- [Instructor] The finite element analysis method
discretizes the continuous CAD geometry
into large numbers of small elements.
The shape of these elements is very important.
Badly shaped elements will result in numerical inaccuracy
and possible failure of the analysis run.
The total number of elements has also to be kept
within reasonable bounds.
The solution time and memory requirements of the analysis
are roughly proportional to the number of nodes squared.
If the element numbers and hence node numbers
are uncontrolled, we can rapidly run
into very long run times.
The first thing we will consider is element quality.
SOLIDWORKS uses tetrahedral elements for solid meshing.
The ideal shape for a tetrahedral element has 60 degrees
including angles at all vertices,
or we can describe this as having equal length edges.
As the distortions increase away from this perfect shape,
the result is increasingly poor
numerical representation of the displacements
and the stress field within the elements.
This means that the stress distributions
can be badly affected.
If the element distortion gets too bad,
then we can contaminate the whole numerical solution
throughout the model.
Let's run a trial mesh on the conrod and see what kind
of elements the default meshing gives us.
So we click on the Analysis Study tab,
conrod static analysis.
If I right mouse click on the Mesh icon
in the Analysis Feature tree, then we want to Create Mesh.
We'll leave the Mesh Density slider bar
in its default central position.
This controls the size of elements globally
throughout the model.
Click OK and the mesh will run.
We right mouse click on the Mesh icon, we go to Details,
and then we have a summary of important details of the mesh.
So we have, for example, the total number of nodes
is just over 13,000.
The total number of elements is just underneath 8,000.
And then the maximum aspect ratio is about 9.8.
Now one of the fundamental measures of element quality
is this aspect ratio.
A high aspect ratio is a fundamental measure
of element distortion.
We've got a ratio of about 9.8 to one.
We can see where this is positioned.
So if I close down this dialogue box here,
right mouse click again on the mesh icon,
and say Create Mesh Quality Plot,
we can check on the Aspect Ratio button here
and then hit OK.
Now there's a new element in the Model Feature tree
under Mesh, called Mesh Quality Plot.
We've got one mesh within that
which is labeled Aspect Ratio.
We can right mouse click and we can hide that,
and we can right mouse click,
and we can show that at any time.
If I now Hide the mesh quality plot,
you notice the mesh has disappeared.
We need to come back up into Mesh
and say Show Mesh.
So it's just a little quirk.
If we'd plotted and shown the aspect ratio,
and I say Hide, we lose the mesh.
You find it back up here again if you just say Show Mesh.
So let's just see that mesh quality again,
and it works again.
It was around about 9.8.
We could see it's located up here.
Let's go and look at the big end.
And it's associated with an element that's trying
to run through the fillet.
Now if we look in really closely,
we can see that element has really flattened out.
This type of feature in the geometry is really awkward
for us to deal with.
It's not ever really there physically.
You can't machine a feature like that,
and when we discretizes it, do the FEA mesh,
then we start to pick up features like that.
We'll come back to this point
as we go on through the course.
Let's zoom out of the model.
The blue here is indicating the lowest aspect ratio
is just close to one.
Let's zoom in and look at an area
with that kind of aspect ratio,
and they're well shaped tetrahedral elements
close to equal angles within there.
We come back out to the full model.
Now there's a second mesh quality review option
within SOLIDWORKS called the Jacobian.
So right mouse click and say Create Mesh Quality Plot.
This time let's check Jacobian.
Now the Jacobian isn't a geometry measure,
but it's part of the numerical evaluation of each element.
Strictly speaking, it can only be calculated accurately
when the full FE analysis is run.
However, SOLIDWORKS can produce an estimate of the Jacobian.
To be useful, this needs to be a high quality estimate.
The high quality estimate can take longer to run
within SOLIDWORKS and could be very time consuming
for a large model.
So with the Jacobian selected, let's check OK.
Now we can see under the Mesh Quality Plot icon,
there's a new Mesh Quality Plot called Jacobian
and that's what we're looking at here.
The maximum value is 2.416.
If we zoom in that area again,
again you can see it's associated with these problem areas
that run out of the fillet.
Now the Jacobian check isn't particularly accurate here
because we've used the default settings.
Later on we're going to improve the accuracy
of the Jacobian check by increasing the order
of accuracy which again could take longer to run
within SOLIDWORKS.
Now the other aspect of meshing we need to consider
is the number of elements.
So let's right mouse click on Mesh
and look at Details again.
