Refining the mesh

The accuracy of an FEA solution is highly dependent on the quality of the mesh. If the mesh is too distorted or coarse near stress concentrations – the results can be skewed. Inventor Nastran provides users a variety of mesh controls and settings to refine the mesh to an acceptable level.

Review and impact the element quality

Once a mesh has been completed, the FEA program should be able to provide information on the quality of the elements. That is, for instance, if you have quad shell elements, you would like them to ideally be uniformly square vs. very long and very narrow rectangles.

In Inventor Nastran, you can access the option to Check Quality For Mesh from the Mesh Model node in the Model Tree.



The checks that can be performed for tetrahedral elements are shown below.



The program will indicate if there are elements that fall outside the ideal ranges. If so, the easiest way to change up the elements is probably to re-mesh the geometry – and that can be done on a global or local level.

Control the global mesh size

Most FEA programs will choose a default mesh size; however, this should generally be considered a starting point. As was just discussed, if the element quality needs to be improved – or if you are working on ensuring a converged mesh (discussed a little later) – one of the easiest things to do is to just change the global mesh size. 

Many FEA programs will allow you to adjust the size by a percentage or by an actual element size (absolute mesh sizing). It might be convenient to consider a known dimension of your model and set the absolute mesh size in comparison. For instance, if your geometry is 1″ thick and you know you want to perform the first analysis with three elements through thickness, then you can set the mesh size to around 0.33″. 

When changing the global mesh size, keep in mind that you are impacting the overall mesh of the model. When the object you are meshing is a solid, if you are reducing the global mesh size, the internal elements are also being reduced. If you have a part with a very large surface area or a very large volume, small changes to the overall mesh size can result in surprisingly large increases in element and node count. 

When globally reducing the size of mesh does, or will, result in too many elements to practically analyze within a reasonable amount of time, consider switching to a local mesh refinement.

Local mesh refinement

Most FEA programs will allow you to select a face/surface, edge, or vertex and specify that you want to increase the mesh density in that region. You can repeat this process in different regions of the model to obtain the finer mesh in just those locations where you need. 

In addition, you generally have access to advanced mesh controls that allow you to control mesh items, such as:

  • Controlling the growth rate from the smaller elements to the unrefined larger elements.



  • Controlling the placement of the midside nodes (or creating curved geometry).



While examining the model globally, these controls act locally at regions that meet the conditions for refinement.

It is worthwhile exploring the advanced meshing features and local controls to refine your mesh. These can help you get an improved mesh where needed, without impacting the mesh count as much as global refinement.

00:09

In this unit, we will be discussing Refining the Mesh using Global Mesh Settings as well as Mesh Controls.

00:19

For this example, we'll be working with this pivoting arm component.

00:23

You'll notice there have been two pin constraints created, as well as a force on the other end.

00:30

Before you begin working with the Mesh,

00:32

I do recommend hiding your boundary conditions to make the visibility of your Mesh and any controls a little bit easier.

00:39

To do that, go to "Object Visibility" in the top right corner and then you can just go ahead,

00:43

and deselect Loads and Constraints and anything else that might be obstructing your view.

00:51

Next, I'll start by generating my baseline Mesh.

00:55

If I go into the Mesh settings, you will see the Element Size by default has been chosen to be 114.852.

01:04

If you're not sure where to start, the default size is usually acceptable.

01:08

However, I do recommend rounding to an even number.

01:11

That way you do not have to worry about these decimal points and you know where you started from.

01:16

So I'll just start at 100 millimeters and I will select "Generate" to take a look at my basic Mesh.

01:26

So once that's been created, I can take a look and see if there are any areas that might need refinement.

01:31

In this case, due to the size of these elements,

01:34

it's struggling to accurately capture some of the smaller features around holes and fillets.

01:40

If I rotate around and zoom in, you'll notice this hole feature has been linearized significantly because the shapes are tetrahedrons.

