next up previous contents index
Next: IV.2 A few small Up: IV. FeResPost Examples with Previous: IV.0 Introduction   Contents   Index

Subsections


IV.1 A small satellite

In this Chapter, one describes the finite element model used in all the examples. The Chapter is organized as follows:


IV.1.1 Presentation of the structure and its modeling

An overall view of the satellite's FE model is presented in Figure IV.1.1. Basically, the structure is composed of an hexahedral lower box and of an upper panel supported by six struts. The hexahedral lower box is made of six sandwich panels connected on 12 metallic bars along their edges. The metallic bars are connected to eight corner nodes. A view of the lower box metallic frame, without the sandwich panels is given in Figure IV.1.2. The corner nodes, and the connections of sandwich panels are modeled with RBE2 elements. However, for thermo-elastic calculations these RBE2 elements are replaced by very stiff CBAR elements.

Figure IV.1.1: Overall view of the satellite's finite element model.
\includegraphics[width=12cm]{RUBY_examples/testSat/postscripts/vue_all}

Figure IV.1.2: Metallic frame of the satellite lower box.
\includegraphics[width=12cm]{RUBY_examples/testSat/postscripts/vue_frame}

The sandwich panels are generally modeled with volumic elements for the honeycomb and surfacic elements for the skins (Figure IV.1.3). A surfacic modeling of a sandwich panel with layered (PCOMPG) element properties has been chosen for only one of the panels: the bottom panel.

To ensure a good transfer of loads to the panels, in particular of the bending moments at connections, small traversing elements have been introduced in the panels modeled with 3D elements. Those elements represent the inserts and connect the two skins. A global view of all the traversing elements is given in Figure IV.1.4.

Figure IV.1.3: Volumic modeling of sandwich panels.
\includegraphics[width=12cm]{RUBY_examples/testSat/postscripts/vue_volume}

Figure IV.1.4: Traversing elements for inserts' modeling.
\includegraphics[width=12cm]{RUBY_examples/testSat/postscripts/vue_inserts}

The struts are modeled with CBAR elements. The struts are connected to the upper panel and to the box +Z panel through metallic fittings modeled with CONM2 and RBE2 elements. (The RBE2 elements are replaced by very stiff CBAR elements for thermo-elastic calculations). The connections of struts to the fittings are ball-bearing connections (only translational degrees of freedom are transmitted, except on the lower side, where the rotation of each strut around its axis is blocked).

The equipments connected to the sandwich panels are modeled with CONM2 and RBE2 elements. (The RBE2 elements are replaced by very stiff CBAR elements for thermo-elastic calculations). A view of some equipments is presented in Figure IV.1.5. On some panels small equipments are modeled by adding a NSM (non-structural mass) to PSHELL properties.

Figure IV.1.5: Open view of the satellite with modeling of equipments.
\includegraphics[width=12cm]{RUBY_examples/testSat/postscripts/vue_open}


IV.1.2 Satellite FEM materials and properties

In the satellite FE model, only seven material cards are defined. The most relevant parameters of material cards are given in Tables IV.1.1, IV.1.2 and IV.1.3.




Table IV.1.1: Isotropic materials used in the finite element model (MAT1 property cards).
Material name MID $ E$ (GPa) $ \nu$ $ \alpha$ ( $ {\text{K}}^{-1}$ ) $ \rho$ ( $ {\text{kg/m}}^{3}$ )
Al-7075-T7351 2 72.1 0.33 $ 23.6{\text{ 10}}^{-6}$ 2796.0
Al-7010-T7451 1 71.7 0.33 $ 23.6{\text{ 10}}^{-6}$ 2820.0
Al-2024-T3 clad 3 69.0 0.33 $ 23.6{\text{ 10}}^{-6}$ 2768.0
(thermo-elastic) 5001 72.1 0.33 $ 23.6{\text{ 10}}^{-6}$ 0.0




