WORKSHOP 4MID-SURFACE EXTRACTION EXAMPLE презентация

represents a junction box, this workshop involves creating surfaces at mid-plane throughout the solid. Then, these mid-surfaces are meshed with 2D quadrilateral elements. From the 2D mesh, a complete analysis model is created, an analysis is performed, and results viewed.

file, j_box.xmt
Create a group that the midsurfaces will be placed in, midsurfaces. Use Group/Create.
Create midsurfaces for the junction box. They will be in group midsurfaces.
Post only the group with midsurfaces.
Edit the gussets created by the midsurface operation. This involves eliminating the long thin tops of the gussets.
Associate the edges of the gussets with the midsurfaces that represent the junction box.
Paver mesh the midsurfaces.
Equivalence the nodes to connect the 2D quad4 elements.
Apply distributed loads to midsurface surfaces.
Constrain select points of midsurface surfaces.
Create material and element properties.
Check the load case.
Submit the finite element model to MSC.Nastran for analysis.
Post process the results from MSC.Nastran

database called
midsurface.db and set the model
preferences.
a. File / New.
b. Enter midsurface as the file name.
c. Click OK.
d. Set the Tolerance to Based
on Model.
e. Set Analysis Code and
Analysis Type to
MSC.Nastran and Structural,
respectively.
f. Click on OK.

parasolid.
a. File / Import.
b. Select j_box.xmt and click on
Apply.
c. Click OK when import
summary appears.
d. Click on the Iso 3 View icon.

the Junction Box should look like when observing it from the ISO3 view. To better visualize the object, click the smooth shaded icon. Then, go back to the wireframe view. It is easier to work with this display.

Group / Create.
b. Enter midsurface for New
Group Name.
c. Make sure Make Current box
is checked.
d. Click on Apply.
e. Click on Cancel.

/ Surface /
Midsurface.
b. Select Automatic icon.
c. Enter 0.1251 for Max. Thickness.
d. Click on Solid List, then on
the solid.
e. Click Apply (If Auto-Execute
is checked do not click on
Apply).

/ Post.
b. Select midsurface
from Select Groups
to Post.
c. Click on Apply.
d. Click on Cancel.

Trim.
b. Check Delete Sliver Surface.
c. To select a surface to trim,
click on any of the gussets.
d. To select the trimming edge,
click on the sloped edge of gusset
e. Repeat procedure for the seven
remaining gussets

the
junction box midsurfaces.
(Need to associate the gussets
to the junction box to make the
quad meshes congruent during
the Paver mesh.)
a. Geometry: Associate /
Curve / Surface.
b. Associate vertical edge
of gusset to adjacent
surface. Click Apply.
c. Associate bottom edge
of gusset to bottom of
junction box. Click
Apply.
d. Repeat for all remaining
gussets.

if Auto Execute is checked,
it is not necessary to click Apply.

after all of the gusset edges have been associated to the junction box midsurfaces. The associated edges are indicated by the triangles.

of the solid.
a. Elements : Create /
Mesh / Surface.
b. Make sure Quad,
Paver, and Quad4 are
selected.
c. Remove check for
Automatic
Calculation and enter
0.1875 for the Global
Edge Length.
d. Click on Surface
List. Select all the
surfaces by dragging a
box around the entire
object.
e. Click Apply

*Surface List should be: Surface 1:13

of the
elements at geometric
boundaries are connected,
they have free edges. This
problem will be remedied with
the Equivalence command.
a. Elements: Verify /
Element /
Boundaries.
b. Check Free Edges
c. Click Apply.

Yellow lines indicate free element edges.

and show
that elements at the internal
edges of the junction box are
connected.
a. Elements : Equivalence /
All / Tolerance Cube.
b. Click Apply.
c. Elements : Verify / Element
/ Boundaries
d. Check Free Edges.
e. Click Apply.