01:50

But my geometry is a cylinder.

01:54

To combat this, you can do two things.

01:57

The first is if you go into the Advanced Settings which is underneath the Element Order selection,

02:04

you'll notice there's several settings in here that could be customized.

02:08

One thing that's extremely useful when working with curved or cylindrical features is activating the project Midside Nodes tool.

02:16

If I do so, it will take these elements around curvature,

02:21

and break them up into two segments to prevent linearization and to more accurately capture that shape.

02:27

If I select "Ok", and then I regenerate using the same element size, but the project Midside Nodes,

02:35

you'll notice it tightens up those elements by breaking them into two segments along that surface.

02:41

It also does it on these fillets here on the exterior of the shape.

02:48

Now, this can also be fixed using a smaller element size that will typically gain you more solution accuracy,

02:57

before you begin applying Mesh Controls or reducing the Mesh any further.

03:01

I do recommend running one analysis to determine where your stress concentrations are most likely to be.

03:08

And that's where you should have focus your attention for the Mesh Controls.

03:12

So I will select, "Ok", and I'll select "Run" to generate my first set of results.

03:19

So it'll kick off the solver and then provide a result.

03:24

And I'll select "Ok".

03:27

So taking a look at this contour,

03:29

I can see right away where some of the stress is going to be obviously on both sides of this bar,

03:35

because it's under tension on the top and compression on the bottom,

03:39

where I have compression, I'm getting a lot of stress on this fillet as well as around this hole.

03:44

So that is likely where I should focus my attention for my Mesh Controls.

03:48

I may not gain much by reducing the Mesh in other areas. So this is where I will add those controls.

03:59

So now that we have our baseline result, we can use this to guide the decisions we make in refining the Mesh.

04:05

So in the next unit, we will be converging our solution to make sure that this result is accurate.

04:11

In order to do that, we need to apply more elements into those key regions.

04:16

So to do that, I'm going to start by unloading the results and I will be applying what's called a Mesh Control to those faces.

04:24

To do that from the Mesh Panel, I will go to Mesh Control.

04:28

This will allow me to apply a finer element size onto a Vertex, an Edge or a Face.

04:35

Any of the elements touching that Vertex, Edge or Face will be affected.

04:40

So in this case, I'm going to focus on the cylindrical hole face as well as the fillets that surround it.

04:46

So to do so, I'll go to the Face Data and I can type in an Element Size.

04:51

I recommend a reduction of at least 50% or more.

04:55

In this case, I'm going to use a reduction of 10 times.

04:59

So I will use a 10 millimeter Element Size and I will apply it to those faces.

05:05

So if I zoom in, I can select that hole as well as the fillet here

05:10

and then they fillet on the outside of the hole to capture that transition.

05:15

I can then select "Ok" to confirm that Mesh Control which will show up with these lines in the graphics window.

05:21

And now when I regenerate my Mesh, what I'll get is a 10 millimeter Element Size on only those faces,

05:29

but it does affect some of the nearby geometry as it transitions to the 100 millimeter Element Size.

05:37

If I would like to control that rate of growth, I can go back into the Global Mesh Settings.

05:44

And if I go to the Advanced Mesh Settings, you'll see a value here for Max Element Growth Rate.

05:52

The default is 1.5, which means the next element can be 1.5 times the adjacent,

05:60

So a 50% rate of growth.

06:02

If I would like this to be a little bit smoother,

06:06

I can bring this value down to something like 1.2, which will add more elements,

06:11

but it will help to create a smooth transition in stress and strain.

06:15

So I will select "Ok", and regenerate the Mesh one more time.

06:20

And you'll notice more elements were created, but I have a much smoother rate of change.

06:26

Now that I'm satisfied with that Mesh, I'll select "Ok".

06:30

And I can then go and run the new analysis and compare where the maximum stress is as well as what its magnitude is.

06:43

So there's more elements, so it takes slightly longer to solve.

