Femap Symposium 2015 Sterling, VA – Co-Hosted with SDA, Inc.
FEMAP Freebody Deep-Dive
Femap Symposium Series 2015
April 14, Sterling VA, USA
Unrestricted © Siemens AG 2015
Femap Symposium Series 2015
FEMAP Freebody Deep Dive
Topics
•
•
•
•
•
•
•
•
What is a Freebody?
Recovering Grid Point Forces in NASTRAN
Understanding Grid Point Force Output
Freebodies in FEMAP
Using the FEMAP Freebody Toolbox
FEMAP Freebody Options
Global / Local Modelling with Freebodies
Additional Topics
Restricted © Siemens AG 2015 All rights reserved.
Page 2
ZEN Feb 9-13 2015
Siemens PLM Software
What is a Freebody?
Freebodies provide an insight into nodal forces and moments that are a result of
surrounding finite element entities
• In FEMAP, freebodies can be
used to display a balanced set
of loads on a structure or
calculate the load across an
interface
• Freebodies are commonly used
when modeling practices dictate
that the resulting FE mesh is a “coarse-grid” mesh and is suitable as an
“internal loads” model
• Commonly modeled structures are often too complicated to model in
sufficient detail to obtain useable stresses
• Allows for forces / moments to be extracted for detail stress analysis
• Freebodies are heavily used (but not limited to) in the aerospace industry
Restricted © Siemens AG 2015 All rights reserved.
Page 3
ZEN Feb 9-13 2015
Siemens PLM Software
Recovering Grid Point Forces in NASTRAN
Enabling GPFORCE Output in NASTRAN Case Control
• Turning on the NASTRAN GPFORCE
case control request is required to
take full advantage of the FEMAP
Freebody Tool
• Analysis Manager
• Master Requests and Conditions
• Output Requests
• Force Balance
• GPFORCE requests can return a large
amount of data, so this option
is not enabled by default
Restricted © Siemens AG 2015 All rights reserved.
Page 4
ZEN Feb 9-13 2015
Siemens PLM Software
Recovering Grid Point Forces in NASTRAN
Enabling GPFORCE Output in NASTRAN Case Control
• FEMAP can work with a reduced set
of data including applied load (OLOAD),
constraint force (SPCFORCE), and
constraint equation (MPCFORCE)
• This is generally not recommended
unless only a generic freebody
display of the entire structure is
all that’s required
• Additionally, care should be taken when
not requesting GPFORCE data for
the entire model
Restricted © Siemens AG 2015 All rights reserved.
Page 5
ZEN Feb 9-13 2015
Siemens PLM Software
Understanding Grid Point Force Output
NASTRAN F06 Output
• When the results destination is set to “Print Only” or “Print and PostProcess”
GPFORCE data can be viewed in the F06 file
• Note that it is still recommended to read GPFORCE data into FEMAP from
the OP2 file, not the F06 file
• Search for “G R I D P O I N T F O R C E B A L A N C E”
G R I D
POINT-ID
0
0
ELEMENT-ID
1
1
1
1
2
2
2
2
2
3
3
3
3
3
267
268
267
268
269
270
269
270
271
272
SOURCE
F-OF-SPC
QUAD4
QUAD4
*TOTALS*
QUAD4
QUAD4
QUAD4
QUAD4
*TOTALS*
QUAD4
QUAD4
QUAD4
QUAD4
*TOTALS*
P O I N T
T1
4.169596E-02
1.213303E-01
-1.630262E-01
9.436896E-16
-7.904667E-01
-3.752280E-01
5.058178E-01
6.598768E-01
-1.798561E-14
-2.833224E-01
-2.021358E-01
1.617432E-01
3.237150E-01
1.049161E-14
F O R C E
T2
1.031393E+00
5.287078E+00
-6.318471E+00
-6.306067E-14
-1.515594E+02
-1.348000E+02
1.277458E+02
1.586136E+02
-1.136868E-12