Table IV.1.2: 3D anisotropic materials used in the finite element model (MAT9 property cards).
Material type Honeycomb 50 Honeycomb 72
MID 5 6
$ {\text{G}_{11}}$ (MPa) 0.670 0.760
$ {\text{G}_{22}}$ (MPa) 0.670 0.760
$ {\text{G}_{33}}$ (MPa) 669.0 1276.0
$ {\text{G}_{44}}$ (MPa) 0.207 0.310
$ {\text{G}_{55}}$ (MPa) 138.0 193.0
$ {\text{G}_{66}}$ (MPa) 310.0 483.0
$ \rho$ ( $ {\text{kg/m}}^{3}$ ) 50 72
$ \alpha$ ( $ {\text{K}}^{-1}$ ) $ 23.6{\text{ 10}}^{-6}$ $ 23.6{\text{ 10}}^{-6}$




Table IV.1.3: 2D anisotropic materials used in the finite element model (MAT8 property card).
Material type Honeycomb 50 2D CFRP 2D
MID 4 10000
$ {\text{E}_1}$ (MPa) 0.500 290000
$ {\text{E}_2}$ (MPa) 0.500 5600
$ \nu_{12}$ 0.3 0.33
$ {\text{G}_{12}}$ (MPa) 0.500 3000
$ {\text{G}_{1Z}}$ (MPa) 310.0 1100
$ {\text{G}_{2Z}}$ (MPa) 138.0 1100
$ \rho$ ( $ {\text{kg/m}}^{3}$ ) 50 1670
$ \alpha_1$ ( $ {\text{K}}^{-1}$ ) $ 23.6{\text{ 10}}^{-6}$ $ -1{\text{ 10}}^{-6}$
$ \alpha_2$ ( $ {\text{K}}^{-1}$ ) $ 23.6{\text{ 10}}^{-6}$ $ 31{\text{ 10}}^{-6}$
$ {\text{S}_{1t}}$ (MPa) 0.050 1600
$ {\text{S}_{1c}}$ (MPa) 0.050 500
$ {\text{S}_{2t}}$ (MPa) 0.050 25
$ {\text{S}_{2c}}$ (MPa) 0.050 140
$ {\text{S}_{s}}$ (MPa) 0.050 55

All CBAR elements receive PBARL properties:

All skins, except those of bottom panel, are made of Aluminum 2024 T3 and have a thickness of 0.5 mm. The honeycomb used in sandwich panels has a density of 50 $ {\text{kg/m}}^{3}$ . Only in the +Z panel of the box a 72 $ {\text{kg/m}}^{3}$ honeycomb has been used. The bottom panel is modeled with surface elements, and has correspondingly a PCOMPG property card (PID=6). Each skin of the bottom sandwich panel is made of CFRP laminated material with plies 0.1 mm thick. The properties are defined as follows:
PCOMPG   6              50.779   30.+6   HILL   20.      0.
         2008    10000  1.-4     0.      YES
         2007    10000  1.-4     45.     YES
         2006    10000  1.-4    -45.     YES
         2005    10000  1.-4     90.     YES
         2004    10000  1.-4     90.     YES
         2003    10000  1.-4    -45.     YES
         2002    10000  1.-4     45.     YES
         2001    10000  1.-4     0.      YES
         100     4      .0284    0.      YES
         3001    10000  1.-4     0.      YES
         3002    10000  1.-4     45.     YES
         3003    10000  1.-4    -45.     YES
         3004    10000  1.-4     90.     YES
         3005    10000  1.-4     90.     YES
         3006    10000  1.-4    -45.     YES
         3007    10000  1.-4     45.     YES
         3008    10000  1.-4     0.      YES
For sandwich panels modeled with solid elements, the honeycomb is oriented in such a way that the direction Z is perpendicular to the panel. Direction X is vertical for vertical panels and oriented towards +X of coordinate system 1001 for horizontal panels.


