Nodal Forces 2

[davidnoc]

Hi All:
I asked for forces and moments at a node from large nastran model. I do not have enough experince with FEA but I think nodal forces in nastran are based on global co-ordinate system,if this is true then I can decide whether the positive force is creating compression or tension based on global co-ordinates but regarding the moment I am not able deside the positive moment I got is creating tension or compression on the structure I am intersted in. Please throw some light on this.

thanks all

 

[davezil]

Hi David,
1.True,nodal forces are in global coordinates.you can set a param to get them aligned to 2d elemnts edges (check the qrg)
2.For static balance, the summation of forces acting on a grid(node) must equal zero.external loads equal internal loads.

when you ask for gpforce in nastran it actually gives you the gp force balance -forces of each element which acts on the node and their summation.
What's important to understand is the forces that acts on the element are in the opposite direction.
Then you can simply draw a free body diagram of the elements in mind .
another great utility you can use is the free body in the results tab in patran (if you own a copy),saves you the trouble of summing forces manually(excel).
Hope this helps
cheers

 

[rb1957]

i believe (i don't have the NASTRAN manual here with me) that there's an option in GPFORCE to express the results in element orientations. i suggest you use it in a simple test model to understand what it's telling you.

i'd also consult the manual on +ve sign covention of the beam element ... this is always something that is not the easiest thing to understand.

 

[davidnoc]

Hi,
Guys thanks for the reply.
Since force out put is in global co-ordinates, I know the direction(tension or compression) for forces but for moment isn't the direction follow right hand cordinate system.

Thanks

 

[rb1957]

i'd've thought that if GPF was giving you forces in the global axes, that it would give moments in the sme axes system ...

alternatively, it gives you it all associated to elements.

 

[gwolf2]

If you want element internal forces and moments in the element local coordinate system use the FORCE and MOMENT output options, if you want forces and moments summed at nodes in the global system use GPFORCE.

Consult the manual for the local coordinate system definitions under CBEAM/PBEAM for example. For the difference between element internal forces and global forces summed at nodes see a theory manual, any will do.

I'll guess that you are using PATRAN, in which case you get to pick up the GPFORCE results in the freebody results menus, any other pre/post processor I don't remember where GPFORCE results go. I know that in FEMAP v9 it didn't do it properly.

Ultimately you will have to do a small test model to understand this, now is as good a time as any to start, forget the big model for a day and sort it out in your own mind.

regards

Gwolf.