Dm quick evalguide design of component

© 2005 ANSYS, Inc. 1 ANSYS, Inc. Proprietary
Design Modeler Evaluation Guide
A Quick Tutorial
Ansys, Inc.
March, 2005
Last modification: May, 26th - PTH

Agenda
• Introduction
• Overview of the GUI
• Parametric Modeling
• Defeaturing and parametrizing an imported geometry
• Handling thin models
• Mid-Surfacing
• Slicing
• Internal volumes
• Enclosure

Introduction

Purpose of this tutorial
• This tutorial will guide you through the basics of Design Modeler. It is not meant to be
an in-depth training.
• You will learn how to:
– Model a parametric geometry
– Defeature an existing geometry before simulating
– Slice models to get specific mesh properties
– Handle thin models
– Create internal volumes
– Enclosures
• You need about 4 hours to go through the entire tutorial. You might skip one part or
the other, since they are independent. However, if you would like to have a broader
understanding of the functionalities, we strongly encourage you to follow the full
tutorial, especially the “Parametric Modeling” part.
• Make sure you read the “GUI overview” since it defines a few required notions that
will allow you to understand the explanations of each section.
• All examples can be done with DesignModeler 9.0 except the mid-surface one
(version 10.0)

Overview of the GUI

GUI - Graphical User Interface
GUI Overview
• GUI Layout:
– The menus and toolbars accept user input and commands
– Tool bars can be “docked” and re-sized to meet user’s preference
• Two Basic Modes of Operation
– Sketching tab (2D)
– Modeling tab (3D)
Mode Tabs

GUI Overview
Menus,
Toolbars,
Pull-down
Lists
Tree
Pane
Details
Pane
Mode Tabs
Status/Info Bar
GRAPHICS
(Model View)
Display
Triad

Main Menu
• Main menu:
– File: basic file operations
– Create: 3D creation and
modification tools
– Concept: Tools to create line
and surface bodies
– Tools: global modeling
operations, parameter
management, program
customization
– View: modify display
settings.
– Help: access documentation

Toolbars
Plane/Sketch Controls Graphics controls
3D geometry tools
File management Selection filters/toolsSketching
Only

• On-Line Help
• Copyright and Support
Info
Documentation

Accessing Help Topics
Contents
Tab
Search
Tab

Basic Mouse Functionality
• Basic mouse control (3 button
mouse assumed):
– LMB
• Geometry selection
• <CTRL> + LMB adds/removes
selected entities
• Hold LMB and sweep cursor =
continuous selection
– MMB
• Free Rotation (shortcut)
– RMB
• Box Zoom (shortcut)
• Open context menus

Adjacent/Flood Select
• In select mode the cursor changes to reflect current selection filter (it
will match the icon).
• Adjacent Select, selects surfaces or edges adjacent to the current
selection. Adjacent Select will pick all model surfaces within a tangent
tolerance of that surface or edge.
Selecting
Selection Filters
• Model features are identified by graphically picking them (selecting)
using the left mouse button
• Feature selection is done by activating one of the selection filters
(also from RMB)
New
Selection
Single/Box
Selection
2D Points, PF
Points, 3D
Vertices
2D Edges, Model
Edges, Line Edges
Faces
Solid Bodies,
Surface Bodies,
Line Bodies
Extension
Options

• Selection filters can also be set via RMB on the
Model View:
– In Sketching Mode:
– In Modeling Mode:
Selecting
Selection Filters

Selecting
Mouse Selection
• Add to or remove from current
selection set
– Depends on current selection filter
(lines, surfaces, etc.)
• “Paint Select” - hold left mouse
button then move (“paint”) mouse
over entities to be selected
– Depends on current selection filter
(lines, surfaces, etc.)
Ctrl++
++ Hold
Note: To un-select all, click once in a blank area of the geometry window

Selecting
Selection Panes
• “Selection Panes” allow
selecting hidden geometry
(lines, surfaces, etc.) after
initial pick
– Panes are color coded to
match part colors (for
assemblies)
– Multi-select techniques
apply to selection panes
as well
Note, each plane represents an entity (surface, edge, etc) that an imaginary
line would pass through starting from the initial mouse click location and
proceeding into the screen in the normal viewing direction.
Initial mouse click

Selecting
Box Selection
• The Selection Toolbar includes a “Select
Mode” button allowing users to select
items via Single Select or Box Select
– Selection based on currently active filter
– Type of selection based on dragging
direction:
• Drag from left to right: items completely
enclosed in the box are selected
• Drag from right to left: items completely
and partially enclosed in the box are
selected
– Note the difference in the hash marks
along the edges of the box to help you
determine which box selection type will
be performed.
Left to Right Right to Left

