Measuring Deformation Values from a Deformation Plot

Dustin-

Are you running Cosmos/M with Geostar or Cosmos thru SolidWorks or something else?

jt

Hi,
Jte, it's unrelevant: all the family of SRAC's products "thinks" the same way.
DustinMechEng, really I can't see your point: "deformation" is another way - very unclear, I recognize - to call "strain" (epsilon); "displacement" is exactly what it is called for: the vectorial difference between the nodes' coordinates under load and the nodes' coordinates in unloaded condition, just like in any other FE program. There is no such thing as a "displacement relative to the fixed point". The "deformation relative to the original shape" is exactly given by the displacement plot!!! Perhaps what you are looking for is the "shrinking" part only of the deformation; in this case, I don't know how to extract it with Cosmos.
Or am I missing something herein?

Regards

Thanks for the responses-

jte- I am using Cosmos thru Solidworks

cbrn- This is a tough topic to convey, so let me explain it by describing a model. Say you have a model of a ball supported by a spring to ground. In addition to the spring, you have a point force on the ball pushing in the direction to compress the spring into the ground. At some point, the spring will deflect a certain amount (say 1 inch) and the model will come into equilibrium. At this point, the center of mass of the ball will have moved one inch. In addition, the point force will have deflected the surface of the ball, at the point of interaction, a certain amount (say .01 inch). Now, if you wanted to know how much the surface of the ball deflected, how would you do it?

The problem I am encountering is that the deflection plot takes into account both the center of mass deflection of the ball and the surface deflection of the ball. If I look at the deflection plot, it shows the surface of the ball (at the point of force interaction) has deflected 1.01 inches. While I know it has only deflected .01 inches. The deformation plot shows this .01 inch surface deflection correctly, however, I can't get the actual deformation values out of it. It just shows it graphically. Hence my original question: how do you obtain the deformation values from a Cosmos deformation plot?

Thanks for the help!

Hi,
if that's the effect of the force over the surface you are interested in, then you are making an extremely simple problem overly complicated:
in equilibrium, the spring will react EXACTLY the active force(s) acting on the ball, so including the spring into the analysis is absolutely pointless.
Simply restrain the ball to zero-displacement in the same location(s) where the spring is attached.
In fact, the presence of the supporting spring adds nothing to the deformation of the ball, it only adds a rigid body motion part.
Another way to obtain the same thing is to subtract to the displacement field of the ball the displacement of the node attached to the spring.
Generally speaking (I can't add details on how to use Cosmos, since I stopped using it 3 years ago so I'm out-of-date), you do can extract the numerical values of anything, and save them in file: if you scope on a surface, it will list the magnitudes of the requested value on all the nodes belonging to that surface.

Regards

Yeah, that ball problem was just an example to explain what I am trying to do. The acutal problem is the pressure problem that I explained in the original post. My object has uniform pressure distribution on all external surfaces. In reality, the entire object will be "squeezed" toward the object center of mass. In Cosmos, I have to fix a point in the model in order to establish boundary conditions for the solver. So, all the points in the model deflect relative to the artifically fixed point. However, what i need to determine, in the end, is the amount of deflection of all points in the model with respect to the original shape of the object (not their deflections relative to the articically fixed point).

Hi,
so, either you can find an isostatic system of erstraints which doesn't alter the solution (e.g. properly chosen points for 3-2-1 method), or you let the model "float" without restraints, provided that you have "weak springs" activated and you make sure your force / pressure field is RIGOROUSLY hydrostatic, or you do some "manual" postprocessing afterwards (it's only a matter of sums / differences, the difficulty being in the number of nodes which could oblige you to split the lister files in several pieces in order to be handled in Excel...).

Regards

cbrn said:

Jte, it's unrelevant: all the family of SRAC's products "thinks" the same way.

Click to expand...

cbrn- Are you implying that the command line in GeoStar is identical to the options available through SW? Similar functionality, but kind of different approach... For example, telling dustin to type actdis; [enter] and then displot;[enter] is a wee bit different than going thru the SW menu approach...

dustin- If I understand your situation correctly, then here's a similar situation: Model a cantilever beam. Fix the end at the origin. Apply a force on the other end. Get SW to list the distance a node near the non-fixed end has moved relative to its original location instead of relative to the origin. Have you looked at the CosmosWorks 2007 Online User's Guide under Index keyword "displacement" and "listing"? Look at the bottom of the "List Displacement" page and take a look at "To list a displacement component with respect to a reference geometry". This approach may be severely limited with a complex shape, but might get you in the right direction...

jt

Hi,
jte, OK, I misunderstood your original intent. The way in which SRAC's programs behave may be strictly similar, but as you say the way to interact with them is completely different.

Regards