tuw]

Hello 5H4D0W,

If you want to control the mesher to be exact size, you will need to use Mesh Control command, and define the edge of the notch to have specific number of nodes or size. Without using Mesh Control, the 2D mesher is only using 'element size' as an approximation for the overall surface to mesh, and would produce results which might not aligned with your intention.

In addition, I hope you are applying a tensile loading to the structure. For your information, 2D mesh has 6 DOF, and one of them is artificial. The artificial one is in the out-of-plane torsional direction. Please refer to k6rot. You can read more in

https://www.esacorp.com/nastran_hints_toc/nastran-2-d-elements/

(the hyperlink is not owned by me). For this reason, doing 3D mesh might be a better alternative to get more accurate result.

In addition, usually we would refer to nodal result for 2D meshing. This is contradicting to your contour result which is reading elemental result.

Hope this helps.

Kind regards,
Tuw

 

[5H4D0W]

Tuw, Thank you very much for the feedback. Unfortunately, it seems I cannot apply your advice in this situation. Let me explain.

The diameter of the notch is 2mm. The circumference of a whole circle is c = d*pi = 2(pi)mm. The arc in the notch is half of this =(pi)mm. That means I wil have (pi/0.003) elements along the arc. So, roughly 1047 elements along the arc.

I have now tried to add a Mesh Control modifier to the arc, density type: number on edge. Number: 1047.
And I still get this:

And yes, the model is properly constrained in the appropriate DOFs. It is experiencing a tensile load horizontally (top picture).

 

[rothers]

You'll never get it exact due to the polygon geometry abstraction used.

What do you have in preferences / meshing ?

High Resolution Polygon Bodies turned on ?

Project Node to CAD geometry turned on with a decent project tolerance ?

 

[5H4D0W]

Hi, Rothers.

I took a look at the Prefs/meshing dialog, and enabled the Project Node to CAD, but this did nothing.

Since I am using NX12, the High Resolution Polygon Bodies option has been moved to the polygon geometry tree. I assume it has previously been located in the preferences?

Anyway, enabling the high resolution in the aforementioned area made a huge difference! That was the key, truly. I still do not have full control of the resolution, but this makes my life a lot easier. Thank you!

 

[Tuw]

After some check, as long as you are not using moment load, the FEA result will be fine. In my test, k6rot only plays a role when moment load is applied in the out of plane direction of 2D mesh.

Tuw

 

[rothers]

We're on NX10.

You can check and adjust proximity of nodes to CAD geometry with Analysis/Finite Element Model Check/Adjust Nodes Proximity to CAD. You need to original CAD part or idealised part loaded (we don't use idealised parts).

Some good info on all this in online help