06:46

Once it's finished, I can view the result.

06:49

And you'll notice I've added about five megapascals of stress.

06:54

What you'll also notice is there's a lot more detail into where the stress is and what that shape looks like.

07:01

Before it was very blotchy.

07:03

But now I have several elements picking up that area,

07:06

giving me more definition and more insight which I can use to converge the result and verify its accuracy in the next unit.

Video transcript

00:09

In this unit, we will be discussing Refining the Mesh using Global Mesh Settings as well as Mesh Controls.

00:19

For this example, we'll be working with this pivoting arm component.

00:23

You'll notice there have been two pin constraints created, as well as a force on the other end.

00:30

Before you begin working with the Mesh,

00:32

I do recommend hiding your boundary conditions to make the visibility of your Mesh and any controls a little bit easier.

00:39

To do that, go to "Object Visibility" in the top right corner and then you can just go ahead,

00:43

and deselect Loads and Constraints and anything else that might be obstructing your view.

00:51

Next, I'll start by generating my baseline Mesh.

00:55

If I go into the Mesh settings, you will see the Element Size by default has been chosen to be 114.852.

01:04

If you're not sure where to start, the default size is usually acceptable.

01:08

However, I do recommend rounding to an even number.

01:11

That way you do not have to worry about these decimal points and you know where you started from.

01:16

So I'll just start at 100 millimeters and I will select "Generate" to take a look at my basic Mesh.

01:26

So once that's been created, I can take a look and see if there are any areas that might need refinement.

01:31

In this case, due to the size of these elements,

01:34

it's struggling to accurately capture some of the smaller features around holes and fillets.

01:40

If I rotate around and zoom in, you'll notice this hole feature has been linearized significantly because the shapes are tetrahedrons.

01:50

But my geometry is a cylinder.

01:54

To combat this, you can do two things.

01:57

The first is if you go into the Advanced Settings which is underneath the Element Order selection,

02:04

you'll notice there's several settings in here that could be customized.

02:08

One thing that's extremely useful when working with curved or cylindrical features is activating the project Midside Nodes tool.

02:16

If I do so, it will take these elements around curvature,

02:21

and break them up into two segments to prevent linearization and to more accurately capture that shape.

02:27

If I select "Ok", and then I regenerate using the same element size, but the project Midside Nodes,

02:35

you'll notice it tightens up those elements by breaking them into two segments along that surface.

02:41

It also does it on these fillets here on the exterior of the shape.

02:48

Now, this can also be fixed using a smaller element size that will typically gain you more solution accuracy,

02:57

before you begin applying Mesh Controls or reducing the Mesh any further.

03:01

I do recommend running one analysis to determine where your stress concentrations are most likely to be.

03:08

And that's where you should have focus your attention for the Mesh Controls.

03:12

So I will select, "Ok", and I'll select "Run" to generate my first set of results.

03:19

So it'll kick off the solver and then provide a result.

03:24

And I'll select "Ok".

03:27

So taking a look at this contour,

03:29

I can see right away where some of the stress is going to be obviously on both sides of this bar,

03:35

because it's under tension on the top and compression on the bottom,

03:39

where I have compression, I'm getting a lot of stress on this fillet as well as around this hole.

03:44

So that is likely where I should focus my attention for my Mesh Controls.

03:48

I may not gain much by reducing the Mesh in other areas. So this is where I will add those controls.

03:59

So now that we have our baseline result, we can use this to guide the decisions we make in refining the Mesh.

04:05

So in the next unit, we will be converging our solution to make sure that this result is accurate.

04:11

In order to do that, we need to apply more elements into those key regions.

04:16

So to do that, I'm going to start by unloading the results and I will be applying what's called a Mesh Control to those faces.

04:24

To do that from the Mesh Panel, I will go to Mesh Control.

04:28

This will allow me to apply a finer element size onto a Vertex, an Edge or a Face.

04:35

Any of the elements touching that Vertex, Edge or Face will be affected.