Graphics Controls
• Rotate Behavior (LMB):
– Cursor near center of graphics
screen = free rotations.
– Cursor outside center = rotation
about Z view.
– Cursor near top or side edge of
graphics screen = rotations about X
(top/bottom) or Y (left/right) axes.
Note: the cursor will change style depending on
window location/action

…Graphics Controls
– Panning
– Zoom in/out
– Box Zoom
– Fit model to graphics screen
– Look At: select model feature (surface, line, etc.) then “Look At”.
Model automatically orients normal to feature, centered at pick
point.
• Additional Mouse Controls
– While in select mode:
• Center mouse button = free rotations.
• Right mouse button = box zoom.
• Shift + Center mouse button = zoom.

…Graphics Controls
– While in Rotate, Pan, or Zoom mode:
• Left click on model temporarily resets center of view and rotation
at cursor location (identified by red dot).
• Left click in open area re-centers model and rotation center to
centroid.
Temporary
rotational
center

Context Menus
• RMB
– Context
Sensitive
Menus appear:
Model View
Print PreviewTree Object
Tree
Sketch
Dimensioning
Note: to delete a feature: highlight it
on Tree, RMB >Delete, or
<Delete> using keyboard

Cursor Modes
• Mouse Cursor is context sensitive
– Indicates chosen operation
• Viewing, Rotation…
• Selecting
• Sketch AutoConstraints
• System Status “busy, wait”

Parametric Modeling

Workshop Overview
• In this workshop, the
assembly shown on right
will be enhanced. Basic
DesignModeler
functionality will be
covered.
• The final design is shown
on the right

Open DesignModeler File
• Launch Workbench via “Start Menu >
Programs > ANSYS 9.0 > ANSYS
Workbench”
• In the Start page, select the “Geometry”
icon. Then select the [Browse] button.
– You will be prompted to select a
DesignModeler database to open
• In the Open dialog box, select the
“DMQuickIntroModeling.agdb” file and
click on [Open].

Create New Plane for 6th
Arm
– The DesignModeler geometry will be opened and
displayed, as shown on the right.
• Select ArmCopyPlane5 from the Tree. Select the
“New Plane” icon to create a new plane based on the
selected plane
– In DesignModeler, new planes for creating sketches
can be defined in a number of ways. In this example,
the five arms have been created by copying and
rotating previous planes by 60°, then copying the arm
sketch onto the planes.
• Change “Transform 1 (RMB)” to “Rotate about Y” with
the “FD1, Value 1” as “60°”.
– The newly-created plane will be renamed to
“ArmCopyPlane6” and rotated 60 degrees, as noted
above.
• Click on the “Generate” icon when done.
– After completing each action, use the “Generate” icon
to have DesignModeler check and execute the new
geometric definitions.
• In the Details view of the newly-created plane, change
the “Plane” name to “ArmCopyPlane6”.

Copy Sketch Instance for 6th
Arm
• Right-click on ArmCopyPlane6 and select “Insert >
Sketch Instance”
– A sketch instance can be thought of as a copy of
another sketch. Sketch instances may not be modified
directly, but they can be used as a way of using exact
copies of other sketches for other features, and these
sketch instances will automatically be updated if
changes are made to the original sketch
• DesignModeler will prompt for a “Base Sketch” to be
used. Select “ArmSketch” from the Tree, under
“XYPlane”. Click on “Apply” for “Base Sketch” to finish
the selection.
– As noted earlier, sketch instances cannot be modified
directly. However, they can be translated, rotated, and
scaled by changing definitions FD1 through FD6 in the
Details view. For this exercise, no reorientation or
rescaling of the sketch instance is necessary.
• Click on “Generate” to apply the new definition.
• In the Details view, rename “Sketch Instance” to
“ArmSketchCopy6”.

Revolve Sketch to Generate 6th
Arm
• Click on the “Revolve” button
• In the Details view, select “Base Object,”
then select ArmSketchCopy6 from the Tree.
Click on “Apply.”
– This will provide the profile (sketch instance)
to be revolved
• In the Details view, select “Axis,” then select
the axis of rotation of the sketch which is
parallel to the Global Y-Axis. Click on
“Apply.” Then, change “FD1, Angle (>0)” to
“30.”
– This provides the axis of revolution, and the
amount of rotation is specified to be 30
degrees.
• Click on “Generate” to complete the
changes.
• In the Details view, change the “Revolve”
name to “ArmRevolve6”