-7.450614E+01
-4.297056E+01
5.205509E+01
6.542161E+01
8.540724E-12
B A L A N C E
T3
-5.078434E+01
-1.944031E+01
7.022465E+01
2.557954E-13
3.756228E+02
-4.464662E+02
2.504629E+00
6.833877E+01
7.389644E-13
3.083269E+02
-3.489907E+02
-2.303685E+01
6.370063E+01
-2.700062E-13
R1
0.0
2.078351E-03
-2.078351E-03
1.934217E-16
1.975718E-01
1.780457E-01
-1.799477E-01
-1.956698E-01
6.383782E-16
1.501767E-01
1.569770E-01
-1.572558E-01
-1.498980E-01
1.665335E-16
R2
0.0
5.017486E-01
-5.017486E-01
0.0
5.075642E-01
-5.262242E-01
-1.129834E-01
1.316434E-01
1.493250E-14
-1.241496E-01
1.129076E-01
-2.788103E-01
2.900524E-01
-2.886580E-15
R3
0.0
4.834255E-04
-4.834255E-04
-2.333203E-16
1.493221E-02
2.671471E-02
-4.392642E-02
2.279495E-03
5.551115E-17
2.011796E-02
4.146868E-02
-1.574009E-02
-4.584655E-02
8.326673E-17
Restricted © Siemens AG 2015 All rights reserved.
Page 6
ZEN Feb 9-13 2015
Siemens PLM Software
Understanding Grid Point Force Output
NASTRAN F06 Output
• GPFORCE results are listed per grid and include Fxyz (T1, T2, T3) and Mxyz
(R1, R2, R3)
• Results are separated into 4 different categories, plus a summation
• Elemental (discrete; per connecting flexible element)
• Applied (total forces / moments applied on node; single quantity per node)
• F-of-SPC (SPC forces on node; single quantity per node)
• F-of-MPC (MPC forces on node, including both constraint equations and
RBE contributions; single quantity per node)
• *TOTALS* (total summation of all contributions; single quantity per node)
• For the majority of cases, this value should be near zero, indicating
equilibrium at the node
Restricted © Siemens AG 2015 All rights reserved.
Page 7
ZEN Feb 9-13 2015
Siemens PLM Software
Understanding Grid Point Force Output
How GPFO Relates to Structure
• Freebody output can be very dependent on the nodes and elements included
in the summation
• Determining which nodes and elements are to be used is varies based on how
the model was idealized as well as what specific quantity is desired
Restricted © Siemens AG 2015 All rights reserved.
Page 8
ZEN Feb 9-13 2015
Siemens PLM Software
Freebodies in FEMAP
Freebodies in FEMAP exist as creatable objects, like nodes, elements, etc.
• They persist in the database
• This is a huge benefit for recreating freebody displays in the future
• Can help reduce analysis errors and rework
• Any number of freebodies can be displayed simultaneously
• Many tools exist to automate free-body-related tasks, such as creating loads
and substructure modeling
Restricted © Siemens AG 2015 All rights reserved.
Page 9
ZEN Feb 9-13 2015
Siemens PLM Software
Freebodies in FEMAP
FEMAP Freebody Types – There are 3 separate types of freebodies in FEMAP
• Freebody – user selects the elements, FEMAP automatically selects related
nodes. Intended to display a balanced set of loads on a discrete piece of
structure
Restricted © Siemens AG 2015 All rights reserved.
Page 10
ZEN Feb 9-13 2015
Siemens PLM Software
Freebodies in FEMAP
FEMAP Freebody Types – There are 3 separate types of freebodies in FEMAP
• Interface Load – user selects both nodes and elements and FEMAP
calculates a summation of loads and forces across the interface and displays
as a single vector
Restricted © Siemens AG 2015 All rights reserved.