Now all free edges shown are desired free edges

model.
a. Loads/BCs : Create / CID
Distributed Load / Element Uniform
b. Enter CID_Distributed_Load in
New Set Name.
c. Make sure to select 2D under
Target Element Type.
d. Click Input Data…
e. Enter <0 100 0> in Surf Distr Force.
f. Click OK.

Click Select
Application Region…
b. Click on Edge icon.
c. Click the edge of any
small hole on the end of
the junction box at the
greatest Y-coordinate.
d. Click Add.
e. Repeat c and d for
remaining three holes.
f. Click OK.
g. Click Apply.

Application Region should
include edges
Surface 4.5 4.6 4.7 4.8

junction box midsurface with the CID distributed loads.

base of the junction box, i.e.
constrain the four holes on the bottom
so that they are fixed.
a. Loads/BCs : Create / Displacement /
Nodal.
b. Enter Fixed for New Set Name.
c. Click Input Data…
d. Enter <0 0 0> for Translations.
e. Enter <0 0 0> for Rotations.
f. Click OK.
g. Click Select Application Region.
h. Select Select Geometry Entities
and click on Curve or edge icon.
i. Select the edge of any hole of the base
and click Add.
j. Repeat procedure for remaining three
holes and Click OK.
k. Click Apply.

Application region should include
Surface 2.21 2.22 2.23 2.24

what the object should look like when constraints are applied. You can observe that the constraints on the bottom four holes of the junction box are all six degrees of freedom.

the
model.
a. Materials : Create / Isotropic
/ Manual Input.
b. Enter Aluminum under
Material Name.
c. Click Input Properties.
d. Enter 10E6 for Elastic
Modulus and 0.3 for Poisson
Ratio.
e. Click OK.
f. Click Apply.

Properties : Create / 2D / Shell.
b. Enter 2D_shell in Property Set
Name.
c. Make sure Homogenous and
Standard Formulation are
selected.
d. Click Input Properties…
e. Click on Mat Prop Name icon and
Select Aluminum from Select
Material.
f. Enter 0.125 for Thickness.
g. Click OK.
h. Under Select Members select the
entire object by dragging a box
around the junction box.
I. Click Add and then click Apply.

Application region is surface 1:13

load case Default from
Select Load Case to Modify.
c. Check to see that the CID
distributed load and the
constraint are assigned to the
default load case.
d. Click Cancel.

: Analyze / Entire
Model / Full Run.
b. Click on Translation
Parameters.
c. Select XDB and Print.
d. Click OK.
e. Click Subcases.
f. Make sure the default subcase
is selected.
g. Click Apply and Cancel.
h. Click Subcase Select…
i. Make sure subcase Default is
selected and click OK.
j. Click Apply.

It may be helpful to check
each window, in order to
become familiarized with each
of the the various forms.

: Access Results / Attach XDB / Result Entities.
b. Click Select Results File…
c. Select the midsurfaces.xdb
file.
d. Click OK.
e. Click Apply.

by
the load.
a. Results : Create /
Deformation.
b. Select Default, Static
Subcase under Select Result
Case(s).
c. Select Displacements,
Transitional.
d. Click Apply.

Here the deformation due to the CID Distributed loads is illustrated.

erase the geometry to get a better
illustration of the load effects.
a. Click on the Display
Attributes icon.
b. Remove the check from the
Show Undeformed box and
from the Show Title box as
well.
c. Click on the Plot/Erase icon.
d. Click on Erase under
Geometry.
e. Click OK.

stress for
the junction box surface model.
a. Results : Create / Fringe
b. Select result case.
c. Select Stress Tensor,
and Quantity : von Mises.
d. Click Apply.

This illustration shows a combined representation of the deformation and von Mises stress of the junction box mid surface model.

a better
fringe plot.
a. Click on the Display Attributes
icon.
b. Change the Display to Element
Edges.
c. Uncheck the Show Title box.
d. Click Apply.

fringe plot along with the deformation plot.