Freeze the “TopBase” Body
• “Freeze” the body by selecting “Tools menu > Freeze”
– Freezing and unfreezing bodies are common operations
when creating multibody assemblies.
• In DesignModeler, there is no distinction between ‘parts’ and
‘assemblies’ as in CAD software, and separate files are not
used to keep track of parts vs. assemblies.
• In fact, DesignModeler has a different concept, which is
called multi-body parts, where bodies in a part will share
coincident nodes on adjacent surfaces when meshed in
Workbench Simulation (instead of using contact elements to
define the interaction between parts).
– Because all parts are created in one database, “freezing”
operations allow the user to specify whether resulting
operations will be merged to the current geometry or
created separately. Frozen bodies cannot be
manipulated, so any further operations will result in new
bodies being created.
– In the next steps, the bottom plate will be created from
an extrusion of a sketch. To prevent the bottom and top
plates from being merged into one body, the top plate will
be “frozen” to prevent any further manipulation to it, and
only the bottom plate will be an active body.
– Frozen bodies will be shown as translucent, although this
can be toggled on/off under “View menu > Show Frozen
Bodies in Transparent Mode”

Create Plane for Second Body
• Rotate the model with the middle-mouse button such
that the bottom face is in view
• Select the bottom face (shown on right) and select the
“New Plane” icon
– Note that, depending on the location of the bottom face
selected, the origin will be positioned differently. This is
because “Use Arc Centers for Origin?” is set to “Yes” by
default, so the center of whichever arc is closest to the
selection point will be used for the origin of the new
plane.
– Make sure that the origin at the center of the model will
be used for the plane origin by choosing “Base Face” in
the Details view, then selecting the inner or outer edges
of the selected face (this will cause the selection to be
near the inner or outer rings, so their center will be used
for the origin).
• In the Details view, click on “Apply” for “Base Face,” if
needed.
– Additional transformations may be applied, as was done
earlier when ArmCopyPlane6 was rotated 60°. However,
for this plane, no further manipulation of the plane is
necessary.
• Click on “Generate” when done.
• In Details view, rename “Plane” to “BaseBottomPlane”.

Create Sketch for Second Body
• Add a new sketch by selecting the “New Sketch” icon in
the toolbar. In the Details view, rename the “Sketch” to
“BaseBottomSketch.” Select the “Sketching” tab from
the Tree to enter Sketch mode.
• In Sketching mode, select “Draw: Circle” and create a
circle with the outer radius equal to the plane boundary.
– When doing this, note that when the cursor is near the
center of the plane, the letter “P” will be displayed. This
is an auto-constraint which will allow the user to easily
set constraints when creating sketches. Make sure that
the center is constrained to the origin of the plane
(“P”=coincident Point constraint), then move the cursor
to the outside diameter of the plane. Note that the “T”
letter will be shown when the cursor is near the outer
diameter. Click again to set the radius with an auto-
constraint equal to the outer radius (“T”=Tangent to
outer diameter).
• Create another circle with a small radius
– Ensure that the center is coincident with the origin of the
plane (with the “P” auto-constraint). Create the outer
radius to be somewhere as shown on right. Note that
the color of the line is teal – underconstrained lines are
shown in teal whereas fully-constrained lines (like the
outer radius) is shown in blue.

Create Sketch for Second Body
(cont’d)
• Select “Dimensions: General” and click on the
teal inner circle sketch. Specify the dimension
location with another left-mouse click.
– The Dimensions section allows users to specify
various types of dimensions. The “General” and
“Semi-Automatic” are the most common options –
the former allows generic specification of
distance, length, or radius dimensions whereas
the latter tries to select all underconstrained
aspects of the sketch.
• Use the “Dimensions: Edit” and select the newly-
created dimension. In the Details view, rename
the “Diameter” to “INNERDIAM”.
– Renaming the sketch dimensions is not required,
but it makes parameter or dimension assignment
(shown later) much easier, if the items have
descriptive names.

Extrude to Create Second Body
• Return to modeling mode by choosing the “Modeling”
tab beneath the Tree.
• Select the “Extrude” icon on the toolbar
• In the Details view, ensure that “Base Object” is set to
“BaseBottomSketch,” the newly defined sketch. If not,
the sketch can be reassigned by selecting the item next
to “Base Object,” selecting the “BaseBottomSketch” from
the Tree, then selecting “Apply.”
• The extrude “Direction” should be set to “Normal,” then
set the “FD1, Depth (>0)” to “1” inch.
– Since the extrusion “Type” defaults to “Fixed,” this
creates an extrusion in the plane’s normal direction at a
fixed distance of 1 inch. Note that, in the Graphics
window, a preview outline of the new extrusion will be
shown.
• Click on “Generate” to create the Extrusion.
• In the Details view, rename the “Extrude” name to
“BaseBottomExtrude”