04:40

So in this case, I'm going to focus on the cylindrical hole face as well as the fillets that surround it.

04:46

So to do so, I'll go to the Face Data and I can type in an Element Size.

04:51

I recommend a reduction of at least 50% or more.

04:55

In this case, I'm going to use a reduction of 10 times.

04:59

So I will use a 10 millimeter Element Size and I will apply it to those faces.

05:05

So if I zoom in, I can select that hole as well as the fillet here

05:10

and then they fillet on the outside of the hole to capture that transition.

05:15

I can then select "Ok" to confirm that Mesh Control which will show up with these lines in the graphics window.

05:21

And now when I regenerate my Mesh, what I'll get is a 10 millimeter Element Size on only those faces,

05:29

but it does affect some of the nearby geometry as it transitions to the 100 millimeter Element Size.

05:37

If I would like to control that rate of growth, I can go back into the Global Mesh Settings.

05:44

And if I go to the Advanced Mesh Settings, you'll see a value here for Max Element Growth Rate.

05:52

The default is 1.5, which means the next element can be 1.5 times the adjacent,

05:60

So a 50% rate of growth.

06:02

If I would like this to be a little bit smoother,

06:06

I can bring this value down to something like 1.2, which will add more elements,

06:11

but it will help to create a smooth transition in stress and strain.

06:15

So I will select "Ok", and regenerate the Mesh one more time.

06:20

And you'll notice more elements were created, but I have a much smoother rate of change.

06:26

Now that I'm satisfied with that Mesh, I'll select "Ok".

06:30

And I can then go and run the new analysis and compare where the maximum stress is as well as what its magnitude is.

06:43

So there's more elements, so it takes slightly longer to solve.

06:46

Once it's finished, I can view the result.

06:49

And you'll notice I've added about five megapascals of stress.

06:54

What you'll also notice is there's a lot more detail into where the stress is and what that shape looks like.

07:01

Before it was very blotchy.

07:03

But now I have several elements picking up that area,

07:06

giving me more definition and more insight which I can use to converge the result and verify its accuracy in the next unit.

Refine the mesh - Exercise

  1. Open the Arm_Refine.ipt part file from your working folder. 
  2. In the Environments tab>Begin panel, click Autodesk Inventor Nastran. 
  3. In the Autodesk Inventor Nastran tab>Mesh panel, click Generate Mesh. 
  4. Once the mesh is generated, in the Mesh panel, click Mesh Settings. 
  5. In the Mesh Settings dialog box, change the Element Size (mm) to 110, then click Generate Mesh.



  6. Once the mesh is generated, click OK to close the Mesh Settings dialog box. 
  7. In the ViewCube, click the FRONT view and zoom in to the hole. 
  8. In the Mesh panel, click Mesh Settings. 
  9. In the Mesh Settings dialog box, click Settings. 
  10. In the Advanced Mesh Settings dialog box do the following: 
    1. In the Midside Nodes area, select the Project Midside Nodes option. Click OK. 
    2. Change Max Element Growth Rate to 1.2.



  11. Select OK. In the Mesh Settings dialog box, click Generate Mesh. Note that the mesh now conforms better anywhere that the geometry is curved. 
  12. Click Ok in the Mesh Settings dialog box. 
  13. From the Mesh panel, click Mesh Control. 
  14. In the Mesh Control dialog box, in the Face Data area, click inside the Selected Faces field. 
  15. Select the faces shown in the image below (face<4>, face<18>, face<19>).



  16. Change the Element Size (mm) to 25 and click OK.



  17. In the Mesh panel, click Generate Mesh. 
  18. In the Nastran Model Tree, right-click on Mesh Control 1 and select Edit.



  19. In the Mesh Control dialog box, change the Element Size (mm) to 10 and click OK. 
  20. In the Mesh panel, click Generate Mesh. 
  21. Save the model.
Was this information helpful?