Page 11
ZEN Feb 9-13 2015
Siemens PLM Software
Freebodies in FEMAP
FEMAP Freebody Types – There are 3 separate types of freebodies in FEMAP
• Section Cut – similar to interface load, a summed load across an interface is
displayed and calculated, however node and element selection is automated
by FEMAP. The user selects a “cutting plane”, defined by a plane, vector or a
curve. The cutting plane can be dynamically located within the model
Restricted © Siemens AG 2015 All rights reserved.
Page 12
ZEN Feb 9-13 2015
Siemens PLM Software
Freebodies in FEMAP
Freebody Contributions
• Freebody contributions in FEMAP are split into six categories
• Applied – represents applied loads
• Reaction – results of SPC forces
• MultiPoint Reaction – results of MPC forces
• Peripheral Elements – effects of elements
surrounding selected elements
• Freebody Elements – effects of elements
selected by the user or by FEMAP
• Nodal Summation – nodal summation values
from the solver, not FEMAP calculated values
• Default contributions are Applied, Reaction, MultiPoint Reaction and
Peripheral elements
• This provides forces and moments acting on the selected structure
Restricted © Siemens AG 2015 All rights reserved.
Page 13
ZEN Feb 9-13 2015
Siemens PLM Software
Freebodies in FEMAP
Freebody Result Vectors – As previously mentioned, the NASTRAN GPFORCE
request is recommended to fully take advantage of the freebody tool, however
the result quantities may be obtained from several different quantities
Primary
Secondary
Applied
GPFORCE
OLOAD
SPC
GPFORCE
SPCFORCE
MPC
GPFORCE
MPCFORCE
Elemental
GPFORCE
None
Nodal Summation GPFORCE
None
The italicized rows above represent default output requests in FEMAP and are
sufficient for displaying a balanced freebody on the entire structure
Restricted © Siemens AG 2015 All rights reserved.
Page 14
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Accessing the Freebody Toolbox
• The Freebody Toolbox is located in the
PostProcessing toolbox and can only
be accessed when results are present in
the model
Global Settings – These controls affect all
freebodies in the model. Control global display
of freebodies, select output set (tied to contour
and deform) and enable data summation on
nodes
Freebody Settings – These controls are
related to individual freebodies, such as
selecting nodes and elements
View Settings – These are global settings that
affect freebody visualization (symbol sizes,
vector scaling, etc.). Same as found in View
Options (F6)
Restricted © Siemens AG 2015 All rights reserved.
Page 15
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Creating a New Freebody
• In the Freebody Toolbox, new Freebodies are created within the Freebody
Manager
• The New Freebody dialog allows for setup of basic settings, such as freebody
type, vector display, and contribution selection
Restricted © Siemens AG 2015 All rights reserved.
Page 16
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Creating a New Freebody
• Any of the settings applied in the New Freebody dialog can be changed at any
time within the toolbox
Restricted © Siemens AG 2015 All rights reserved.
Page 17
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Accessing Different Freebodies
• Multiple Freebodies can be displayed at any
time however, only a single freebody can be
active at any time within the toolbox
• Use the drop-down menu to change the active
freebody and modify settings
• Display of individual freebodies can be
controlled with the “Is Visible” checkbox as
well as with the Visibility Quick View Dialog
Restricted © Siemens AG 2015 All rights reserved.
Page 18
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Freebody Vector Types
• Depending on the freebody type, there are vector quantities for nodal vectors
and a single total summation vector
• Nodal Vectors
• Displays the summation at each node, based on the selected freebody
contributions
• Available for all freebody types
• Total Summation Vector
• Displays the total summation across all nodes at a pre-defined position.
The selected position does not affect summed force calculations, but will
affect summed moment calculations due to the difference in moment arms
• Available for Interface Load and Section Cut freebodies
• Both force and moment vectors are available and can be individually toggled
• Vectors can be displayed as either components or resultant vectors
• Individual components can be toggled on and off
Restricted © Siemens AG 2015 All rights reserved.
