cancel
Showing results for 
Search instead for 
Did you mean: 

Meshing a CubeSAT model+Lengthy post processing times

Creator
Creator

Hi all, I am a newbie.

I have problems  meshing a cubesat model...having PCBs and Transmitter Assemblies...

 

Please help

14 REPLIES

Re: Meshing a CubeSAT model+Lengthy post processing times

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hi!,

Ufff, if not being more explicit it will be difficult to help you, post the FEMAP model here, explain your specific problem(s) and this way we can help you, OK?.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Meshing a CubeSAT model+Lengthy post processing times

Creator
Creator

Thank you for quick response. I attached a JPEG...

 

I want to do a normal modes and modal frequency analysis

But i get several warnings and fatal errors, tried to see if removing the internal mass will help, but expectedly the returned eigen modes were too low,

So i attache a node to the COG of base plate but it doesn't work.

Re: Meshing a CubeSAT model+Lengthy post processing times

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

For the picture it seams to me that you are starting the house by the roof: in the FEMAP message area I see commands like TET meshing, HEX meshing .... if running this way "you will receive what you deserve": complex meshing, lengthy postprocessing, continuous errors ..

 

Not at all running the above way, you need to be smart, this is not CAD by FEM/FEA: I suggest to build first the simplest FEMAP model as much as possible, based in 1-D CBEAM elements, 2-D Shell CQUAD4 elements and 0-D CONM2 mass elements, forgot at all 3-D Solid elements at this stage.

 

You need to learn how to define properly joints between different types of elements, in dynamic analysis the use of mass & rigid RBE3 & RBE2 elements is critical:

  • The RBE3 element is a powerful tool for distributing applied loads and mass in a model.
  • The RBE2 provides a very convenient tool for rigidly connecting the same components of several grid points together.
  • The CONM2 element allows to define a concentrated mass about its center of gravity.

Also another reason why your dynamic model should be smartly build is because when later you plan to perform, for instance, a Modal Frequency Dynamic response Analysis (SOL111) the output *.op2 size could be Gigas & Gigas of results, impossible to postprocess, then you need to create a FEMAP model would be able to capture correctly both mass & stiffness, but at the smallest size as possible, and here the use of the above element types as mass, beam & plate are perfect!!.

 

To use FEMAP correctly is critical first to know in depth the NX NASTRAN solver resources, to know the capabilities & features of every element type from the NX NASTRAN Element Library, in summary to know Finite Element Method, then the use of FEMAP is easy. Start reading the NX NASTRAN manuals, they are a gold mine!!.

 

To get more help, please post your specific question.

 

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Meshing a CubeSAT model+Lengthy post processing times

Creator
Creator

Thank you.

 

You are right. How can I get access to this NX Library? All I have as a resource is the Examples "book" that came along with the software.

 

What will you recommend as a quick fix, if I want a mass to act down the base of the structure without using the actual CAD elements?

Re: Meshing a CubeSAT model+Lengthy post processing times

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

In FEMAP go to HELP > NX NASTRAN and all the NX NASTRAN manuals will open.

 

Regarding your question, do the following:

1.- Joint all solids you want to convert as mass using command "GEOMETRY > SOLID > ADD".

2.- Create a 0-D concentrated mass element in the CoG of the new created solid using command "TOOLS > MASS PROPERTIES > SOLID PROPERTIES". The important task here is to create a CONM2 element + grid in the CG, when requested for the mesh density simply enter a value of 1.0. Later edit the created mass property and in the field "MASS, M or MX" enter the correct mass of the solid. Please caution with units: if your model is in meters (ie, you are using the SI system of units) MASS is in kg and density is in kg/m3. If you work in mm & N, then MASS should be in Tons and density in Tons/mm3).

 

MASS-properties.jpg

 

3.- Next define a RBE3 rigid element to joint the grid node of the MASS element at the attachments points with the rest of the structure. The DEPENDENT node of the RBE3 element should be the grid node of the CONM2 mass element. The INDEPENDENT nodes should be the attachments on the frame of your structure. Please note before create the RBE3 element you need to have meshed your main structure (the frame) to have available the nodes at the attachments.

 

rbe3-dof.png

 

rbe3.png

 

The following picture shows a simply assembled structure composed by different types of finite elements: mass, beam, RBE3, shells and solids. The concentrated mass CONM2 element is attached to the structure using a rigid SPIDER RBE3 element.

 

CONM2.png

 

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Meshing a CubeSAT model+Lengthy post processing times

Creator
Creator

Thank you.

 

I followed the steps above and I was able to have a concentrated load act down the base of the structure. I also got rigid link to act between the contact at the base of the structure with the main frame.

So now I have two properties, the main frame which I have defined as a solid property, and the Concentrated Mass properties

1. While meshing, do i need to mesh the newly formed solid(from concentrated mass) again?

 

2. The unit system is also quite confusing. While importing my model to FEMAP, A scale factor of 1000 is automatically applied. I measure cross sectional area and confirm that my value is in mm (therefore I assume that the force is N and the mass is tonnes), However on doing a buckling analysis, the eigen value returned is quite huge (29,000) and unrealistic. Am I defining units wrongly?

Re: Meshing a CubeSAT model+Lengthy post processing times

Siemens Phenom Siemens Phenom
Siemens Phenom

My guess is that you are using inconsistent unit values for the mass density of your materials.  To ensure consistent units, follow the units in the table below:

 

Model Data

English
(lbf-in-s)

Metric
(mN-mm-s)

Metric

(N-mm-s)

SI

(N-m-s)

Length

inches

mm

mm

m

Mass Density

lbm/in3

kg/mm3

Tonnes/mm3

kg/m3

Force

lbf

mN

N

N

Stress, Pressure,

Modulus of Elasticity,

Shear Modulus

psi (lbf/in2)

KPa

MPa

Pa

Moment,

Torque

lbf-in

N-mm

N-mm

N-m

Velocity

in/sec

mm/sec

mm/sec

m/sec

Acceleration

in/sec2

mm/sec2

mm/sec2

m/sec2

Temperature

°F

°C

°C

°C

Coefficient of Thermal Expansion

in/degF

mm/degC

mm/degC

m/degC

Best Regards,
Chip Fricke
Principal Applications Engineer - Femap Product Development

Re: Meshing a CubeSAT model+Lengthy post processing times

Creator
Creator

Thank you for this chart, it helps.

How do I know whether my force is mN or N (for the metric set)?

If scale factor is 1000 during geometry import, then force is mN?

if scale factor is 1, force is N?

Re: Meshing a CubeSAT model+Lengthy post processing times

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

1.- I don't understant the question, plot a picture better: once you have your mesh done not need to remesh again, make sure that all the nodes of the RBE3 element are picked properly.

2.- The reason to use Tones for mass, density = Tons/mm3, length in milimeters, load in Newtons and pressure in MPa is because the coherence of units when performing a normal modes/Eigenvalue analysis using NX NASTRAN (SOL103). You can import your model in meters (scale factor 1), this is up to you, but working in milimeters is handy and covenient.

3. For buckling analysis a value of 29000 for the buckling load factor is relative, it depends of the load level applied:

  • if you apply an unitary load of 1 N, then 29000 is your buckling load.
  • But If you applied real loads, then BLF=29000 is meaningless, revise your model.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/