Dear fellow engineers,
I'm trying to solve catenary problems using FEMAP.
See bellow how it can be usefull for me.
However I don't know how to formulate the problem (aka set boudary conditions and use large deformation solver).
Has anyone done this kind of problem?
Well, this is not a problem of FEMP, that is a pre&postprocessor only, but the FEA solver you use with FEMAP. Actually FEMAP support the CABLE element definition in the Graphics User Interface (GUI) using the ROD PROPERTY.
But if you are using the bundle FEMAP with NX Nastran, then in this case with NX Nastran solver we don't have a genuine CCABLE element yet, it had been requested many times by the nx nastran community (I filed myself an ER#1853240 in 2011) but SIEMENS PLM yet do not offer this capability for NX NASTRAN (SOL106) nonlinear module. Things are changing quickly, SIEMENS PLM already has developed natively the MultiStep Nonlinear solver (SOL401), and also is the owner of the powerful nonlinear SAMCEF solver through the acquisition of LMS company, then in the future who knows, surely we will have the CCABLE element under the SOL401 nonlinear solver soon???, I hope so!!.
For now, as a workaround, what you can do is to use the CROD nx nastran element with the Nonlinear Solver (SOL106) or Advanced Nonlinear Solver (SOL601) to simulate a CABLE in the following way: the CROD element may have material nonlinear extensional properties, you may supply plastic or nonlinear elastic material properties. Since the stress-strain curve for compression need not be the same as for tension, this element can, for example, be used to model cables which cannot carry compression.
I have used Femap with NX Nastran for a cable-car style problem (cable over pulleys, using "slidelines" for cable to pulley contact). In this case we used standard NX Nastran beam elements, although we artificially changed the beam I1 I2 values to reduce the bending stiffness (not an extreme reduction, otherwise convergence can be very difficult). However, for this to work well, the number of increments required to run the analysis needs to be very high (hundreds, or even thousands) to converge to the proper shape/results - but for a beam model of moderate size, the runtime was still quite reasonable in SOL106 (NL Static).
I have a trial version of FEMAP with Nx Nastran.
I have access to the ROD element from GUI.
Are you saying that this is not usable with the NX Nastran solver?
If they are usable what are the minimum values to be defined for the property (area, nonstructural mass, initial tension ???)
As far as I can see I don't have access to the native Nastran properties.
All terms under "Additional Options" are not supported by NX NASTRAN solver, if you set ON and do a PREVIEW ANALYSIS you will receive an error in the FEMAP message window because NX Nastran don´t support any entry you define after activating the cable option, then forget to activate the option, OK?.
In the PROPERTY VALUE section of the ROD PROPERTY is where you have to define the values: this is the classical CROD NX NASTRAN element (remember: a rod element supports tension, compression, and axial torsion, but not bending) where the cross section of the rod is the minimum value you need to enter (ie, the cross section of the cable). Plus also you need to define the nonlinear material property using a stress-strain curve not working in compression, ie, only-tension element.