Page 19
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Freebody Vector Visualization
Visibility Quick Toggle Buttons
• All On / All Off
• Forces On/Off
• Moments On/Off
• Toggle between resultant/component
• Select summation location (interface load
and section cut only)
Restricted © Siemens AG 2015 All rights reserved.
Page 20
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Freebody Vector Visualization
Detail Options
• Additional detailed options for visualization
can be found by expanding the Total
Summation Vector and Nodal Vector(s)
nodes
• Select components displayed (Fx, Fy, Fz),
(Mx, My, Mz)
• Select components included in calculation
(interface load and section cut only)
Restricted © Siemens AG 2015 All rights reserved.
Page 21
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Freebody Coordinate Systems
• The selected freebody coordinate system
controls the coordinate system for both nodal
vectors and the total summation vector (if
applicable) for the selected freebody
• Nodal vectors may optionally be displayed in
the nodal output coordinate system
• If no nodal output system was specified on
the node, the default coordinate system used
is the global rectangular system
Restricted © Siemens AG 2015 All rights reserved.
Page 22
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Freebody Mode
• When using “Freebody Mode”, the user selects
elements and FEMAP will automatically select
related nodes
• This mode is designed to display a balanced
set of loads on a selected set of elements
• Entities may be selected manually (default) or
inferred for a selected group
• The default contribution selections will display
forces/moments acting on the selected
elements
Select Elements
Reset Element Selection
Highlight Selected Elements
Restricted © Siemens AG 2015 All rights reserved.
Page 23
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Display of balanced set of loads on wingpost model. All elements in the model
were selected for this display
Restricted © Siemens AG 2015 All rights reserved.
Page 24
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Interface Load Mode
• Interface load freebodies display nodal
vectors for selected nodes as well as a total
summation vector at a selected location
• Unlike freebody mode freebodies, interface
load freebodies are not likely to be in
equilibrium
• In addition to element selection, nodes must
be selected manually – FEMAP does not infer
them based on the selected elements
• When selected entities from a group, both
the nodes and elements of interest must
exist in the group
Restricted © Siemens AG 2015 All rights reserved.
Page 25
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Interface Load Mode – Selecting Nodes
Locate Summation Vector at Node Centroid Select Free Edge Nodes
Select Nodes
Reset Node Selection
Highlight Selected Nodes
When selecting elements, any elements
may be selected, however only those
connected to the selected nodes will be
used
Restricted © Siemens AG 2015 All rights reserved.
Page 26
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Interface Load – Selecting Components in Summation
• Individual force and moment contributions
that are included in the total summation
vector calculation can be toggled on and off
• By default, all force and all moment vectors
are included in the calculation
• Changes made here will affect the total
summation calculation
• Turning on and off certain contributions
is dependent on how the model was
idealized ; it is up to the analyst to
understand how the FE model correlates
to real-world structure
Restricted © Siemens AG 2015 All rights reserved.
Page 27
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Interface Load Display, Showing Summed Shear Load at a Rib
Restricted © Siemens AG 2015 All rights reserved.
Page 28
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Section Cut Mode
• An extension to Interface Load mode
• The user defines a cutting plane in the
model and the contributing freebody
nodes and elements are determined
automatically
• Total summation location can be placed at
• Plane/path intersection
• Nodal centroid
• Static location
• Nodal and total summation vectors can
optionally be aligned tangent to the path
without having to create additional
coordinate systems
Restricted © Siemens AG 2015 All rights reserved.
Page 29
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Freebody Section Cut Modes
Plane: Cutting plane is defined via base
point and normal vector. Path is defined as
the normal vector; cutting plane will always
be normal to the path
Curve: Cutting plane is normal to the
tangent vector at a point along the plane.
Cutting plane will always be normal to the
tangent vector
Plane / Vector: Similar to Plane, however an
additional vector is defined for the path. The
cutting plane will always remain co-planar to
the original plane and does not have to be
normal to the path
Vector: Cutting plane is normal to the
defined vector. Path is the defined vector;
cutting plane will always be normal to the
path
Restricted © Siemens AG 2015 All rights reserved.
