Abaqus, ANSYS, Algor, Mechanica which is the best? 8

[mechengr1313]

I am at a company that has Algor and Mechanica but believe we are approaching the limits of our current software. I have used ANSYS in the past, about 3 years ago and know it is a fine program. Does anyone here have any experience with both Abaqus and ANSYS and could give me a comparison for the two programs. We build large assemblies on the order of heavy equipment and we want to look at how the entire structure behaves in a twisting enviroment. I have modeled parts of assembly in Algor but am having problems now getting the mesh to go though the solver with the large assembly. I am exporting the geometry from Pro/e and was going to have Algor do a midplane mesh of the parts due to their thin structure shap but that has failed due to the mesher not being able to provide a continuous mesh without holes. What I am wondering is, who in your opinion has the best mesher for thin sections and which one works well with large meshes? In my opinion, a large mesh is around 2,000,000 elements. One last thing, should we even mess with Mechanica or get something else? Thanks for your advise in advance.

Mark

 

[GBor]

Johnhors,

I don't know a great deal about the actual implementation of Mecahnica, but I've usually seen it used for analysis of thick materials under very large bolt heads. I am not familiar with Mechanicas tetrahedral element formulations. I know COSMOS has a good tet formulation. Algor's and NENastran's are pretty good, but often misused. I generally move to 8 to 20 node bricks (and, yes, that may be hexahedral shaped elements).

Garland E. Borowski
Borowski Engineering & Analytical Services, Inc.

 

[johnhors]

GBor

In an ideal world I would use 20 node bricks as well, however I have to mesh very complex 3D solids which I am not allowed to simplify, the only practical solution is to use tets. I don't understand your concern's with tet element formulations as I thought that this is well understood and certainly for h-method analyses any FE package will generate identical results for linear analysis using conventional ten node tets (with the exception of modified tets in Abaqus).

ParabolicTet

Rigid links (like RBE2 in Nastran) should be avoided in FE analysis, they are highly artificial and produce meaningless results. An Abaqus tie is best avoided as well but it is not the same as a rigid link it simply glues disparate meshes together, the "tied" meshes are still free to flex and stretch, the tie provides continuity of dispacement but not stress.

 

[GBor]

Johnhors,

Sorry, the concern over tets is not with the element formulation, but with the application. Same is true of any 3-D element for h-methods...I would use more than 1 through the thickness (actually, I would use more then 2).

I used to work for a large defense contractor. A sub-contractor brought me an analysis report of which they were quite proud. They had meshed the entire solid model in tets because "that's the only way the computer could do it". It had single tets through the thickness and on quick inspection, had CLEARLY missed the stress dither...there were no stress increases around stiffening elements under heavy load. I wasn't sure whether to question the software or the engineering staff of the subcontractor. I was very familiar with the FEA package and knew the element formulation to be correct. The problem was in the application.

Garland E. Borowski
Borowski Engineering & Analytical Services, Inc.

 

[johnhors]

GBor

I agree 100% with your comments. In fact I would extend them, firstly just about any FEA software will deliver excellent results IF driven correctly. Secondly mesh on a first pass should be fine enough to pick up concentrations in obvious locations, subsequent runs with finer a mesh should be applied until stress values converge (commonly called mesh convergence). Thirdly apply CORRECT and REALISTIC boundary conditions. A balanced load and moment approach with minimal supports should always be used (i.e. the sum of loads in any global direction equals zero, taking moments about any global axis should also equate to zero, if this is employed correctly then minimal 3 - 2 - 1 supports can be applied which will prevent rigid body motion and rotation, but will not react any load).

Unfortunately, probably the vast majority of FE analysts tend to apply loads at one end and fix the other, thus reducing all their models to a cantilever (arguably a mathematical entity that doesn't actually exist), simply reverse the clamped and loaded ends to see a completely different set of results!

 

[GBor]

Well Said! Well "Spoken"!

Garland E. Borowski
Borowski Engineering & Analytical Services, Inc.

 

[mloew]

johnhors,

You have no idea how many times I have had to convince analysts of this approach. Thank you for stating it so clearly in your post.



Best regards,

Matthew Ian Loew


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

 

[johnhors]

Matthew and Garland

Thanks for your kind comments.

I've always regarded FE as a tool, albeit a very powerful tool. But as with all tools there is a correct way and a wrong way to use them. You wouldn't put a chainsaw in the hands of an ill-trained user, or a learner driver in a racing car, would you? Yet everyday we put such people in charge of FE analysis tools, which could potentially cause far more damage than the chainsaw or racing car.

I started my career as a stress man in the late 70's, working at Longbridge, Birmingham UK, a big car manufacturing plant, analysing anything and everything found on a car. For every component I was taught to draw out a free-body diagram and label all the forces acting on it. It was then quite natural to perform a check load and moment balance, before proceeding with stress hand calculations. I have always striven to run FE analyses the same way, thereby avoiding the false stress concentrations that the incorrect "everything is a cantilever" approach produces. Additionally, I NEVER apply point loading to a solid model, not even via a rigid body element! Variable distributed pressures that closely mimic actual contact conditions produces much cleaner results.

best regards
John

 

[antti]

RE: the original (old) question), we are in the lucky position of using many of the codes mentioned in this thread. If I had to make do with one, then it would have to Abaqus, mainly due to the large amount of contact analysis we do, since I work for a brake manufacturer. I'm not trying to be the Abaqus salesman either, just my personal preference.

 

[feadude]

johnhors
What do you mean by
"minimal 3 - 2 - 1 supports"
Thank You

 

[johnhors]

Feadude

Any single unsupported part/component has six degrees of freedom that do not involve any internal strain energy, three in translation and three in rotation. A 3D natural frequency analysis of an unsupported part will produce six zero frequency modes, one for each of these freedoms, these are usually called the “rigid body” translations and rotations because the part does not deform. The stiffness matrix of an unsupported part is singular (i.e. no inverse or flexibility matrix exists). In natural frequency analysis this problem is easily overcome by applying an eigen shift which makes the stiffness matrix non-singular. However with static linear analysis there is no equivalent to an eigen shift and it is impossible to solve the problem without applying supports. What minimal 3-2-1 supports do is ground the part to remove the six rigid body freedoms in such a way that they apply no restriction to any internal deformation of the part. For example consider a part that has three widely separated and easily pickable points/vertices in the global XY plane. Point 2 is chosen to share the same Y and Z coordinates as point 1 (i.e. point 2 is offset a distance x from point 1). Point 3 lies in the XY plane but it MUST NOT be colinear with points 1 and 2 (i.e. all three points must not lie in a straight line). Now point 1 is fixed to earth with x = y = z = 0 , all three translations are fixed, which removes the three rigid body translations of the part. At this stage the part is still free to rotate about point 1 in any direction. Next point 2 is fixed to earth with y = z = 0. The part has now just got one rigid body rotation left. It can freely rotate about the vector between points 1 and 2. This last rigid body freedom is then removed by fixing point 3 with z = 0.

Of course there are many variations that can be used instead, a similar approach can be applied to any of the global planes, or if there is no convenient global plane available then a local axes system will suffice.

However it is achieved the number of supports must equal six for a minimal support condition, any less and the structure is under supported and is insoluble, any more and the structure is over constrained.

When used correctly, the supports will not react any load SO LONG AS a fully balanced set of loads and moments is applied.

I hope that this explains it for you.

 

[feadude]

johnhors
thank you