Workshop 3

Mesh Control
Workshop 3 - Meshing Controls
Workshop 3 - Goals Workshop Supplement

ANSYS Workbench - Simulation

• Use the various DS mesh controls to enhance the mesh for
the crankshaft model.
• Problem statement:
– The model consists of a Parasolid file representing a
crankshaft for a small engine shown below.
– Our goal is to mesh the model using all defaults and inspect
the result. Next we will add mesh controls to modify the mesh
in various regions of the model.

March 29, 2005

Inventory
#002216
WS3-2
Workshop 3 - Meshing Controls
Workshop 3 - Assumptions Workshop Supplement

ANSYS Workbench - Simulation

• Since this is a meshing exercise we will not be applying
loads or solving the model. Instead we will assume a linear
static structural analysis is to follow the meshing
operation.

March 29, 2005

Inventory
#002216
WS3-3
Workshop 3 - Meshing Controls
Workshop 3 - Start Page Workshop Supplement

ANSYS Workbench - Simulation

• From the launcher start Simulation.

• Choose “Geometry > From File . . . “

and browse to the file “Crankshaft.x_t”.

• When DS starts, close the Template

menu by clicking the ‘X’ in the corner
of the window.
Note: Although we could use the
Simulation Wizard, the remaining
workshops contain instructions on
March 29, 2005
manual completion. Inventory
#002216
WS3-4
Workshop 3 - Meshing Controls
Workshop 3 - Basic Meshing Workshop Supplement

ANSYS Workbench - Simulation

1. Highlight the mesh branch to
view the mesh and access the
meshing controls.

March 29, 2005

Inventory
#002216
WS3-5
Workshop 3 - Meshing Controls
. . . Workshop 3 - Basic Meshing Workshop Supplement

ANSYS Workbench - Simulation

2. Inspect the mesh detail window. Notice the
default global control is “Basic” and the 2
“Relevance” is 0. Advanced mesh features
are available as a licensed option.
3. RMB on the mesh branch and choose to
“Preview Mesh”.

March 29, 2005

Inventory
#002216
WS3-6
Workshop 3 - Meshing Controls
. . . Workshop 3 - Basic Meshing Workshop Supplement

ANSYS Workbench - Simulation

• The completed mesh (shown
here) is made up of a relatively
coarse tetrahedral mesh.

4. Expand the “Statistics”

section of the details window
to check the number of nodes
and elements.
Note the actual number of nodes
and elements will vary slightly
across different machines and
platforms.
4
March 29, 2005
Inventory
#002216
WS3-7
Workshop 3 - Meshing Controls
Workshop 3 – Mesh Relevance Workshop Supplement

ANSYS Workbench - Simulation

5. In the detail window for the mesh change the “Relevance”
to 50 (note: relevance may be set by dragging the slider bar
or typing the desired value into the field).

• Again RMB the mesh branch and “Preview” the mesh. A

visual inspection of the mesh along with the statistics
section in the detail window can be used to compare the
effects of the meshing changes.

March 29, 2005

Inventory
#002216
WS3-8
Workshop 3 - Meshing Controls
Workshop 3 – Sizing Control Workshop Supplement

ANSYS Workbench - Simulation

• We will assume the pin section
(shown boxed at right) is an area
of interest for us. We will apply
a local mesh control in this
region.
• We’ll take advantage of several
shortcuts in DS to help us
evaluate the appropriate size for
the control.

March 29, 2005

Inventory
#002216
WS3-9
Workshop 3 - Meshing Controls
. . . Workshop 3 – Sizing Control Workshop Supplement

ANSYS Workbench - Simulation

• First orient the model so we are viewing down the X axis as
shown here.

• A handy shortcut to do this is to use the triad to re-orient

the model. Clicking on any of the axes (or the “iso” ball)
the triad will rotate the model accordingly.

March 29, 2005

Inventory
#002216
WS3-10
Workshop 3 - Meshing Controls
. . . Workshop 3 – Sizing Control Workshop Supplement

ANSYS Workbench - Simulation

• Zoom into the area of interest. Notice the region is made
up of 3 surfaces. To gauge the size of the region we can
use the ruler tool (If the ruler is not displayed, use the ruler
toggle at the top of the GUI to activate it).
• Inspection of the model shows the
pin section is roughly 10 mm
across.

March 29, 2005

Inventory
#002216
WS3-11
Workshop 3 - Meshing Controls
. . . Workshop 3 – Sizing Control Workshop Supplement

ANSYS Workbench - Simulation

6. Select the 3 surfaces in the pin region.
• Note: by holding the CTRL key we can select each of the
desired surfaces individually using left mouse clicks. An
alternative shortcut called “paint selecting”, is to hold the
left mouse button while dragging the cursor over the
desired areas (no CTRL key necessary).

March 29, 2005

Inventory
#002216
WS3-12
Workshop 3 - Meshing Controls
. . . Workshop 3 – Sizing Control Workshop Supplement

ANSYS Workbench - Simulation

7. With the 3 surfaces selected choose “Sizing” from the
mesh control menu.
7

8. In the detail for the size control change “Element Size” to 1

mm.

8
March 29, 2005
Inventory
#002216
WS3-13
Workshop 3 - Meshing Controls
Workshop 3 – Mesh Refinement Workshop Supplement

ANSYS Workbench - Simulation

• Again “Preview Mesh” and inspect the new mesh as before.
• We will also assume the chamfer section on the side of the
flywheel is also an area of interest.

March 29, 2005

Inventory
#002216
WS3-14
Workshop 3 - Meshing Controls
. . . Workshop 3 – Mesh Refinement Workshop Supplement

ANSYS Workbench - Simulation

9. To apply the refinement control first select the chamfer
surface.

10. Highlight the mesh branch and RMB. Choose “Insert >
Refinement”.

10
March 29, 2005
Inventory
#002216
WS3-15
Workshop 3 - Meshing Controls
. . . Workshop 3 – Mesh Refinement Workshop Supplement

ANSYS Workbench - Simulation

• Mesh refinement is an iterative meshing tool that can be set
to integer values from 1 to 3 . A value of 1 provides the
least refinement (coarsest mesh) while a value of 3
provides the most refinement (finest mesh). Leave the
refinement level set to 1 and again “Preview Mesh”.

March 29, 2005

Inventory
#002216
WS3-16
Workshop 3 - Meshing Controls
Workshop 3 – Mapped Faces Workshop Supplement

ANSYS Workbench - Simulation

• Finally we’ll apply a “Mapped Face Meshing” control to a
surface in the model. Mapped face meshing is typically
used in contact analyses to insure a “regular” mesh on the
contact surface. High quality elements are often required
when detailed contact results are desired.
11. Select the cylindrical surface shown here (either side of the
part is OK).

11

March 29, 2005

Inventory
#002216
WS3-17
Workshop 3 - Meshing Controls
. . . Workshop 3 – Mapped Faces Workshop Supplement

ANSYS Workbench - Simulation

12. Highlight the mesh branch and RMB. Choose “Insert >
Mapped Face Meshing”.
• Again “Preview Mesh”. 12

March 29, 2005

Default Mesh Mapped Face Mesh Inventory

#002216
WS3-18