Introduction to StressCheck®

These slides complement the Getting Started Guide of StressCheck®. The

step-by-step procedures of importing a Parasolid file, creating the mesh,
entering input data, solving and post-processing are illustrated.
Manual construction of a mesh for a parameterized plane elastic body and
specification of parameterized loading are illustrated on the basis of
Exercise 4.3.9.
 Introduction to StressCheck
• Import a Parasolid file
– Start StressCheck and make sure that the Reference/Theory
Toolbar is displayed.
• It is good practice to display all toolbars: Click on View and
select ALL Toolbars. We will not need the Part/Assembly
Toolbar, turn it off.
– Select Planar / Elasticity / mm/N/sec/C
• The type of analysis and units must be consistent with the
Parasolid file.
– Select File > Import
• A reminder will be displayed. If you did not update the units as
indicated above, do so before importing the file.
• Using the browser import your Parasolid file.
• In this example we will import NotchedBeam1.x_t

2
 Create an automesh (1)

• You should see the Parasolid sheet body

shown below.

• Select the icon or click Alt – I. This will

take you to the StressCheck Input dialog box.
• Click on the Mesh tab and set the scroll boxes
at the top display to: Create/Mesh/Auto.

3
 Create an automesh (2)
• You will see the dialog box
shown on the right.
• Complete as shown and
click on Accept. This means
that you have accepted the
default meshing parameters.
A meshing record will be
created.
• Click on Automesh. This will
produce the mesh of 6-node
isoparametric elements
shown in next slide.

4
 Create an automesh (3)
• The mesh shown below will appear

To zoom left click on the icon and drag

with the right button held.
Zooming on the circular fillets you will see that
the 90 – degree circular sector is
approximated by only one element.
Smaller elements will be created at the fillet if
you select Create / Mesh / Curve then select
both fillets, use default values in the mesh
interface, Accept > Automesh

5
 Enter input records (1)

• The refined mesh is shown below

• Assign the thickness

– Select > All Elements
– Enter the thickness (4.0)
– Accept

6
 Enter input records (2)

• Material properties are entered in two steps.

Define Assign

7
 Enter input records (3)

• Load records
– Let us enter uniformly distributed loads
Select curve

Assign name of the load record

Specify direction

Specify component and

value then Accept

8
 Enter input records (4)

• Constraint record
– Let us enter a rigid body constraint record as
shown on the shown in the figure on the left.
Select the two corner points as shown
below and the rigid body constraint will
be created automatically (no need to click
on Accept).

Rigid body constraint

9
 Enter input records (5)

• Solution record
– Associates the names of a
constraint record (RB) and
load record (UDL) with the
name of a solution (SOL).
– Click on Accept to create
record.

10
 Recommended exercise
• In the preceding steps we first created the
mesh then entered the input data.
• We could have entered the input data then
created the mesh.
– In general it is good practice to associate the load
and constraint records with geometric objects
(points, curves) rather than with meshing objects
(nodes, element edges or edge curves).
• Enter the input data first then create the
mesh.
– The input data can be entered in any order.

11
 Solution (1)

• Click on the icon or press Alt – S

– You will see the solution tab below. Fill in the
range of p values (in this case 1 to 8) and click on
Solve.

12
 Solution (2)
• You will see the second solution tab shown
below.
– Complete as shown and click on Solve.

13
 Postprocessing (1)

• Click on the icon or press Alt - X

• Select the Error tab, and complete the solution ID
and run numbers, then Accept.
– You will see a graph showing a the relative error in energy
norm in the Chart tab, and you can select to see the tabular
data in the Table tab.
p N PE beta % err.
Relative error in energy norm 1 415 -1.199360E+06 0 11.72
2 1527 -1.215952E+06 1.93 0.95
3 3335 -1.216057E+06 2.12 0.18
4 5839 -1.216061E+06 2.51 0.04
5 9039 -1.216061E+06 2.5 0.01
6 12935 -1.216061E+06 2.25 0.01
7 17527 -1.216061E+06 2.08 0
8 22815 -1.216061E+06 2.08 0

14
 Postprocessing (2)

• Click on the Plot tab

– Select the solution record and run number that you wish to
plot. Here p=8 was selected.
– For a contour plot click Fringe.
– Select the function to be plotted. Here we selected Seq (the
von Mises stress).
– Specify the number of midsides. This determines the
resolution of the data plot. Here 5 was selected.

15
 Postprocessing (3)
• Click on the Min/Max tab
– Select the solution records p=1 to p=8.
– Select the function of interest. Here we selected S1 (the first
principal stress).
– Specify the number of midsides. This determines the search
grid. Here 9 was selected. Click on Accept and you will see
the graph below.

16
 Manual construction
• Manual construction is recommended when a
part is to be analyzed repeatedly, as in a
design study.
– The part is characterized by a set of parameters.
– Example: See Exercise 4.3.9 in the text.

17
 Manually constructed mesh

• Example of a manually constructed mesh

– The elements and the nodes are shown below

– The name of the input file is NotchedBeam.sci

– To read the input file click on the icon then
select the filename and double click on it.
– We will construct this mesh step by step.

18
 Enter the parameters

• Click on the icon and select the parameter

tab. Enter the parameters.
– Note that M2 depends on M1 and V. – Why?

19
 Construct geometrical objects (1)
• Click on the icon and
select the geometry tab
– Select Create > Rectangle
> Locate
• Enter parameters a, b as
shown.
• Click Accept, and the
rectangle will appear.
– Center rectangle by
clicking on the icon
• The global coordinate
system is in the lower left
corner of the rectangle.

20
 Construct geometrical objects (2)
• Create a second rectangle
using the parameters
shown on the right.
– The result is shown below.

