ELFORCE in Nastran

[jsboy]

Could anyone explain to me what is the definition of element force output in Nastran with ELFORCE card? I have to know how it is caluculated. Thanks!!!

 

[hombre]

jsboy,

The ELFORCE (or FORCE) card generates the nodal forces at the four corners of the 2 dimensional element and/or at the center of the element.

If CENTER is specified, only the force at the center is output which is the average of the nodal forces at the corners of the element. ((C1+C2+C3+C4)/4) with C(N) being the nodal forces at the corners)

If CORNER is specified, the nodal forces at the corners as well as at the center is output.

Hope this helps,

Hombre

The CENTER option is the default, by the way.

 

[Eap2n]

jsboy,

Remember that, just like in classical plate theory, the force/moment values are given per unit length, i.e. its not the total force/moment acting on a node. The values are calculated by integrating the stresses over the element thickness.

Erik

 

[jsboy]

Erik,
Thanks for your answer but would you please provide more detailed explanation on this? I am not really sure what you are saying here.

 

[hombre]

He is saying that the force output from NASTRAN for 2D elements is force per unit length (lbs/in for example). Therefore, you need to multiply the elemental force by the element length.

Hombre

 

[Eap2n]

jsboy,

Be careful because if what you are really after is the total force acting at a node you are much better off in NASTRAN getting it from the grid point forces (GPFORCE). The freebody tool in PATRAN is great for visualizing the grid point force output. Remember that the forces calculated with ELFORCE are element-based values so they are not inherently continuous at the nodes which means they are not going to give you the "true" nodal force, depending on the quality of your mesh with respect to the stress gradient in the region you are looking at.

Hope this makes more sense, let me know if it does not.

Regards,
Erik

 

[jsboy]

Thanks Erik!! Very clear!!