Provide Dimensional Assignment
– In this step, the inner diameter of the bottom body will be set to
twice the value of the inner radius of the top body
• Select “XYPlane: BaseProfile” sketch. Turn off the solid
geometry and view normal to the sketch.
– The BaseProfile sketch, used to create the top body, will be
shown. Note that it is a cross-section sketch which was revolved
about the Y-Axis. There is a dimension called “INNERRADIUS”
that defines the inner radius of the center hole.
• Turn the solid geometry display back on and select the
“Parameters” icon from the toolbar.
• In the “Parameter/Dimensions Assignment” tab, type
BaseBottomPlane.INNERDIAM=2*XYPlane.INNERRADIUS in the
window. Select the “Check” tab, then the “Close” tab.
– The dimension assignment is done by specifying the Parent
name, then the dimension name. In this case, INNERRADIUS is
from XYPLANE, and INNERDIAM is from the BaseBottomPlane.
Hence, to make the diameter of one equal to twice the radius of
the other, the above expression is entered in the Parameter
window.
• Click on the “Generate” icon.
– Notice that, now, the center hole of the bottom body is the same
diameter (3 inches) as the center hole of the top body. Because
a dimensional assignment is made, if the radius of the top body
hole changes, so will the hole in the bottom body.

Cut Holes in Second Body
• From the Tree, expand HoleCut and select the
HoleProfile sketch. Then click on “Extrude.”
– The same sketch used to create the holes in the upper
body can also be used to modify the lower body. A
sketch is not limited for use for a single part/body.
• In the Details view, change the “Extrude” name to
“BaseBottomHoleCut”. Change “Operation” to “Cut
Material” and ensure that the “Direction” is set to
“Normal”
– Although considered an extrusion, the type of extrusion
can be changed between adding or removing material.
Adding a ‘frozen’ body is also possible, as well as
imprinting faces.
– The direction is selected as “Normal”, but it can be
changed to be a given vector based on the normal of a
selected surface or by vectors defined by selected edges
or vertices.
• Select “To Surface” for the “Type” of cut. For the target
face, select the bottom-most face, as shown highlighted
on the right.
– Extrusions can be performed by specifying a distance or,
in this example, by selecting a surface. If a surface is
selected, this allows the cut to always be a certain depth,
even if the thickness of the second body is changed.

Create Top Cut in LowerBase
• Expand the “2 Parts, 2 Bodies” branch in the Tree.
Rename the second “Body” to “LowerBase”.
Right-click on the LowerBase branch and select
“Hide Body.”
– Renaming bodies makes it easier to differentiate
bodies when brought into Workbench Simulation.
– An inner surface needs to be selected, so
temporarily hiding the second body makes this
easier.
• Select the inner cut, as shown in the figure on the
right (highlighted surface, indicated with an arrow).
Select the “New Plane” button from the Toolbar.
In the Details view, change the “Plane” name to
“BottomCutPlane1”. Change “Transform 1 (RMB)”
to “Offset Z”.
– A new plane based on a selected surface will be
created. This is an outline plane, similar to the
one created earlier for the main extrusion of the
LowerBase body

Create Top Cut in LowerBase
(cont’d)
• Select “Parameters” from the Toolbar. Under the
“Parameter/Dimension Assignments” tab, add
BottomCutPlane1.FD1=XYPlane.CUTDEPTH and click on
the “Check” then “Close” tab.
– The BottomCutPlane1 Z-offset was left at zero earlier.
By adding a dimension assignment, the z-offset was
made to always be equal to the bottom of the surface.
• Click on “Generate” when complete.
• Unhide the LowerBase body by right-clicking the item in
the Tree and selecting “Show Body”
• With “BottomCutPlane1” selected in the Tree, click on
the “Extrude” icon from the Toolbar. Change the
“Extrude” name to “BaseBottomCut1”. Change
“Operation” to “Cut Material” with a “Direction” of
“Normal”. “FD1, Depth (>0)” should be changed to “0.5”
inches. Click on “Generate” when done.
– Instead of using a sketch to create a cut, a plane (outline
plane) created earlier was used. This outline plane is
based on a surface, so, if the surface changes, the
outline plane will be updated accordingly.