So we've got a default mesh size of around about 0.4
of an inch, and we've got just over 13,000 nodes,
and about 7,700 elements.
Let's experiment on half the elements
sized down to 0.2 of an inch,
and this will be globally throughout the model.
So I right mouse click on Mesh, choose Create Mesh,
open the Mesh Parameters option, and rather than accepting
the default which as I said was around about 0.4,
let's halve that and go for 0.2.
Click OK, and it'll remesh.
Let's go to the standard view.
We can see in general we've got a much finer mesh.
So literally globally, we've halved the element size.
Right mouse click on the mesh icon, choose Details again,
and now we can see the total number of nodes has jumped
to around about 92,000.
The total number elements has jumped to over 60,000.
The key metric is the number of nodes.
This is directly related to the number of degrees
of freedom in the model.
So here we've got about 6.6 times more nodes
than we did when we had 0.4 inch as the default size.
Now analysis runtime is roughly proportional
as a square law, so the analysis on this basis
will take up to 43 times longer.
It is not always that extreme, but certainly it is
some kind of power law there.
So 40 times longer to run, that could be quite significant.
So we'll close that down.
Let's check the aspect ratio by going here
Mesh Quality Plot, opening that up,
and we've got our Aspect Ratio Plot here ready to go.
So we now just say Show, and now we can see our aspect ratio
has gone up to 12 and, lo and behold,
it's in the same place as before.
So putting in a finer mesh is actually
making this aspect ratio worse.
If I zoom in really tightly, you can see this element here
is really flattening out.
You can imagine in the limit as we try to put more
and more fine elements in, we're getting tighter
and tighter in here and we're really chasing our tail.
We're trying to mesh something which isn't
physically realizable, and that's a kind of a trap
that we can get into with FE analysis.
So we're going to think about techniques to avoid that.
It's a limitation we just have to accept.
Let's come back to our full view.
Let's repeat this exercise and halve the mesh size again.
So Mesh, Create Mesh.
Again we had 0.2, so now we're going to halve that to 0.1.
Just click OK, it's remeshing.
You can sense it's taking longer to do the meshing now.
It's not instantaneous, even on the machine I'm using here.
Now it's complete.
You can see the model is really saturated now
with very tiny elements, 0.1 of an inch size throughout.
Let's right mouse click on Mesh, go to Details.
We can see the metrics, see what we've done.
The total number of elements is over 400,000.
The total number of nodes is over 600,000.
That's a big factor on the number of initial degrees
of freedom on the initial mesh.
And if we scale that up, I've worked out it means
a runtime of about 1,000 times longer in an extreme case.
So we're getting to the stage
where we're chasing this power law.
Successively halving the element size
means much, much longer runtime.
So it's obviously not a very effective
or productive strategy to try
and improve the quality of the mesh.
Let's check out the aspect ratio.
Again we open up the Mesh icon, Mesh Quality Plot.
Let's right mouse click on Aspect Ratio and say Show.
So if we zoom into the same place,
we see now we've got extremely high
aspect ratio elements again.
Let's zoom out.
Let's also check the Jacobian.
So come over to the Jacobian Quality Plot,
right mouse click and say Show.
The Jacobian is around about 2.11.
Again, it's slightly worse than before
but again the Jacobian here is a very inaccurate measure.
So let's set the element size back to 0.4
to avoid saving a large database.
So we come into Mesh, Create Mesh,
reset it to 0.4,
check to run the mesh,
you see that was very fast, back to our course mesh.
So we'll save off the model now,
and again we've kept it as a small size model.
We'll go to File, Save As, and we'll save it off
as baseline_9.
Now it's asking do we want to copy the result files?
The result files here are actually the mesh fill plots
showing us the Jacobian and the aspect ratios.
So they are classified as results
even though we haven't run the analysis as yet.
So the answer is Yes to that.
So in conclusion we've see that the element quality
can be very badly affected in difficult geometric areas
such as that fillet run out.
There's also a relationship between the local element size
and element quality.
In this case, refining the mesh actually makes
the element quality worse in that problem area.
We also saw a factor of 1/2 and 1/4 on element size
has an increasingly dramatic effect on the size
and the number of degrees of freedom in the model.
That meant that the mesh had took a lot longer
for the last model and the analysis was slowed down
even more dramatically.
We'll be looking for more efficient methods of meshing
and controlling element quality when we come
to do the production meshing.