21
 Construct geometrical objects (3)
• Create fillets
– Specify radius (rf).
– Click on each of the
intersecting lines where you
want the fillet inserted.
– Points are created at the
ends of the circular arc.

22
 Construct mesh (1)

• To construct a mesh first create the nodes

then create the elements. Select Mesh.
- Nodes can be created in several ways. We will
create nodes by
- locating them where points already exist
Create > Node > Point select the point(s) where you
wish to locate nodes click accept
- the mid-point method
Create > Node > Midpoint click on the two nodes, a
node will be created in the mid-point
- projection
Create > Node > Projection select the node(s) you wish
to project. Hold the Ctrl and Shift keys then click Accept.

23
 Construct mesh (2)
• After turning off the Point and System
displays you should see the figure below.
– The labels pt, mp and pr indicate the point, mid-
point and projection methods
pt pt
pr pr pr pr pr

mp
pr mp mp pr
pt pt
pr
pt
pt

pt

24
 Construct mesh (3)
• Create elements:
– Create > Quadrilateral >Selection
– Click or select any four nodes. A quadrilateral
element will be created.
– Alternatively hold Ctrl - Shift then bring the cursor
near the centroid of the element you wish to
create. A green outline will appear. Left click and
release Ctrl – Shift.

25
 Check mesh & refine
• Check for errors in meshing
– Check > Edge > Free Edge. The free edges will
be highlighted. Troubleshoot if necessary.
• Refine (read Example 7.3.1 in the text)
– Click on the tab h-Discretization
– Select > Edge Curve > Simple Graded
– Name (any name), Layer (leave blank), Midsides
(1), Grading (0.2)
– Click on any edge on the cut-out, Accept, Mesh.

26
 Define formulae
• Click on the icon
– Define formulae for the
normal traction on the right
(TNR), normal traction on
the left (TNL) and the
shearing traction (TT) as
shown on the right.
• Create a centroidal
coordinate system
– Geometry > Create >
System > Locate
X = 0, Y = b/2, Z = 0

27
 Apply load

• Click the Load tab

– Select > Any Curve > Traction
– Click on the curve(s) to be
loaded
– ID: Any name (Tractions)
– Direction: Norm/Tan
– System: Select the system
created in the previous step
– Normal: Formula (TNR)
– Tangent: Formula (TT)
– Accept

28
 Check equilibrium
• Rigid body constraints should be applied only
when the body is in equilibrium. – Why?
• To check whether the applied loads satisfy
equilibrium;
– Check > All Elements > Selection > Accept
– A report showing the net force components and
moment acting on the body will appear. These
should be very nearly zero, that is, orders of
magnitude smaller than max(|M1|, |M2|, V).
– If the body is not in equilibrium then there is an
error in input. Trouble shoot.

29
 Solution & post-processing
• Enter the material properties, apply rigid body
constraints and create the solution record.
• Solve p = 1 to p = 8.
• Extract the first principal stress. You will see
the results below. At p=8 S1 = 205.7 MPa
Run DOF Max. S1
1 63 1.9900E+02
2 167 2.0010E+02
3 271 2.1100E+02
4 415 2.1460E+02
5 599 2.0910E+02
6 823 2.0810E+02
7 1087 2.0670E+02
8 1391 2.0570E+02

30
 Modifying the mesh

• Modify the record for h-Discretization so that

Midsides = 2, Grading = 0.3 and click on
Mesh. You will see the mesh shown below:

• Solve again and extract the maximum value

of the first principal stress. At p = 8 you will
find it to be 204. 5 MPa.

31
 Extrude

• If you have access to the Professional Edition

of StressCheck then you can convert this
planar problem to a 3-dimensional one by
extrusion.
• Let us impose constant moment on the
boundaries BC and DA determine the value
of the moment that will cause an out of plane
displacement of 2.0 mm.

32
 Extrusion
• Select Extrude (Reference/Theory
toolbar).
– You you will see the body shown below.

33
 Define the normal traction

• Define formula for the

normal traction Tn
corresponding to a unit
moment.
– Enter the formula shown
on the right.
– Click Accept

34
 Apply tractions
• Apply unit moment
– Select Face Surface, enter ID
(UnitMoment), Direction:
(Norm/Tan), Normal: Tn
Accept.
– Repeat for the opposite side
– Check equilibrium.

35
 Create solution record

• StessCheck automatically
converted the rigid body
constraints to 3D.
• Create a new solution record
– Solution ID (Sol_M)
– Constraint Record (RB)
– Load Record (UNITMOMENT)
• Solve
– Since there are two active
solution records, there will be
two solutions.

36
 Display the deformed configuration

• Plot the deformed

configuration
• Find the maximum
displacement Uz:
– (Uz)max = 4.369E-4 mm
– The moment that will
cause 2 mm maximum
displacement is therefore
M = 4578 Nmm.

37
 Recommended exercises
• Determine the maximum von Mises stress in
the extruded configuration corresponding to the
applied moment of 4578 Nmm and verify that
the relative error is not greater than 2 %.
– Answer: 119.8 MPa.
• Compare the maximum normal stresses
computed for (a) the two dimensional body and
(b) the extruded body loaded in-plane only.
– Answer: (a) 204.5 MPa (b) 189.6 MPa
– Note: For answer (a) see p. 31.
– Note: The location of the maximum is the same for
(a) and (b): x = 112.8 mm, y= 5.88 mm.
38
 Recommended exercises
• Import the file NotchedBeam1.x_t
• Create the parameters

• Create a circle with center (x0,y0), radius r0

• Use Boolean subtraction to create the sheet body;

• Construct an isoparametric mesh (automesh).

39
 Recommended exercises
• Using the default parameters you should see a mesh
like this:

• Using the default refinement at the curved boundary

segments, you should see a mesh like this:

• What will happen if you change the parameters that

define the circular hole?

40