Mirroring Loads and BCs in ANSYS 1

[whernandez]

Does anyone know how to mirror loads (i.e. surface pressures on areas) and boundary conditions in ANSYS? I have a symmetric model, which I reflect. However, only the areas and mesh are copied. Is there a macro to reflect loads or bc's? I would appreciate whatever help anyone can provide.

Thanks

 

[Stringmaker]

If your model is truly symmetric why not model it as so and use the /EXPAND command when postprocessing to illustrate the full model.

If this is not the case then as you have discovered only solid and FE geometry can be reflected. The easiest way to apply loads is to create components once the model is completed and use those components for selection. To my knowledge no FE program has the ability to "reflect" loads.

Good luck,
-Brian

 

[cbrn]

Hi,
I don't understand very clearly: if the model is completely symmetric (i.e. geometrically symmetric AND also from the BCs point of view), why would you need to re-create the entire model?
Take advantage of the symmetry, put symmetry conditions where needed and, if you want to "see" the model as if it was entire, use the Expansion.

Regards

 

[whernandez]

My model is symmetric; however, I need to use Inertia Relief in my analysis. In order to use Inertia Relief I would have to adjust the Gravity and Angular Accelerations to run the symmetric model as a static analysis. I would like to aviod this calculation and just Reflect the Areas, Mesh, and Surface Loads for the Inertia Relief case.

Thanks

 

[aphilic]

Hi,

I have a question basicly related to this forum. Actually I want to know the exact symmetry conditions that cbrn mentioned. I mean, lets assume that we have a half sphere. Then we reflected it to make it a full sphere. But in fact we have two half spheres facing each other. As much as I know, we have to combine the facing areas and make it like one area (i.e. nodes and keypoints) and then use the Symmetry B.C. command under:

Define Loads > Apply > Structural > Displacement

But before that, those two areas must be one single area of the half spheres.

My last question is if this process can be done after meshing or must it be done before it?

Regards,

Can

 

[DonTonino]

The two meshes can be combined simply by using the Merge command (NUMMRG, applied to nodes); if by reflecting the volumes you reflect the meshes as well, to combine (by merging, gluing etc) the areas you'll have to clear the meshes as you would receive an error message otherwise, and then merge again the two volumes (or the volume, if you added the two semi-volumes you had).

 

[aphilic]

Hi,

My purpose was to reduce the time at solving process when I defined symmertic small piece and reflect it multiple times. So I thought if i mesh the small piece and then reflect the volume and mesh together, then i thought my purpose would be satisfied. However, as you mentioned and as the warning of Ansys claim, I have to clear meshes for combining two areas. So if I clear the meshes, then combine areas, and then re-mesh each volume, generated by the reflection of the original small piece, again; then i will not have any time saving effect for the model, will I? Or am I missing something?

Regards,

Can

 

[DonTonino]

By reflecting the meshes you can save a (usually) small time on the total spent on the modeling; the most useful aspect of reflecting (based on my experience of course) is to be found in the global mesh to be more 'regular', with constant number of elements and nodes in every volume/surface etc. Computational time depends (approximately) on total number of elements though; so if you reflect a mesh, your model will need approximately double the time to run. To save time you can use the symmetric boundary conditions, but only as long as your model is truly symmetric, i.e geometry, material properties and loads are symmetric.

If I have correctly understood what you mean to do, I guess that you won't have any reduction in solving time as you say you reflect the volumes and the meshes multiple times; you can check your model to see if you can take full use of any symmetric condition that can be found so not to have to do any reflecting more than the truly needed.

If your problem is axisymmetric, consider also developing an axisymmetric model using the built-in options (check the ANSYS manual, 'Modeling and Meshing Guide', chapter 2.6 'Find Ways to Take Advantage of Symmetry', for requirements and tips about axisymmetric structures)

 

[aphilic]

Hi,

Thank you DonTonino, that was the asnwer actually, I dont have to reflect it, I have to put symmetric boundary conditions. Yes, all those things are symmetric Thanks again.

Regards,

Can

 

[DanRail]

Hi,

Rather than beating you up for not using symmetry boundary conditions I'll assume that you need to do this or you wouldn't be asking.

I run a lot of load cases where the model and SOME loads are symmetrical but other loads are not.

There are some old unsupported commands that might help.

These still work in Ansys 8.0 although they have not been documented since rev 5 or so. I can't speak for Ansys versions later than 8.

The problem for you (maybe)is that they need incremented node and element numbers from the original portion of the model to the reflected portion.

If you defined your mesh (nodes and elements) prior to mirroring and did you mirroring with NSYM, and ENSYM commands (or equivalent) then surface pressures can be generated using the EPGEN command. Forces can be generated using the FGEN command, but you might need to get creative with local coordinate systems to get the directions to reverse.

I hope this helps some,

-Dan