Create Bottom Cut for LowerBase
• Select the bottom face of LowerBase body, then create a “New
Plane”. Rename the “Plane” to “BottomCutPlane2”. If needed,
select “Base Face” and adjust the origin to be at the center of the
model, as shown on the right. Then click on “Generate”.
– Recall that, with “Use Arc Center for Origin?” set to “Yes,” the
origin of the new plane will be defined using the closest arc where
the plane was selected. Using “Base Face,” the user can reselect
the face near the centermost circle to use the center as the origin
for the new plane.
• Enter sketching mode by selecting the “Sketching” tab in the
Tree. Create a circle coincident with the origin (“P” auto-
constraint symbol should be shown), then dimension the circle
with a 7 inch diameter.
– Entering sketch mode will automatically create a new sketch (if not
previously defined) on the selected base plane (or surfaces).
– Creating and dimensioning a circle uses the same steps as done
earlier in creating the main extrusion of LowerBase.
– If the “P” coincident-point auto-constraint is hard to differentiate
with the “C” coincident-line auto-constraint, turn off the line select
filter from the toolbar (circled on right). Then, only points (i.e., the
origin) will be selectable, and the “P” auto-constraint will be easily
generated.

Create Bottom Cut for LowerBase
(cont’d)
• Re-enter “Modeling” mode by selecting the
appropriate tab from the Tree. In the Details
view, rename the sketch to
“BottomCutSketch2”.
• Select the “Extrude” icon from the toolbar.
• In the Details view, rename the “Extrude” to
“BaseBottomCut2”. Change “Operation” to
“Cut Material.” Respecify the “Direction” to
“Reversed,” with a fixed distance (“FD1,
Depth (>0)”) of “0.3” inches. Click on
“Generate” when done.

Create First Bolt Head
• Select the top face of the TopBase body, as illustrated
on the right. Create a “New Plane”.
• In the Details view, rename the “Plane” to
“BoltHeadPlane” and change the “Base Face” such that
the origin is at the center of one of the holes. Click on
“Generate” when completed.
• Select the “Sketching” tab to enter sketch mode.
• Create a circle with a “P” auto-constraint at the origin of
the newly created BoltHeadPlane. Dimension this to
make the diameter equal to “1.2” inches.
– Recall that if the “P” auto-constraint symbol does not
readily appear, change the selection filter to points only.
This makes it easier to have the coincident point “P”
auto-constraint, as only existing points are now
selectable.
• Re-enter “Modeling” mode, and rename the sketch to
“BoltHeadSketch”.

Create First Bolt Head (cont’d)
• Select the “Extrude” icon. In the Details view, rename
the “Extrude” to “BoltHead” with a fixed depth of “0.2”
inches in the normal direction. Click on “Generate”
when done to create the bolt head.
– Note that a new body is created since TopBase is a
frozen body.
• Hide the solid model geometry by toggling off the
“Display Model” icon from the toolbar
• Select BoltHeadPlane and create a “New Sketch”.
Rename this “Sketch” to “BoltShaftSketch.”
– A new sketch to define the bolt shaft will be created
• Enter “Sketching” mode by selecting the tab below the
Tree.

• Create a similar circle as done earlier for the bolt head
with “Draw: Circle” and a “P” auto-constraint at the plane
origin.
• Dimension the diameter with “Dimensions: General”.
Rename the dimension with “Dimensions: Edit”, and
enter “BOLTSHAFTDIAM” for the “Diameter” in the
Details view.
• Open the “Parameters” window from the toolbar. Under
“Parameters/Dimension Assignments”, enter
BoltHeadPlane.BOLTSHAFTDIAM=TopBasePlane.CUTDIAM
ETER-0.1 to specify the bolt diameter to have a 0.1 inch
clearance compared with the hole. Click on the “Check”
tab to verify the result of the dimension assignment, then
click on the “Close” tab.
– After specifying the dimension assignment, the
BOLTSHAFTDIAM parameter will have a “D” next to it in
the Details view, indicating that it is a driven dimension.

• Re-enter “Modeling” mode by selecting the tab below the Tree.
With BoltShaftSketch selected, click on the “Extrude” icon from
the toolbar.
• In the Details view, change “Extrude” to “BoltShaft”. Specify the
extrusion “Direction” as “Reversed”. For “Type”, change to “To
Surface”. For the “Target Face,” select the bottom-most surface
of LowerBase, as shown on the right. Click on “Generate” when
done.
– In this case, instead of creating an extrusion of a fixed distance,
existing geometry is used as a reference point for the extrusion
depth. In this way, if the depth of the TopBase or LowerBase
bodies change, so, too, will the bolt shaft.
• To copy the bolt, select “Create menu > Body Operation”
• In the Details view, change “Type” to “Copy”. For “Bodies”, select
the newly-created bolt body. For “Source Plane”, select
“ArmCopyPlane1” from the Tree. For “Target Plane,” select
“ArmCopyPlane2”. Click on “Generate” to create the new copy of
the bolt.
– Although ArmCopyPlane1 and ArmCopyPlane2 may not lie on the
same plane as the bolt body, these two planes are rotated 60°
from each other along the same axis of revolution. Hence, these
two planes can be used as a way of copying the bolt body 60° to
another hole location.

