How much mesh refinement should I do?

  • Topic Is Locked
  • Last Post 17 July 2019
  • Topic Is Solved
peteroznewman posted this 12 November 2017

 A linear statics model calculates a maximum equivalent stress, which is compared with a yield strength.

An initial mesh has a certain element size around the point of maximum stress. 
A second mesh with smaller elements is solved and gives a new value of maximum stress.
A third mesh with even smaller elements gives a third value of maximum stress.

How do you decide when to stop refining? 

One method is described in ASME V&V10.1 “Illustration on V&V for Computational Solid Mechanics” and is called Calculation Verification, one small part of the entire Verification and Validation process.

 Below is an example using a tetrahedral mesh with a Sizing Mesh Control on a Sphere of Influence.

Maximum Stress from six mesh sizes were plotted. The red line is a best fit line through the three smallest element sizes. This line, or the calculation in Section 7.2 of V&V10.1, can be used to extrapolate the maximum stress to a zero-size element. This is the estimate for the exact maximum stress, but is only valid when the results are being calculated in the asymptotic convergence regime. The line estimates the maximum stress is 607 MPa.  See this discussion for an alternative mesh control using inflation.

The three largest element sizes are clearly trending toward a very different zero-size element value and should not be used since those results are not in the asymptotic convergence regime. V&V10.1 has more information on how to determine if you are in that regime.

In this example, I used a factor of 1.5 to change each successive element size. V&V10.1 recommends the factor be > 1.3.

Order By: Standard | Newest | Votes
Rashi posted this 09 May 2018

Thank you very much for this article.

In your article and in the V&V10.1 it mentions about "asymptotic convergence regime", how can we know our results are in this region?

The explanation in the standard is bit confusing (V&V10.1). Which compares a theoretical and a calculated value for variable"p".  


peteroznewman posted this 09 May 2018

Great question Rashi, and one that I had also pondered after finding the illustration and the standard to be lacking in clarity on that point.

Here is a tutorial that someone at NASA put together for CFD models. It has a paragraph on Asymptotic Range of Convergence.

mekafime posted this 14 August 2018

Hi Peter,

for this example, is recommend use 0.1 or 0.15 element size?

peteroznewman posted this 14 August 2018

Hi Mekafime,

The element size is not an absolute value, and it would depend on the length units anyway.

The idea is that you let ANSYS mesh with an edge size that makes a reasonable looking mesh to get your first point on the plot. 

Say in your case, the element edge length was 12 mm.  The rule is to divide by 1.5 to get the next point on the plot. So the series of solutions for the mesh size for elements around the peak stress would be: 12, 8, 5.3, 3.5, 2.4, 1.6 mm

You solve for each of those element sizes and plot the corresponding Maximum Stress.  Once you start to get a set of three or four points that are trending toward a straight line, you can stop cutting the element size.



  • Liked by
  • msnadeem
mekafime posted this 15 August 2018

Hi Peter,

the size that you state is :

and the stress value is the max 

Many values in size of mesh and stresses and with this I have the mesh convergence study?

peteroznewman posted this 16 August 2018

Hi mekafime,

Yes, that may work if you are on an unlimited Research license, since you are making a global mesh size change, you will get smaller elements everywhere, even away from the peak stress where the smaller elements are not needed.

If you are on a Student license, you might find that you exceed the allowable node count of 32,000 nodes before you have enough points on your mesh convergence plot when using the above mesh refinement approach.  A more efficient method is to apply localized sizing around the peak stress. Create a Coordinate System near the location of peak stress. Create a Sizing control on the bodies and set the size using a Sphere of Interest with an appropriate radius so that the smaller elements are inside that sphere, while outside that sphere the global mesh size is used.

Sometimes a model includes a stress singularity, which means that the stress keeps increasing as the element size decreases. Adding a blend to a sharp interior corner of the geometry in CAD is the usual mitigation to eliminate the stress singularity.



  • Liked by
  • mekafime
abenhadj posted this 17 August 2018

Enough to deduce that your solution is mesh independent and you can then switch on to a Richardson extrapolation. Here some ideas from the NASA: 

Best regards,


mekafime posted this 29 June 2019

Hi Peter,

I just found a problem like the one you mentioned about the stress singularity as the size of the elements is reduced. How I can add a blend to a Sharp interior corner ? Have you a video about this?


peteroznewman posted this 29 June 2019

How you add a blend depends on the Geometry editor you use. Is it DesignModeler, SpaceClaim or another CAD system?

mekafime posted this 29 June 2019

Hi Peter

DesignModeler and SolidWorks.

peteroznewman posted this 29 June 2019

In SolidWorks, you use the Fillet tool.

mekafime posted this 10 July 2019

Hi Peter,

In this model I have a fillet in a side because is a tube.

I use sphere of influence with mesh size 1.3 factor 

I can use 10 mm for my model?


peteroznewman posted this 10 July 2019

What is the wall thickness?   What displacement are you measuring?