Page 30
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Section cut defined using plane
Restricted © Siemens AG 2015 All rights reserved.
Page 31
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Section cut defined using curve
Restricted © Siemens AG 2015 All rights reserved.
Page 32
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Additional Section Cut options
• Slider tool can be used to move the cutting
plane along the length of the path
interactively within the available entities
• Section cut entities may be limited to a
specific group or selected from the entire
model, and can be limited to a search
distance from the base location of the
cutting plane
• The cutting plane can optionally be given a
thickness tolerance that will allow for
accurate selection of entities that are
slightly out-of-plane
• Clipped entities can either be included or
excluded from the summation calculations
Restricted © Siemens AG 2015 All rights reserved.
Page 33
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Cut plane initial position
Cut plane moved along the path
Freebody nodes
Freebody elements
Restricted © Siemens AG 2015 All rights reserved.
Page 34
ZEN Feb 9-13 2015
Siemens PLM Software
Using the FEMAP Freebody Toolbox
Freebody Tools
1
2
3 4 5
1 – List freebody to message window
2 – List freebody to data table
3 – List freebody summation to message
window (interface load / section cut)
4 – List freebody summation to data table
(interface load / section cut)
5 – Freebody validation tool; warns user
when freebody results are potentially
missing from the model
Restricted © Siemens AG 2015 All rights reserved.
Page 35
ZEN Feb 9-13 2015
Siemens PLM Software
Global-Local Modeling with Freebodies
The freebody Multi-Model Load from Freebody tool automates the creation of
global-local models
• Used to map freebody loads from a coarse grid
model to a fine grid model and automatically
create connections with RBE3 elements
• Start with a balanced freebody in a coarse model
• FEMAP can automatically locate suitable target
nodes in the fine grid FEM and will connect with
RBE3 elements
• Once properly constrained, the detail FEM is
ready to run with a mapped set of loads
• The detail FEM must exist in the same space as
the part in the coarse grid FEM
Restricted © Siemens AG 2015 All rights reserved.
Page 36
ZEN Feb 9-13 2015
Siemens PLM Software
Global-Local Modeling with Freebodies
Define Target Model Parameters
Freebody loads can be applied to target
nodes based according to
• Existing nodes (IDs must match)
• Closest node in space to source
node
• Existing nodes to be connected with
RBE3 elements
• User can define target nodes or
FEMAP can automatically find
• Search distance can be limited
• Maximum nodes to map can be
limited
Restricted © Siemens AG 2015 All rights reserved.
Page 37
ZEN Feb 9-13 2015
Siemens PLM Software
Global-Local Modeling with Freebodies
Restricted © Siemens AG 2015 All rights reserved.
Page 38
ZEN Feb 9-13 2015
Siemens PLM Software
Additional Topics – Freebodies with
NX Nastran Glue / Contact
As of NX Nastran v10.1, the GPFORCE output request does not include
contributions from glue or contact in the F06 or OP2 data block
• The result is a nodal imbalance that is the summation of all other contributions
• Nodes that are affected by glue or contact will not be in equilibrium
• The nodal summation quantity is equal and opposite to the existing
summation
G R I D
0
0
POINT-ID
686
686
686
686
686
686
686
686
686
10000
10000
ELEMENT-ID
821
822
827
828
857
858
863
864
468
SOURCE
HEXA
HEXA
HEXA
HEXA
HEXA
HEXA
HEXA
HEXA
*TOTALS*
HEXA
*TOTALS*
P O I N
T1
-7.854530E-03
-4.059431E-03
7.568718E-03
-2.503399E-02
-2.316282E-02
-1.751655E-03
3.478360E-03
5.081535E-02
-1.318390E-16
2.385245E-17
2.385245E-17
T
F O R C E
T2
5.974986E-02
4.661321E-02
-6.126883E-02
-9.182400E-02
4.661320E-02
6.132058E-02
-9.182400E-02
3.061997E-02
5.620504E-16
5.842150E-02
5.842150E-02
B A L A N C E
T3
7.854530E-03
2.316282E-02
-7.568719E-03
-3.478359E-03
4.059429E-03
1.751656E-03
2.503399E-02
-5.081535E-02
-4.440892E-16
3.122502E-17
3.122502E-17
R1
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
R2
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
R3
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
Restricted © Siemens AG 2015 All rights reserved.