Copy Bolt Bodies
• Rename the “Body Operation” to “Bolt Copy 2”
• Copy the two bolts again by selecting “Create menu >
Body Operation”. Specify “BoltCopy34” as the “Body
Operation” name. Change “Type” to “Copy”, and for
“Bodies,” select both bolt bodies. The “Source Plane”
should be “ArmCopyPlane1”, but specify the “Target
Plane” as “ArmCopyPlane3”. Click on “Generate” to
create bolts #3 and #4.
– In the previous step, ArmCopyPlane1 and
ArmCopyPlane2 were used. In this case, because a
copy of both bolts are done, a rotation of 120° needs to
be specified, so ArmCopyPlane3 is used instead for the
target plane.
• Repeat the above step to create bolts #5 and #6.
– This is done in a similar manner as above, although the
specified bodies will now be the newly-copied bolts #3
and #4.
• In the Tree, expand the “8 Parts, 8 Bodies” menu and
rename the bolts as “Bolt1” through “Bolt6”
– The resulting assembly should be similar to the one
shown on right, with all bodies named accordingly

Defeaturing and parameterizing

The model
Load the Design Modeler file
“DMQuickIntroDefeaturing.agdb”
– Start ANSYS Workbench
– Choose “Empty Project”
– Select “Browse” under “Link to
Geometry file”
– Browse to
DMQuickIntroDefeaturing.agdb
– Click “Open”
– Click “Generate” to refresh the
model
This assembly is a Autodesk Inventor
part which was attached in Design
Modeler.
We will perform many operations on this part:
•Body Delete
•Face Delete
•Fill
•Bodies merging
•Face imprint

Model Import
• We now explain how the model was imported in ANSYS
Workbench – This is just an information, not a step you have to
perform.
Starting from the CAD system (Autodesk Inventor in this case), the
user just goes to “ANSYS 9.0” menu item and select “Workbench”

Model import (cont’d)
This dialog appears. Select “Empty project”
The geometry is shown under the “Link to active CAD geometry” item.
Click on the file name
Finally create a New geometry based on the
CAD part. Once Design Modeler has started,
select the appropriate length unit and click the
“Generate” button to import your model.
Note: if you start from a non-associative format (parasolid, sat, Catia…), the starting point would be a
“Link to geometry file” (dashed pink ellipse above) instead of the active CAD file. The next steps remain
unchanged.

Steps to be performed
1. Remove body with “Body operation”
2. Remove holes with “Face Delete”
3. Remove fillets or chamfers with “Face
Delete”
4. Move bodies with “Body operation”
5. Create a parametric feature with “sketch”
and “extrusion”

Removing unwanted bodies
Select Create->Body Operation
Click on the four bodies marked with
a cross on this picture (hold CTRL to
select multiple bodies at the same
time)
Make sure the type option of the tool
is set to “Delete”
Click “Generate”
χ χ χ
χ

Removing holes – Face delete
Freeze the full assembly (Tools ->
Freeze).
We will now remove the holes of the
leftmost plate
Unfreeze the left plate (Tools-
>Unfreeze then select left plate)
Choose Create->Face Delete
Select the inner holes faces as shown
right (green highlighted)
Click “Apply” in the tools options.
Click “Generate” to get this

Removing fillets and chamfers
Freeze the full assembly (Tools -> Freeze).
We will now remove the fillets and
chamfers out of the circled part
Unfreeze the circled part (Tools->Unfreeze
then select part)
Pick one face of the part and press RMB.
Select “Hide all other bodies”
Choose Create->Face Delete
Select the two fillets faces and the chamfer
at the bottom
Click “Apply” in the tools options.
Click “Generate” to get this
Finally click RMB and select “Show all
bodies”

Merging objects – Partial unfreeze
Another interesting feature of
DM concerns the ability to
merge parts that have
coincident surfaces.
Let’s try on the yellow parts
shown on the right
Unfreeze the two parts (Tools-
>Unfreeze then select both
parts – Hold CTRL key for
multiple parts selection)
Make sure the “Freeze others”
is set to “yes”
Both parts are now merged into
a single one

Adding a parametric feature
We will now add a circular
imprint to the model, whose
diameter will be
parameterized. This kind of
imprint is useful to apply
load on a specific area that
does not belong to the
original CAD model
First select the face as
shown on the picture, then
choose “Sketching” under
the tree view (the face
contour now appears as a
black dotted line)
Click the “look at sketch
icon” to get a correct view
of the working plane

Adding a parametric feature (cont’d)
Draw a circle on the surface as
shown here.
Go to “dimensions”, click on
“General” then pick the circle.
It automatically adds a
diameter dimension to the
model.
You can edit the value of the
diameter in the option window.
Using horizontal and vertical
dimensions let you
parameterize the location of the
circle based on the sketch
main axis. The dimensions can
then be changed as we did for
the diameter.

