Cancel
Showing results for 
Search instead for 
Did you mean: 

Verschiedene Fragen zu Femap v11.2

Pioneer
Pioneer

Hey Leute,
ich muss im Rahmen meiner Bachelorarbeit einige FE-Analysen durchführen und habe zu diesem Zweck zunächst mit dem mir bekannteren Solid Edge und schließlich mit Femap 11.2 gearbeitet.
Dabei sind mir so einige Fragen und Probleme aufgekommen , vielleicht könnt ihr mir ja helfen sie zu lösen.
(Ich habe mit den FEM bzw. FEA zuvor keine Erfahrung gemacht und von daher entschuldigt meine leihenhafte Beschreibung bzw. die vermutlich dummen Fragen)

-Die Baugruppe soll aus verschiedenen Materialien bestehen (Metalle und Polymere) , ich kann zwar mehrere Materialien in die Liste aufnehmen und definieren, jedoch kriege ich es nicht hin sie einzelnen Solids zuzuordnen.
Hat da jemand einen Rat ?

-Das Modell soll sich im Rahmen einer Zugbelastung verbiegen, wobei eine Art Draht mit dem Polymer in Kontakt tritt und eine Krümmung verursacht (Ähnlich der Sehne im Finger, welche beim ziehen den Finger beugt)
Da meine Drahtsehne jedoch zunächst nicht auf dem Material aufliegt und sich ja auch relativ zu der Führung verschieben kann , lässt sich keine Verbindungsbedingung formulieren und Femap ignoriert das aufeinandertreffen der beiden Oberflächen einfach, so das die Sehne irgendwo im Material hängt.
Lässt sich dieses Problem mit Solid Edge lösen (Das kommt mir einfacher verständlich vor, scheint aber nicht so umfangreich wie Femap) , wenn nein, wie löse ich es mit Femap ?

-Im Gegensatz zu Solid Edge, lässt sich bei Femap nirgends erkennen welche Einheiten Standardmäßig verwendet werden ... wo kann ich herausfinden welche Einheiten Femap verwendet, bzw sie ändern.

Jedem Antwortenden danke ich schonmal im Voraus Smiley Happy

3 REPLIES

Re: Verschiedene Fragen zu Femap v11.2

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

1.- Simply create the Material Property, then create the "Element Property" where is mandatory to select the previous material, and finally assign the Property to the Geometry using command "Mesh > Mesh Control > Attributes on Solid" if you plan to mesh with 3-D solid elements, or "Attributes on Surface" if you have defined a 2-D Shell property to mesh mid-surfaces, etc.., OK?.. Next when meshing the geometry you simply select the default option "Use Meshing Attributes".

 

2.- Not understood at all the explanation of the "Tendon on the Finger" problem, please write on English to see if we can help you better.

 

3.- FEMAP is unitless, this means that you can run any system of units you like, BUT you are the only responsible of units coherent, not FEMAP (funny, right?). Then, make your numbers, because this is critical: I strongly suggest to work geometry in millimeters ALWAYS. How?. Go to FILE > PREFERENCES > GEOMETRY and select millimeters (by default FEMAP arrives configured in INCHES). This setting affect when you import geometry, the dimensions of the CAD file are translated to "mm", OK?. Then if you have a curve length of 100, it means you have 100 mm, easy, don' t you?. From now in advance ALL of your dimensions are in millimeters, problem solved!.

 

preferences-geometry.png

 

Regarding material, the default material library "MATERIAL.ESP" comes in INCHES, POUNDS, PSI, etc.. I strongly suggest to select the material library that comes in MPa, mm, N, etc.. simply go to FILE > PREFERENCES > LIBRARY and under material select the file "mat_enf_mm-N-Tonne-degC-Watts.ESP". Then from now in advanced each time you insert a material from the database will be coherent with the units length of mm. So, you need to apply force in Newtons, pressure in MPa, mass in Tons, density in Tons/mm3, and Stress results will be in MPa, understood?.

 

preferences-material.png

 

Keep pushing FEMAP, you will realize the powerful you have in your hands!!.

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: Verschiedene Fragen zu Femap v11.2

Pioneer
Pioneer

First of all, thank you very much for the extensive reply !

The problem with the tendon in the finger is more a basic question, than a specific one.

I tried to upload a picture of the simulation, so you can understand it simplier, but it doesnt work 

( error message "${arg:exception.imageMeta.originalFileName}: Image Format not Permitted Sorry, images of type '${arg:exception.imageMeta.mimeType}' are not allowed.")

Seems like .bmp or .jpg are unconventional 0.o (I put the picture in the Attachment)

So i will explain it, the problem is, that i have two objects connected together and there is a force on the one of them which couses the object to bend towards the other one.

At the point when both objects collides , there should be an interaction which stops the movement, but Femap acts like there is no obstacle and moves one object through the other.

 

 

 

Re: Verschiedene Fragen zu Femap v11.2

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

I have simply saved again your *.PNG file and is possible to insert in the post.

Well, this is a simply question to answer: LINEAR surface-to-surface contact make sense to run the LINEAR STATIC solver of NX NASTRAN (SOL101) when BOTH bodies are physically in contact, touching, OK?. If contact bodies are not in contact (a gap exist), then linear static displacement & stress results are useless, simply colors, unless the gap distance is very, very small. But for the picture of your model, I guess this is not the case, the separation between both contacting bodies is important.

 

CONTACT-sol101.png

 

If you have a physical GAP distance between bodies, then a NONLINEAR ANALYSIS should be required to run activating as minimum both geometric (large displacements effect, "PARAM, LGDISP,1") and contact nonlinearities.

 

For nonlinear analysis using NX NASTRAN you have available two modules, well, soon three:

  • NX NASTRAN BASIC NONLINEAR (SOL106): one important limitation is that surface-to-surface contact is not available, but we have the CGAP nodo-to-node contact elements, as well as slide-line contact (take a look to FEMAP example problems 26, 27, 28 & 29).
  • NX NASTRAN ADVANCED NONLINEAR (SOL601): Really powerfull supporting all type of nonlinearities (geometric, contact & material), but is an add-on module, not part of the basic FEMAP & NX NASTRAN bundle. Take a look to the following link:

http://community.plm.automation.siemens.com/t5/NX-CAE-Forum/Small-Sliding/m-p/303937#U303937

 

  • NX NASTRAN new nonlinear (SOL401): well, currently under development (only available under NX but soon in FEMAP) is a NEW nonlinear solver developed natively by SIEMENS PLM CAE team, and in the near future will replace basic nonlinear module (SOL106). Will feature surface-to-surface & edge-to-edge nonlinear contact, quite promising!!.

I hope all is clear, 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/