What types of analyses are you trying to perform (linear static, geometric or material non-linear, heat transfer, fluid flow, pipe, etc.)?  Are the tutorials not enough information to develop general guidelines?

You may also want to check Algor's e-learning site.  It has many free webcast videos that are useful and can be played at any time.

Hi GBor,

Thanks for your prompt reply. When you say " General Guidelines" what do you mean by that? Could you please be more specific about that? What these Guidelines should consists of? The analyses are linear static stress, heat transfer steady and transient and thermal stress.

So what does it mean "Guidelines and Procedures" in this context? What kind of topics should be included in these Guidelines ?

Regards,

Bogdan

I am having a little trouble understanding what you are actually trying to do, but ALL analyses start in much the same way:

1)  Develop the geometry of your object
2)  Apply a mesh to the geometry
    a)  Determine the type of mesh needed (beam, plate, brick)
    b)  Determine the mesh size or automesh parameters
    c)  Verify mesh continuity
    d)  Check for areas of needed refinement
3)  Determine and apply boundary conditions
4)  Determine and apply loads
5)  Analyze
6)  Confirm results (testing, hand analyses, engineering judgement, etc.)
7)  Refine mesh and reanalyze (this is referred to as a "mesh sensitivity" test and I've seen it done many different ways)

The boundary conditions and loads vary depending on the part installation, application, and analysis type, but all analyses are pretty much:  geometry, mesh, boundary conditions and loads, analyze, post-process.

I would suggest that you develop guidelines for any CAD models that would be developed.  For instance, will you import IGES files or STEP files?  If so, make sure you know what parameters need to be exported from the CAD software.  IGES should be trimmed surface (144 entities, I think).  If you do assemblies, which works better for the information that you want to import.

Or, are you building all models in FEMPRO.  If so, there are many "Tips and Tricks" to efficiently modeling in FEMPRO.  Some of these would be helpful, but perhaps you should establish precision information.

For the mesh, will you require quad element meshes, or are triangular meshes acceptable?  Can you accept automeshes that result in only 12 elements around a bolt hole?  Or do you require a minimum of 18?  Or do you not want to put bolt holes in global models knowing that you will analyze them by hand?  If so, how will you extract fastener loads?  There are also guidelines for when you should use brick elements instead of plates, and how will you model beams?  Are the beams large enough that they should be modeled as plates, or do they really follow beam theory?

Boundary conditions:  When are symmetry conditions appropriate?  Should you analyze with fixed boundary conditions or pinned, or both and average the results?

Loads:  Do you attempt to balance the loads so that you use a minimum of boundary conditions and do you apply the loads as pressures instead of point loads?  What is the best method of applying thermal loads?  If you have an air gap in the middle of a part, do you ignore it, or do you have a process for handling the heat transfer through the air?

Post-processing:  When you have a high stress concentration, when do you believe it?  Do you separate the thermal stress and the static stress, or do you need to combine them?

There are MANY, MANY issues I could bring up, but I would need to know more about your product and what you do to analyze them to narrow down the types of guidlines that you may need to develop.  You may be able to find some on the web that would be applicable to your situation, or you may be able to modify some generic thoughts.

There is an FEA forum on Eng-Tips.  You may want to check in to it.  You can often gain a great deal of understanding just by reading about other software packages.

Respectfully,
Garland

Garland E. Borowski, PE
Star Aviation

The manager of my company has asked me to develop a set of Guideline and procedures for FEA models in general. The company has purchased Algor licence. What you have suggested to me in your last reply is a kind of procedures for modeling an analysis. What then is the difference between "Procedures " and "Guidelines " for FEA modeling ?

Your advices are quite welcomed.

Kind Regards,

One Point

I would look at "Procedures" as those processes which can consistently be followed for any and all situations.  For instance, you can always perform a simple comparison to your mesh size and modeling technique by modeling a circular plate under a certain load with certain boundary conditions and comparing it to the hand calculation in Roark's Formulas for Stress and Strain (accuracy verification).  The "Procedure" may also dictate that the size of the circular plate be approximately the same size as a key circular feature in your part or assembly that you will be analyzing.  This verifies that your mesh size is reasonably and that the software is calculating what you need it to calculate.

The "Guideline" would be that if the part's thickness is approximately 10% or greater of the shortest physical characteristic (the radius for our circular plate example), then you should use brick elements instead of plate.  "Guidelines" may also include other "rules of thumb" such as:  If 10% of the total stress range appears in any single element, you need to refine your mesh; or, if the "precision" dither in Algor shows greater than 0.2, refine the mesh; or, if the strain energy density is XX, then...

"Guidelines" can be violated if the area violating the guideline is not of interest so long as it is still properly defining the load path.  "Procedures" must be followed so that everyone is doing the same thing for each model.  "Guidelines", at least in my mind, relate more to the parameters in the model, where "Procedures" relate to the process of developing, analyzing, and post-processing the model.

