DOF Spring Tension / Compression 1

[YoungTurk]

How is the DOF spring tension / compression sign convention determined?

I would think it would be independant of element coordinate system, a simple nodes closer -> compression, but my results seem to contradict that.

Better yet, what is the appropriate documentation to check for this?

 

[rb1957]

GPF ?

 

[YoungTurk]

GPF = grid point force

The answer to my question may have something to do with this, but I know not what.

I am using the Nastran NX solver, and post processing in Femap looking at the spring axial force output vector results for the DOF springs.

 

[rb1957]

GPF shows you the balance of FEM forces at a point. you'll be ablve to see the contribution of the CELAS in global axes, so visualising the direction of the force is easier, and you'll see is the spring in tension or not. (intuitively, tension would be the nodes separating apart, no?)

 

[YoungTurk]

How do I display this?

I tried the list>output>force balance but that is text in the message window.

I've tried a variety of setting under the freebody tool, but I can't seem to get a decent display. See attached.

 

[rb1957]

post-process/freebody display ... the new freebody is much more flexible, and a right pain in the a$$.

the old freebody was under view/select ... i don't think it could display GPF results (only constraint reactions).

but if you print the f06 file you can read the results. only don't print the GPF if you're going to show it in the new FeMap (10.3?) ... it doesn't like it (it likes "process only" ouptut).

 

[rb1957]

YT,

mea culpa ... i didn't see your pic at first. you're using the old FeMap, so freebody won't display it for you. but you're listing/querying the nod and getting the GPF results. so which element is the spring ? which direction is the load onto the node in ? isn't that you're answer ??

is the point of the question that you need a compression only loadpath ?

 

[YoungTurk]

The version is 10.2.

What I'm driving at is whether there is a standard convention for DOF Springs tension / compression. If not, what is the sign defined relative to (element orientation?)

Yes, I can figure out whether a particular element is in tension compression by comparing node locations, but this would be cumbersome at best for a model with hundreds of spring elements to be checked.

The GPF solution doesn't help me without the display; there is a positive/negative value for loads into/out of the element; without knowing sign convention it is not clear to me which way the load is going.

I can also do a simple model, or examine a well understood part of the model and come to a conclusion on whether there is tension or compression, but without knowing how the sign convention is determined it isn't clear whether my conclusion applies to results from elsewhere in the model.

The goal is to be able to pull the DOF loads and calculate the tension while ignoring compression for the load points. This would be done en mass for the model rather than examining each element individually.

 

[BlasMolero]

Dear YoungTurk,

The sign convention for the scalar force and stress results in spring elements CELAS2 is determined by the order of the scalar point IDs on the element connectivity entry.

You should be careful how you interpret signs when you use scalar spring elements CELAS2. For instance, reversing the order of G1 and G2 on the CELAS2 entry reverses the sign of the element force.

The sign of force and stress output for scalar elements depends on how the grid points are listed (ordered) when you define an element, and not on a physical sense of tension or compression. This is not the case when you use line (one-dimensional) elements such as CROD and CBAR/CBEAM.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[YoungTurk]

Thank you.

Any recommendation on how to re-define the orietation (presumably by interchanging the nodes as necessary) to make the orientation match the desired vector?

 

[BlasMolero]

Dear YoungTurk,
Well, if you have created lines to mesh with spring elements and you want the mesh to remaints associated with geometry, simply delete the 1-D mesh and orient properly the lines. In FEMAP you can see the direction of curve lineas using command "F6 > Labels, entities, .. > Curve - Surface Direction > Show curve arrows". To reverse the direction of any curve line use "Modify > Update Other > Reverse Curve". Next remesh curves with 1-D elements and you are done!.

If your FE model do not have any geometry, simple edit the element using "Modify > Edit >Element" and re-pick the nodes of the element in the order you like.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/