global to local 1

[rahulbarve]

dear engineers,
i have carried out structural analysis for global model using ANSYS 11. now i have identified certain important local zones where i want to do a fine mesh analysis.

1) how do i apply boundary conditions from earlier results to these zones if i make a new model.

2) is there a facility where i can bring out these zones in the model, refine the mesh and ANSYS will by itself apply boundary conditions ?

thanks
Rahul

 

[GregLocock]

I guess it depends on what preprocessor you are using, what you are asking for sounds possible, if not foolproof.

Why not just refine the mesh locally in the regions of interest?

Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[rb1957]

as greg says, you can use mesh refinement in your existing model but you need to be careful (eg out-of-plane support of added nodes, particularly if you're using 2D membrane elements); but maybe the model is too big, not yours, etc ...

you can also make a refined model of the detail you're interested in. the key is how to attach this detail to the rest of the world. you know the forces applied to the detail, and you know the displacement along the perimeter of the detail ... apply these as enforced displacements, displace the new intermediate nodes linearly, constrain the model in 6 dofs (rigid body motion) and enjoy the results of your labours.

 

[rahulbarve]

Greg,
the global model is a model of a very big structure, and hence all the tiny brackets, are kind of approximate in this model....
once the results for this model comes out, i need to choose some of these brackets for further analysis, thus modeling with more accuracy.. also sometimes the shell thickness is to be changed to allow more corrossion locally..hence i cannot use just the refinement in the same model.

RB, that seems to be a good idea. but at the same time i also have to apply stresses on the same elements obtained from the global analysis. i dont think i willl be able to apply constraints and forces on same nodes...

cheers
rahul

 

[rb1957]

the enforced displacement of the perimeter should create the same internal stresses. you know the displacement at some places on your detailed model, the smae locations as the coarse grid model, and interpolate for the new fine grid nodes.

but i was thinking you wanted to detail a portion of the model (say the corner of a cut-out).

but maybe you're looking to analyze in detail a discrete piece of structure, like a brkt. in this case, it's better just to take the interface loads from the model and apply them directly to the detail model; or just do a hand calc.

 

[gwolf2]

You need to look on some of the ANSYS forums for how to implement the generic advice already given. Either use the ANSYS forum on eng-tips or use the more specialised XANSYS forum. Whichever way you go, expect it to be very awkward. Neither Classic or Workbench are very friendly once you want to do real FE.

gwolf.

 

[ColonelSanders83]

Just my two cents worth.

If the structure is big and the brackets small then a breakout model is indeed appropriate. Chances are there are many of these brackets or tie in’s throughout the structure. Personally I would take a slightly different approach to the analysis.

I would make a breakout model of the joint and find out where it fails my allowable criteria (stress and/or strain limits) for each individual component of my load and/or displacements. This defines my safe operating envelope and anything below maximums is blessed at a glance.

This has the benefit of only having to analyze any particular joint type once and the same design can be used again in the future without having to rerun an analysis based on new loadings. This may not be applicable to your case in particular but I have found it to take about the same amount of time to analyze based on reaching a limit rather than from an imposed load and or displacement at the model boundary.

 

[spongebob007]

ANSYS has the capability to transfer loads from one model to another. Look up "submodeling" in the help files. I haven't done it in a number of years so I really can't tell you the steps.