Page 39
ZEN Feb 9-13 2015
Siemens PLM Software
Additional Topics – Freebodies with
NX Nastran Glue / Contact
In FEMAP 11.2, the ability to reverse the nodal summation value was added,
allowing the nodal imbalance to be treated as a separate contribution in the
equal-and-opposite direction
• This option should only be used if the
cause of the imbalance is a result of
data missing from the GPFO table
and not as a result of mechanism at
the node
Restricted © Siemens AG 2015 All rights reserved.
Page 40
ZEN Feb 9-13 2015
Siemens PLM Software
Additional Topics – Freebodies with
NX Nastran Glue / Contact
Default contributions
Freebody elements / nodal summation
Freebody elements + nodal summation
Reversed nodal summation
Restricted © Siemens AG 2015 All rights reserved.
Page 41
ZEN Feb 9-13 2015
Siemens PLM Software
Additional Topics – Load from Freebody Tool
Freebody results can be used to create loads within an existing model using the
Model->Load->From Freebody tool
• Works with all freebody modes
• For interface load and section cut
freebodies, total summation load
can be created at a new node in
the model
• Loads can be created in an
existing load set as well as
in a new load set
Restricted © Siemens AG 2015 All rights reserved.
Page 42
ZEN Feb 9-13 2015
Siemens PLM Software
Additional Topics – Load from Freebody Tool
Freebody Loads
Restricted © Siemens AG 2015 All rights reserved.
Page 43
ZEN Feb 9-13 2015
Siemens PLM Software
Additional Topics – Load from Freebody Tool
Created Loads
Restricted © Siemens AG 2015 All rights reserved.
Page 44
ZEN Feb 9-13 2015
Siemens PLM Software
Additional Topics – Sum Data on Nodes Option
By default, freebody vectors at each node are displayed as a summation of the
selected components
• A global setting allows for nodal
quantities to be displayed as
individual contributions. It affects
all displayed freebodies
• This allows for comparison to
• F06 data, as well as troubleshooting
of models
• This option is best used with
the element shrink view option
Restricted © Siemens AG 2015 All rights reserved.
Page 45
ZEN Feb 9-13 2015
Siemens PLM Software
Additional Topics – Sum Data on Nodes Option
ID: 342
Source
Fx
Fy
Fz
Mx
My
Mz
ELEM 8
-4.12634 -2.76307 -130.752 46.32936
47.4351 -1.88713
ELEM 182
-18.5132
142.901 -466.199 0.280101 0.999626 0.022155
ELEM 80
208.315 34.15445 109.5391 0.067844 0.091289 -0.06195
Restricted © Siemens AG 2015 All rights reserved.
Page 46
ZEN Feb 9-13 2015
Siemens PLM Software
Q and A
Restricted © Siemens AG 2015 All rights reserved.
Page 47
ZEN Feb 9-13 2015
Siemens PLM Software
Contact Info
At Siemens:
Patrick Kriengsiri
FEMAP Development
At SDA:
Russ Hilley
Staff Structural Analysis Engineer
411 Eagleview Blvd
Exton, PA 19341
46030 Manekin Plaza Ste. 120
Sterling, VA 20166
404-353-6596
678-780-9578
[email protected]
[email protected]
Restricted © Siemens AG 2015 All rights reserved.
Page 48
ZEN Feb 9-13 2015
Siemens PLM Software