Adding a parametric feature (cont’d)
Click the “Extrude” icon
Set the options as shown.
Make sure you select only
the concerned body.
Click generate. The top
surface now has the imprint
on it
If you click on “Sketch 2”
under the Extrude object in
the tree, the dimensions are
shown in the options
dialog. You can change the
value of the dimensions
and then update your
model by clicking
“Generate”

Handling thin models

The model
“DMQuickIntroThinModels.agdb”
Geometry file”
– Browse to
DMQuickIntroThinModels.agdb
Modeler.
We will transform this solid model
into a thin model.

Model thicknesses
6.5mm
5mm
13mm
10mm

Understanding the basics of Thin/Surface
feature
Let’s take a single thin body with 6.5mm thickness and go through
various options to get a single surface out of the solid
We consider here that the green face is one face we would like to
keep (this could be the opposite one as well)
One face kept and translated inward by half the thickness
One face kept and translated outward by half the thickness

Thin/Surface feature
• This feature can be used :
– to thicken a surface in order to create a
volume
– to hollow a body

Extracting surface bodies
Freeze the model (Tools-
>Freeze)
Unfreeze the 3 plates with
6.5mm thickness (shown in
solid on the picture)
Pick one face of each solid
Select the “thin/surface”
Feature and set the options
as shown
Click generate

Extracting surface bodies (cont’d)
Freeze the model (Tools-
>Freeze)
Unfreeze the tube with 5mm
thickness (shown in solid on the
picture)
Pick the internal or external faces
(you can pick one face and use
the “Extend Selection” tools with
“Extend to limits”)
Select the “thin/surface” Feature
and set the options as shown
Click generate

Extracting surface bodies (cont’d)
Repeat the previous operations with the last two solid bodies to get the model
shown below

Extending surfaces
We will now extend the surfaces
to touch.
Select the Surface Extension tool
(Tools->Surface extension)
Pick the edge of the surface you
want to extend as shown on the
picture
Select the face to extend to (you
could also specify a distance)
Click generate
Select the edge to extend
Target face

Extending surfaces (cont’d)
You can also select multiple
edges and multiple surfaces
in a single operation.
Select the Surface Extension
tool (Tools->Surface
extension)
Pick the edges as shown
here
Select the faces of the tube
Click generate
Select the three lines for each blade
Select the 5 faces of the tube (planes and fillets)

Extending surfaces (cont’d)
You can also
extend the tube to
the largest
surface.
The final result is
shown here

Joining surfaces
If we stop at this stage and
mesh the resulting surfaces,
we get a mesh similar to the
one shown on the right.
There is no connection of any
kind between the surfaces so
all parts are mesh totally
independent from each other.
Using the “Joint” feature of
Design Modeler will help
solve this issue.

Joining surfaces (cont’d)
Select the “Joint” Tool (Tools->Joint)
Select the tube, the largest surface and
the bottom one then click “Apply” in the
tool options. Make sure “Share
Topology” is set to “Yes”.
Click Generate
Clicking on the joint feature just created
in the construction tree shows green
lines wherever a connection between
surfaces exists.
The surfaces have now imprints
corresponding to their intersections.
We will also form a new part with these
3 surfaces, so that they share common
nodes at the created intersections.
Select “Form new part” from the Tools
menu, pick the three bodies and
generate. The bodies are grouped under
a “Part” in the tree

Joining surfaces (cont’d)
The mesh now shows the common boundaries (in green on the picture)

Automated Mid Surfacing
(available from DesignModeler 10.0)

The model
“DMQuickIntroMidSurface.agdb”
Geometry file”
– Browse to
DMQuickIntroMidSurface.agdb
Modeler.
We will transform this solid model
into a thin model using the mid
surfacing tool.

