Using Material Designer To Perform Homogenization Studies
3D Printing and other advanced manufacturing methods are driving the increased use of lattice-type structures in structural designs. This is great for reducing mass and increasing the stiffness of components but can be a real pain for those of us doing simulation. Modeling all of those tiny features across a part is difficult to mesh and takes forever to solve.
PADT has been doing a bit of R&D in this area recently, including a recent PHASE II NASA STTR with ASU and KSU. We see a lot of potential in combining generative design and 3D Printing to drive better structures. The key to this effort is efficient and accurate simulation.
The good news is that we do not have to model every unit cell. Instead, we can do some simulation on a single representative chunk and use the ANSYS Material Designer feature to create an approximate material property that we can use to represent the lattice volume as a homogeneous material.
In the post below, PADT’s Alex Grishin explains it all with theory, examples, and a clear step-by-step process that you can use for your lattice filled geometry.
One of the great new features in ANSYS Mechanical 19.2 is
the ability to perform a lattice optimization.
Accomplished as an option within Topology Optimization, lattice
optimization allows us to generate a lattice structure within our region of
interest. It includes varying thickness
of the lattice members as part of the optimization.
Lattice structures can be very beneficial because weight can
be substantially reduced compared to solid parts made using traditional
manufacturing methods. Further, recent
advances in additive manufacturing enable the creation of lattice structures in
ways that weren’t possible with traditional manufacturing.
Here I’ll explain how to perform a lattice optimization in
ANSYS 19.2 step by step.
For the lattice optimization, I’m starting with a part I
created that acts as a corner brace:
At this early point in the simulation, the Project Schematic
looks like this:
I used the Multizone mesh method to get a hex mesh on the
Simple loads and constraints are recommended especially if
you’ll be doing a downstream validation study.
That is because the downstream simulation on the resulting lattice
geometry will most likely need to operate on the FE entities rather than
geometric entities for load and constraint application. The boundary conditions
in this simple model consisted of a fixed support on one side of the brace and
a force load on the other side:
After solving, I reviewed the displacement as well as the
Satisfied with the results, the next step is to add a
Topology Optimization block in the Project Schematic. The easiest way to do
this is to right click on the Solution cell, then select Transfer Data to New
> Topology Optimization:
You may need to re-solve the static structural simulation at
this point. You’ll know if you have
yellow thunderbolts in the Project Schematic instead of green checkmarks for
the Static Structural analysis.
At this point, the Project Schematic now looks like this:
The Mechanical window now has the Topology Optimization
The change to make to enable a lattice optimization is
accomplished in the details view of the Optimization Region branch:
We then need to specify some settings for the lattice. The first of these is the Lattice Type. The various types are documented in the ANSYS
19.2 Help. In my example I selected the
The other properties to define are:
Minimum Density (to avoid lattice structures that are toothin. Allowed bounds are 0 and 1)
Maximum Density (elements are considered full/solid fordensities higher than this value, allowed bounds are 0 and 1)
Lattice Cell Size (used in downstream geometry steps andadditive manufacturing)
Values I used in my example are shown here:
Assuming no other options need to be set, we solve the
lattice optimization and review the results.
The results are displayed as a contour plot with values between zero and
one, with values corresponding to the density settings as specified above.
Note that at this stage we don’t actually visualize the
lattice structure – just a contour plot of where the lattice can be in the
structure. Where density values are
higher than the maximum density specified, the geometry will end up being
solid. The lattice structure can exist
where the results are between the minimum and maximum density values specified,
with a varying thickness of lattice members corresponding to higher and lower
The next step is to bring the lattice density information
into SpaceClaim and generate actual lattice geometry. This is done by adding a free standing
Geometry block in the Workbench Project Schematic.
The next step is to drag and drop the Results cell from the
Topology Optimization block onto the Geometry cell of the new free standing
The Project Schematic will now look like this:
Notice the Results cell in the Topology Optimization branch
now has a yellow lightning bolt. The
next step is to right click on that Results cell and Update. The Project Schematic will now look like
Before we can open SpaceClaim, we next need to right click
on the Geometry cell in the downstream Geometry block and Update that as well:
After both Updates, the Project Schematic will now look like
The next step is to double click or right click on the
now-updated Geometry cell to open SpaceClaim.
Note that both the original geometry and a faceted version of the
geometry will exist in SpaceClaim:
It may seem counter intuitive, but we actually suppress the
faceted geometry and only work with the original, solid geometry for the
faceted process. The faceted geometry
should be automatically suppressed, as shown by the null symbol, ø, in the SpaceClaim tree. At this point it will be helpful to hide the
faceted geometry by unchecking its box in the tree:
Next we’ll utilize some capability in the Facets menu in
SpaceClaim to create the lattice geometry, using the lattice distribution calculated
by the lattice optimization. Click on
the Facets tab, then click on the Shell button:
Set the Infill option to be Basic:
At this point there should be a check box for “Use Density
Attributes” below the word Shape. This
check box doesn’t always appear. If it’s
not there, first try clicking on the actual geometry object in the tree:
In one instance I had to go to %appdata%\Ansys and rename
the v192 folder to v192.old to reset Workbench preferences and launch Workbench
again. That may have been ‘pilot error’
on my part as I was learning the process.
The next step is to check the Use density attributes
box. The Shape dropdown should be set to
Lattices. Once the Use density
attributes box is checked, we can then one of the predefined lattice shapes,
which will be used for downstream simulation and 3D printing. The shape picked needs to match the lattice
shape previously picked in the topology optimization.
In my case I selected the Cube Lattice with Side Diagonal
Supports, which corresponds to the Crossed selection I made in the upsteam
lattice optimization. Note that a planar
preview of this is displayed inside the geometry:
The next step is to click the green checkmark to have
SpaceClaim create the lattice geometry based on the lattice distribution
calculated by the lattice optimization:
When SpaceClaim is done with the lattice geometry
generation, you should be able to see a ghosted image showing the lattice
structure in the part’s interior:
Note that if you change views, etc., in SpaceClaim, you may
then see the exterior surfaces of the part, but rest assured the lattice
structure remains in the interior.
Your next step may need to be a validation. To do this, we create a standalone Static
Structural analysis block on the Project Schematic:
Next we drag and drop the Geometry cell from the faceted
geometry block we just created onto the Geometry cell of the newly created
Static Structural block:
We can now open Mechanical for the new Static Structural
analysis. Note that the geometry that
comes into Mechanical in this manner will have a single face for the exterior,
and a single face for the exterior. To verify that the lattice structure is
actually in the geometry, I recommend creating a section plane so we can view
the interior of the geometry:
To mesh the lattice structure, I’ve found that inserting a
Mesh Method and setting it to the Tetrahedrons/Patch Independent option has
worked for getting a reasonable mesh.
Care must be taken with element sizes or a very large mesh will be
created. My example mesh has about 500,000
nodes. This is a section view, showing
the mesh of the interior lattice structure (relatively coarse for the example).
For boundary condition application, I used Direct FE
loads. I used a lasso pick after aligned
the view properly to select the nodes needed for the displacement and then the
force loads, and created Named Selections for each of those nodal selections
for easy load application.
Here are a couple of results plots showing a section view
with the lattice in the interior (deflection followed by max principal stress):
Here is a variant on the lattice specifications, in which
the variance in the thickness of the lattice members (a result of the
optimization) is more evident:
Clearly, a lot more could be done with the geometry in
SpaceClaim before a validation step or 3D printing. However, hopefully this step by step guide is
helpful with the basic process for performing a lattice optimization in ANSYS
Mechanical and SpaceClaim 19.2.