FEMAP to ANSYS

Hello!,
FEMAP allows you not only to export your FEA model to Ansys but also to launch Ansys solver inside FEMAP, solve with Ansys solver, and recover output results for postptrocessing in FEMAP.

I suggest the following steps:
1.- After finishing your FEA model in FEMAP, define your analysis study using "Model > Analysis".
2.- Under "Analysis Program" choose solver ANSYS, and under "Analysis Type" you can setup the type of analysis to run (linear static, linear buckling, normal modes/eigenvalue, etc..) and define the parameters of the analysis.
3.- In the "Analysis Set Manager" you can issue command PREVIEW INPUT, and FEMAP will show you the Ansys file input.
4. Alternatively you can issue command EXPORT and FEMAP will write your Ansys input file.

Or alternatively you can issue command "File > Export > Analysis Model", the end will be the same.

Best regards,
Blas.



~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:

Thanks Blas! It works fine!

One more question;

When I do the translation, the RBE-3 (that are include in the model)

have a mass associated that I didn't create. What is the reason for

this behaviour and how can I resolve the problem?

Dear David,
First at all the RBE3 is a NX NASTRAN and FEMAP finite element type-only, in Ansys do not exist a similar element, then FEMAP translate it as CP coupling constraint commands or CERIG commands.

Second, revise your model, if you were the only author (or creator) of the FE model then you will know what commands you used to create it: only exist a command in FEMAP that created both mass element and rigid element, that is command "Tools > Mass Properties > Solid Properties" that will ask you to select a solid and the next question is "OK to create a representative node and mass element?", the next prompt is the density (by default 1.0), and finally will ask you "OK to link mass to mesh?". Well, at this point I suggest to cancel command because FEMAP don't allow you to specify what type of RIGID element to create (RBE2 or RBE3), then is better to make this process "by hand": after cancel command, FEMAP will create a 0-D MASS element (named CONM2) + node at the center of gravity of the solid. FEMAP also will create the property associated to this element. Simply edit the property to enter the correct mass value.

The final step will be to connect the above MASS element with your supports: simply use command "Model > Element > TYPE = RIGID" and make sure to select RBE3 (interpolation): here select the MASS NODE as DEPENDENT and all the support nodes as INDEPENDENT. Click on NODES to select nodes using METHOD = BY CURVE, etc. Regarding DOF, make sure to select TX,TY,TZ only in both DEPENDENT & INDEPENDENT fields (desactivate rotations).

And you are done, you have created your first SPIDER RBE3 element, a "feature" unique in FEMAP!!.

Please let me know if this is what you did in FEMAP session.
Best regards,
Blas.



~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:

Dear Blas;

First of all, I've to tell that I created the model in Patran. Then

I imported it in FEMAP because I read in some forums that is a

useful way to translate to ANSYS.

When I export the model to ANSYS, femap ask me what kind of

translation want to do: CP coupling constraint commands or CERIG

commands. What is the best choice?

I show you the questions that femap ask me;

1. OK to write rigid elements as CERIG commands?(No=CP commands)

2. Creating small mass on master nodes. Use Rotary intertia option for small mass?(No = Transations only)

3. Creating small mass on master nodes. Use 3D option for small mass?(No = 2D option)

Thanks!

Dear David,
That explains the situation, regarding mass elements is up to you if you want to have them in your model or not, FEMAP will translate what you have in your FE model, then I don't understand very well the question.

The use of mass elements + RBE3 rigid elements is a common practice we all use to include components that do not contribute to the stiffness of the structure but its mass is important for the dynamic behaviour of the structure.

Regarding translation of RBE3 to Ansys, the use of CP coupling constraint is classical.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran: