Mirroring Loads and BCs in ANSYS
Mirroring Loads and BCs in ANSYS
(OP)
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
Thanks





RE: Mirroring Loads and BCs in ANSYS
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
RE: Mirroring Loads and BCs in ANSYS
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
RE: Mirroring Loads and BCs in ANSYS
Thanks
RE: Mirroring Loads and BCs in ANSYS
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
RE: Mirroring Loads and BCs in ANSYS
RE: Mirroring Loads and BCs in ANSYS
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
RE: Mirroring Loads and BCs in ANSYS
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)
RE: Mirroring Loads and BCs in ANSYS
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
RE: Mirroring Loads and BCs in ANSYS
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