cancel
Showing results for 
Search instead for 
Did you mean: 

REACTION FORCE AND MOMENTS

Experimenter
Experimenter

hi

 

I need help to understand the reaction force and moment.

 

I am doing a static analysi of 1 m beam with 1 N applied at the one end and fixed constarn at other end. Then i got 1N reaction force and 1N-M moment at the end which fixed. this reasult is the same as the mathmatic calculation.

 

second, i have done the same analysis using solid element for the same diamention, and got totally different results for force and moment.  i am confused, please help. thanks.

 

Guanqun

 

 

 

 

4 REPLIES

Re: REACTION FORCE AND MOMENTS

Siemens Phenom Siemens Phenom
Siemens Phenom

For the beam element model, there is a single grid that is constrained, so all reactions are at that grid and match what you expect.

 

For the solid elemnet model, there are 4 grids that are restrained (from the image, it looks like one face of a single brick element). You need to sum the forces and moments to get the resultant reaction force. Note that there are no rotational DOF on solid elements. The moment comes from the force times the distance to the point you are summing about.

Re: REACTION FORCE AND MOMENTS

Experimenter
Experimenter

Hi JimB

 

Thanks for help.

 

you are correct, using identify result to sum the force and it is same with the applied force now, but for the moment, is any way to show the result in NX? or i have to check it by hand calculation?

 

Thanks.

Guanqun

Re: REACTION FORCE AND MOMENTS

Creator
Creator

The easiest way to be able to recover the total interface loads in this case is to use a rigid element (RBE2). The independent node would be SPCed, and the element would be connected to all of the boundary nodes of the solid elements.

Re: REACTION FORCE AND MOMENTS

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor

Hi,

You can always check the .f06 file generated by Nastran during the analysis. It is at the same place than the .sim file.

 

In this f06 file, at the begining you will find the OLOAD TABLE , that describe the resultant of the external applied load. At the end of the file, when the calcultaion is done, you will find the SPCLOAD TABLE (and the MPCLOAD LOAD if you fixed node on rigid body like RBE2).

 

You only need to check that OLOAD = -(SPC LOAD+MPCLOAD) to verify than the equilibrium is OK.

 

PLus there is a parameter called epsilon in the .f06 file that gives information on the equilibrium error. IF superior than 1e-3 then your model il not well balanced.

 

The f06 file can be open with any text manager (textpad, notepad etcc)