Extracting surface bodies
Select the “Mid Surface tool” (Tools-
>Mid-Surface)
In the tool options, select “Automatic”
for the selection method
Set minimum threshold to 0.1mm and
maximum threshold to 15 mm (doing
this, you set the extreme values for
detecting face pairs – in other words,
the minimum and maximum sheet
thickness to work with)
Then select “Yes” for “Find face pairs
now”

Face pairs identification
The 20 face pairs found are shown in blue.
Now click on generate to extract the mid surfaces

First result
This extraction also returns a few non desired faces corresponding to the holes

Removing face pairs
In the tree, click the RMB
on “Midsurf” item and
select “Edit selections”.
This reactivates the
options
Click on “Face pairs”
In the main window, click
RMB then “Remove face
pairs”

Removing face pairs – cont’d
Click each of the fillets near to the holes – You have to remove 7 pairs (5 are shown here, the two missing
are near the green circled one)
Click “Apply” in the options then the “Generate” button

Final extraction
The undesired faces are now removed. If you go over the surface bodies in the tree, you will
see that the thickness has automatically been affected to each of the bodies.

Surface extension and joining
• You now can extend and join the surfaces
as shown in the previous tutorial.
Instructions are not repeated here. Click
on this link to get back to the previous
tutorial

Slicing

The Model
“DMQuickIntroSlicing.agdb”
– Select “Browse” under
“Link to Geometry file”
– Browse to
DMQuickIntroSlicing.agdb
The goal of this tutorial is to
show you how to use slicing in
order to get a swept mesh of
this part.
The default mesh obtained on
such a part is a tetra mesh as
shown.

Slicing: what does it mean?
• Slicing is an operation that will allow you to split a solid into
smaller parts.
• The purpose of slicing can be meshing with hexa (swept)
elements but also affecting multiple materials in various
areas of the model
• Three type of slicing are available:
– Slice Off Faces: a set of faces is selected and a slice will be
generated to create a solid from these faces
– Slice by plane: a plane is chosen and the part is sliced by
this plane
– Slice by sketch: you can use sketches to draw an arbitrary
shape that will be used for slicing (using extrusion or revolve
features). This last type is not addressed in this tutorial.

Slicing Off faces
We start slicing the part using the faces of
the rightmost feature
Any slice operation can only be performed
on frozen bodies. So we freeze everything
(Tools->Freeze)
Select all the faces of the feature as shown
Select Create->Slice and “Apply” to use the
previously selected faces
Click generate: your model has now two
parts.
Since we want to keep a unique body, we
will form a new part: select Tools->Form
new part, pick all bodies, click “Apply” and
“Generate”
The construction tree should look as
indicated
Now, if we mesh this new part, we have the
result shown to the right. This is a mix of
tetra and hexa elements.

Now, the part will be sliced parallel to the XY
plane, at two altitudes shown by the green
faces on the top left picture. We will also
slice it along the third green face
perpendicular to the two first.
To slice the part at this level, we need
creating a plane corresponding to these
faces. To do this, pick one of the face, then
the “Plane” icon, then click “Generate”. The
planes look like the right top picture.
Once the three planes have been created,
select the Slice tool (Create->Slice), set the
options to “Slice by plane”. Select one of the
plane as cutting plane. To do this, click on
“Base Plane”, then choose the plane name in
the construction tree then click “Apply”.
Finally, “Generate”.
Repeat the previous step for the 2 other
planes.
You now have 8 bodies that you can group
into a new part.
We still have one solid in the part that is not
swept.
Slicing by plane

Slicing by plane (cont’d)
To finalize the model, we
will use two additional
slices, based upon the
two green faces shown
on the right.
Create the planes
corresponding to these
two faces and slice the
part.
You now have 10 bodies
that you can group into a
new part.
And the mesh is totally
swept!

Internal volumes

The Model
“DMQuickIntroInternalVolume.
agdb”
– Select “Browse” under
“Link to Geometry file”
– Browse to
DMQuickIntroInternalVolu
me.agdb
The goal of this tutorial is to
show you how to create the
internal volume of an hollow
body.

Filling a part
Select the “Fill” Tool (Tools-
>Fill).
Select all the internal faces of the
body as shown here in green and
click “Apply”. You must have 10
faces selected
You now have 2 bodies: the
original one and the internal
volume.
You can delete the outer body
(Create->Body Operation)
Note that the outer body needs
be frozen before creating the
internal one.

Enclosures

The Model
“DMQuickIntroIEnclosure.agdb”
Geometry file”
– Browse to
DMQuickIntroEnclosure.agdb
The goal of this tutorial is to show
you how to create an enclosure
around this model.
In this case, the goal is to create
the air surrounding the motor for a
electromagnetic simulation.

Creating the enclosure
Internal view of the enclosure
Select the “Enclosure”
Tool (Tools->Enclosure)
Set the options as shown
here (note that you can
choose other enclosure
shapes)
If we cut the enclosure,
we can see that it really
fills all the gaps between
the various solids of the
original model.

Dm quick evalguide design of component

More Related Content

Similar to Dm quick evalguide design of component (20)

Recently uploaded (20)

Dm quick evalguide design of component

Editor's Notes