I suggest the sphere of influence include the fillet around both tubes instead of just the center portion.

mekafime posted this 11 July 2019

Hi Peter

Wall thickness = 5.92 mm

Displacement in Y (vertical)  from node in the middle of the tube, I'm refining the mesh of the horizontal tube.

Do you indicate that the sphere should be like this?


peteroznewman posted this 11 July 2019

I suggest you forget about the Sphere of Influence and just use the Mesh sizing control that is applied to the two tubes and the fillet. You can try size 10, 6.6, 4.4, 3.0, 2.0, 1.3 mm and plot that data.  What would be interesting is to see the effect on the results at a fixed element size, say 3 mm, of changing the Formulation of the contact.  MPC is probably the best. 

I'm concerned that you have bonded contact in the region of high plasticity.  I refer you back to the post that I made before that I don't like contact used in regions of high plasticity.  This image represents an alternative way to make the connection. The bonded contact is far from the region of high plasticity which is occurring in a contiguous solid.


mekafime posted this 11 July 2019

Hi Peter,

I have this assembly of 3 pieces (image) and I need only the central part

I used cuts, trying to improve the mesh, the shared topology only apply on horizontal tube

What tool could I use in DesignModeler to merge the pieces? 



peteroznewman posted this 11 July 2019

Boolean Unite

mekafime posted this 11 July 2019

Hi Peter,

I use Boolean , with some cuts because I need some points to take dates to graphics.

But when I do meshing is irregular 

I can´t use cuts because is the plasticity zone.


mekafime posted this 11 July 2019

I used hex dominant

peteroznewman posted this 11 July 2019

Great, now you can do the element size series for all those bodies meshed at 10 mm, 6.6 mm, 4.4 mm, 3.0 mm, 2.0 mm, 1.3 mm element size and plot the result data.  If you are using plasticity, Equivalent Total Strain is a good result to plot.

mekafime posted this 11 July 2019

The plot states this:

There´s a big difference.

About Equivalent Total Strain in short...

mekafime posted this 13 July 2019

Hi Peter

I already obtained the requested graphic but I have a problema in this (new) computer when I use 2 mm of element length the computer freezes and I have to restart (Do you know how I can solve that in ANSYS?). So I'm using 3 mm as minimum element size up to15 mm.

Attached Files

peteroznewman posted this 14 July 2019

Your Y axis has obscured the values. Here is a better plot of the last 3 points.

This doesn't seem to make sense. Can you attach your project archive?

  • Liked by
  • mekafime
mekafime posted this 14 July 2019

I added it in the previous answer.


mekafime posted this 15 July 2019

Hi Peter,

Could you open the model or I attach it wrong?

peteroznewman posted this 15 July 2019

I have opened your model in 2019 R2.

I see you measured Equivalent Total Strain at a Node.  The intention of the convergence check is to plot the maximum global value, not one specific node. I am running your model across the element sizes to get new data to plot. This is automated using Parameter Set.

Is this data evidence of convergence to a zero element size result of Max. Eq. Total Strain = 0.013 or would the next data point at 0.89 mm element size be much greater than that?  UPDATE: the result for element size 0.89 mm is 0.013265.

peteroznewman posted this 15 July 2019

I added the last point to the convergence plot. 
The green line is the best fit through the last 4 points, the red line through the last 2 points.

It might be reasonable to estimate that the Max. Total Strain is < 2%.

mekafime posted this 15 July 2019

Hi Peter,

I'm trying to reproduce the same values that you obtained, I have some doubst.

- How do I get the graph ? (I'm in parameter set)

- 1.3/1.5 = 0.866 (0.89) or do you refer to another value?

- Would the ideal size be 1 mm, how much more could I take?



mekafime posted this 16 July 2019

I tried to parameterize the unión but the same thing happens to me when I use 2 mm of size of element the computer freezes, What other option do I have?

peteroznewman posted this 16 July 2019

I was going from the 3, 2, 1.3333, 0.8888, 0.5925 progression and rounding off. I was tempted to run the last value to see where it came out. I switched to Sphere of Influence to keep the mesh size within the ability to solve In-core for the 0.89 mm size.

Suppose I did run the 0.59 mm size and it turned out to be on the green line pointing toward a Max. Eq. Total Stain of 0.02.  That means that if you ran the model with the 1.3 mm element size, the result would show a Max. Eq. Total Strain of 0.01 while the true solution was 0.02.  You could say that is a 100% error, but the better way to think of it is to compare the value with a critical value such as the elongation at break.

If your model was for a brittle material that has an elongation at break of 0.015, then the difference between a result of 0.01 and 0.02 is the difference between predicting success and predicting failure to support the load. In that case it would be important to use small elements.

If your model was for a ductile material that has an elongation at break of 0.5, then the difference between 0.01 and 0.02 is insignificant. In that case you could use larger elements.

  • Liked by
  • msnadeem
Show More Posts

Topic Is Locked