Hi GBor,

Looking at what you have mentioned to me about developing Procedures and Guidelines for FEA analysis in Algor, I would like to ask you if it would be OK to consider the following list as Procedures to perform a FEA analysis and while working on each of those steps to introduce a set of most appropiate Guidelines related to the type of anylises considered.
So, should I consider the following as "Procedures" and then elaborate on each of them ?

As I am still a beginner in FEA i lack the knowledge of some topics regarding meshing quality and meshing refinement. What is a "mesh sensitivity" test and could you please suggest me 2 of the most easy ways to perform this?

                Finite Element Procedure
1)  Develop(create or import) the geometry of your object
2)  Apply a mesh to the geometry
    a)  Determine the type of mesh needed (beam, plate, brick)
    b)  Determine the mesh size or automesh parameters
    c)  Verify mesh continuity
    d)  Check for areas of needed refinement
3)  Determine and apply boundary conditions
4)  Determine and apply loads
5)  Analyze the solution
6)  Confirm results (testing, hand analyses, engineering judgement, etc.)
7)  Refine mesh and reanalyze (this is referred to as a "mesh sensitivity" test and I've seen it done many different ways)..



 

You basic steps look pretty good, but you will probably need much more definition if you are writing a procedure for a company.

As for the mesh sensitivity, there are two ways to do it.  One combines steps 6 and 7 of your procedure by developing a "validation model".  This model uses element types and loadings similar to what your global model will see, but it does so on a local model that has a known, empriacally-based solution.  For instance, if I am using plate elements to model the structure of a box, I probably can't easily hand calculate the deflection of the back face if my loading is a pressure load on the front face, but I CAN hand calculate the deflection of a simply supported flat plate subjected to a pressure load.  So, I model a flat plate the size of one face of my "box" and use finite elements of a specific size, I load the plate with a pressure and pin the edges.  I hand calculate what the deflection of the center should be based on Roark's or whatever theoretical method is avialable and I compare.  If it is reasonably close (5%?), I am comfortable meshing my global box with finite elements of the same size as those in my local model and applying the same type of load (pressure).

If the local model isn't close, you have to reevaluate the element types that you are using.  If you are confident that the situation calls for plates, then mesh with a smaller mesh size.  If the stress levels change by more than about 10%, your mesh isn't "converged", and you need to remesh even smaller.  You can do this iterative method for the local model or the global model as appropriate.

In Algor, there is a feature for "mid-side nodes".  This is an easy way of performing a mesh sensitivity analysis for certain element types (plates, bricks, etc.)  Run the analysis with mid-side nodes "off" and then switch the elements to mid-side nodes "on".  This places another integration point at the mid-point of the edge giving you a slightly higher order element.  If the results don't change significantly, your mesh size should be acceptable.

Do watch out for highly localized stresses.  Many times you can ignore them, but some engineering judgement needs to be exercised judiciously.

Hello GBor,

Thanks for your valuable suggestions. Regarding the meshing process could you please tell me what does it mean :
    A.  Verify mesh continuity
    B. Check for areas of needed refinement

How could I verify mesh continuity in the model? By visual inspection?

What area should I consider for mesh refinement?

Lets assume that my models could be an oil storage tank(linear stress analysis) or a pipeline(transient heat transfer analysis)or a pipile resting on supports(Linear Static Analysis)?

Looking forward to hearing from you.

Regards,

OnePoint

There are several way to "verify mesh continuity", but this basically means make sure that adjacent parts are properly attached.  I usually do this by first inquiring on the maximum and minimum length lines and using the minimum length that seems appropriate to set my search tolerance.  For instance, if my minimum length line returns a value of 0.125", I may set my tolerance to 0.1".  Then, I do a global snap.  This makes sure that nodes that are close, but for some reason not connected are apprpropriately snapped together.  This usually works sufficiently, but I am careful how I build my models.

Another easy way to tell is to run a modal analysis and look at the mode shapes.  Parts that aren't connected will "flop around".  Then you know what you need to tie together.

As for areas needing refinement, this is any area of interest where the stress levels appear to be high, but the stress gradient across a small area makes up a large portion of the stress scale.  For instance, if I am running an analysis on an oil storage tank and I see large stresses where the end of the tank is connected to the body of the tank, I may want to refine the area near this geometry to make sure I am capturing the true stress at this point.  The mesh sensitivity analysis usually takes care of this because you refine the mesh to determine if you get similar answers.

If you are going to do a lot of this, I recommend that you spend time watching the free webcasts that Algor offers.  I can't explain everything here at Eng-Tips and there are some valuable and freely available resources at www.algor.com or www.etechlearning.com.