IV.1.3 Conventions for numbering and groups

In order to ease the writing of post-processing scripts and the management of FE model, one defines numbering ranges for various parts of the model. The main numbering ranges are given in Table IV.1.4 with the associated groups, when a corresponding group exists. These groups are defined in the Patran session file ``groups.ses''.




Table IV.1.4: Numbering ranges and corresponding group names.
Part group name numbering range
panel -X ``pan_MX'' 20000:24999
panel -Y ``pan_MY'' 40000:44999
panel -Z ``pan_MZ'' 60000:64999
panel +X ``pan_PX'' 30000:34999
panel +Y ``pan_PY'' 50000:54999
panel +Z ``pan_PZ'' 70000:74999
upper panel ``pan_SUP'' 90000:94999
metallic frame -- 80000:84999
struts ``struts_ALL'' 85000:89999

Other groups are defined in the session file:


IV.1.4 Loads and Boundary conditions

One give here information on the various loads and boundary conditions used in the examples presented in Chapter IV.2.


IV.1.4.1 Loads

One makes the distinction between load cases corresponding to quasi-static accelerations or forces applied on the structure and thermo-elastic loads cases.

First, three load cases corresponding to quasi-static accelerations applied to the entire satellite structure are defined in file ``unit_accel.bdf''. These accelerations are defined by Nastran ``GRAV'' cards and are oriented in directions X, Y and Z. Their Load identifiers are 601001, 601002 and 601003 respectively.

Then loads corresponding to quasi-static acceleration on parts of the structure are created by defining the appropriate force fields. The method used to defined those force fields is explained in the example presented in section IV.2.5.1. Six files contain these force fields:

One also defines temperature fields for thermo-elastic load cases calculations: The method used to defined these temperature fields is explained in the example presented in section IV.2.5.2.


IV.1.4.2 Boundary conditions

Only two different fixations of the satellite are used in the examples of Chapter IV.2:


IV.1.5 Main data files

In the definition of main data files, one tried to avoid the definition of too many load cases one the structure. Therefore, one defines elementary load cases on the structure. The Results of these load cases can be recombined at post-processing level to produce the recombined Results.

The elementary load cases are defined in the following sections. One also summarizes the additional calculations that have been performed with Nastran to allow the testing of Result importation for other Nastran Solution Sequences.


IV.1.5.1 Acceleration unit loads on entire structure

One defines two data files corresponding to unit accelerations applied to the entire structure. These data files correspond to the static and thermo-elastic versions of the model respectively. On the static model, the corresponding load case names are:

These load cases are defined in file ``unit_xyz.bdf''. Correspondingly, one defines unit load cases on the thermo-elastic version of the model in file ``orbit_unit_xyz.bdf'':


IV.1.5.2 Acceleration unit loads on parts of the structure

Two data files corresponding to the local unit acceleration fields defined in section IV.1.4.1. These files are named ``unit_xyz_pan_pz.bdf'' and ``unit_xyz_upper.bdf'' respectively. They define the following load cases:


IV.1.5.3 Thermo-elastic load cases

One defines also two data files corresponding to the definition of thermo-elastic load cases on the structure. The file ``temp_disc.bdf'' defines four load cases in which discontinuous temperature fields are applied to the structure. The four load cases are defined as follows:

The file ``temp_grad.bdf'' defines three load cases corresponding to gradients of 100 $ ^\circ$ C/m applied on the entire satellite:


IV.1.5.4 Other solution sequences

Several main Bulk Data Files defined in ``MAINS'' directory are provided to allow the testing of result importations for different Nastran solution sequences:


IV.1.6 Organization of FEM in files and directories

One gives here information on the way the model has been split into several files and the organization of the files into different directories.

The files are located in six different directories:

Note also that each file include in a ``.bdf'' main data file can itself include other files.

The directory ``PATRAN'' contains a Patran session file that can be used to import the definition of groups in a Patran or FeResPost DataBase.


next up previous contents index
Next: IV.2 A few small Up: IV. FeResPost Examples with Previous: IV.0 Introduction   Contents   Index
FeResPost 2017-05-28