Abaqus, ANSYS, Algor, Mechanica which is the best?
Abaqus, ANSYS, Algor, Mechanica which is the best?
(OP)
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
Mark





RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
There can be no advantage in using thin shell elements as you have 6 dofs per node whilst a brick model has 3 dofs per node, but twice as many nodes. For that reason you might be better just meshing it using bricks, wiht one elemnt through the thickness. That would solve the pronlem of mid-plane meshing.
Look at other posts for a comparison of software. For linear problems they'll all do the job. For non-linear/contact analyses Abaqus is probably better.
corus
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
With only one (linear) element through the thickness, it is not possible to pick up the proper stress distribution from bending. At least three nodes through the thickness are required to model the parabolic nature of bending stresses.
Also, ANSYS has recently solved a 100 Million + DOF model on a single computer. There is no practical limit anymore for model complexity WRT solving. Meshing is, of course, another issue.
Best regards,
Matthew Ian Loew
Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
In addition, there is a problem with using shell elements along the mid-plane in that you are left with gaps between each plate. This can involve either time consuming stitching together of the parts or having to stretch one or more plates to make them join at coincident nodes. This gives rise to errors at the intersection with too much material. This is why I'd consider using brick elements first if I were importing a CAD drawing.
corus
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
I am not referring to the bending displacement, but the stress profile through the section. Less than three nodes through the thickness will not pick up the correct stress pattern even though the displacements might be accurate! As far as the midplane shells, most FEA packages handle these offsets just fine. MECHANICA and ANSYS (packages I am familiar with) handle the connections (welds, fasteners, etc.) very well indeed.
Best regards,
Matthew Ian Loew
Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
Mark
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
I know that ABAQUS has the facility to tie disparate meshes together. What it amounts to is a special form of contact, in which the "slave" surface's nodes are tied to the master (thus the displacements are locked to the interpolated displacement of the master surface). Thus there are effectively no artificially-induced stiffnesses (such as would come out of RBE2 linkages between the parts).
At the time it came out, only ABAQUS had this capability.
ANSYS didn't have this, but my information may be dated (Matt, do you know?).
---
Regarding the original question, there is no "best" FEA software for all users. The answer is user-dependent and is a mixture of several important criteria:
1) Problems to be solved
2) Amount you are willing to spend
3) Constraints within your environment
a) what data format is provided to you
b) what data format is expected from you.
1 and 2 are generally pretty straightforward--the more complex #1 is, generally the higher #2 is. There are a few exceptions, but this is a general rule.
ALGOR is fairly capable of linear problems, but as the problems get more complex its functionality becomes limited. Likewise Mechanica. Both have some nonlinear capabilities, but nobody doing detailed rubber analysis would likely use either of these codes.
ALGOR, however, is inexpensive. Mechanica is nicely embedded into CAD software, thus it has its obvious strenghths.
ABAQUS and ANSYS are both very capable codes in linear analyses, and are also both very strong for nonlinear analyses. However they both cost significantly more than ALGOR.
In a sense this is like asking "which is better, a Cadillac CTS or a Chevrolet Malibu?". Most would agree that the Cadillac is a "more capable" car, but that doesn't mean that most would buy the Cadillac (since the price has a big impact).
Regarding my point #3--a very critical though often overlooked set of requirements is what form your initial data takes (CAD data that you make? CAD data from your company or anohter company? FEA meshes from somewhere else?). Likewise, what form are you expected to deliver--in automotive many Tier 1 companies are expected to provide runnable models for the OEM's. Implicit in this is the fact that it must be in a form which OEM's can run themselves (thus negating the possibility of "non-OEM" FE packages). These "constraints" can dramatically impact the decision-making process for purchasing an FE package.
---
Finally...
Always be wary of people who advocate one code as being absolutely the best for everything. They are generally either selling the code, or else they don't have a wide enough experience to be able to seriously evaluate the various codes.
Brad
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
I have been using ANSYS with a Mechanical desktop front end. The models are built as solid models with in the CAD package and transferred to ANSYS through a software called a plugin inside a new interface called workbench. I have worked with assemblies haveing a large number of parts. The transfer of geometry has always been flawless. I beleive that ANSYS will handle a problem of the size indicatedd by you ( 2 million elements). Run time will depend on the computer hardware you use.
Also workbench creates contacts automatically. It does auto meshing. But sufficient controls on mesh are provided to tailor the mesh to your need. I will recommend that you look at ANSYS workbench software. It is very good for modelling assemblies.
Thanks,
Gurmeet
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
Mark
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
What I'm looking for specifically is this:
o A good mesher, perferably one that does mixed meshing of volume elements. I need this as I often have to mesh suspended (ribbon) membranes using brick elements on complicated compliant constraints which can be meshed with tets.
o An FEM tool which allows mixed mesh elements types in one model.
o A CAD/FEM package like CosmosWorks which seamlessly integrates design geometry variations with FEM.
o Multiphysics to handle piezoelectrics and mixed orthotropic material types in one FE model.
o Geometric nonlinear and material non-linear problems.
I have been leaning towards ABAQUS, but I am worried about not having a good mesher front-end, and losing the geometry parameter variational study within CosmosWorks.
Any suggestions, or any links which compare various tools such as ANSYS, ABAQUS, I-DEAS, UniGraphics, NASTRAN, etc. would be appreciated.
Thanks!
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
I looked at Abaqus and ANSYS and we bought Abaqus this week. I think they are both very good programs for what we are doing, ie. very large assemblies. The reason we went with Abaqus was, their salespeople are engineers and actually knew how to run the software and not just a preplaned demo. I would call them and ask them to take your problem and show you how they would solve it using Webx so you could watch. Just have them prove it will work before you buy it. I would make any company show you their program will do what you want before buying it. After you buy it, salespeople tend to forget why you bought their program in the first place. Check this out Thread727-67468 interesting advice. Hope that helps a little.
Mark
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
David R. Dearth, P.E.
Applied Analysis & Technology
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
I've now in the process of defining a non-linear package for my new employer and would totally agree with the comment to get the suppliers to prove their product on your product. I'm pitching Ansys against Marc - any comments for or against ?
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
Brad made some vary good points and, fortunately, recognized his own limitations in certain areas. I have used Algor, NEiNastran, COSMOS, and many specialty packages. Algor continues to enhance their user interface, but their engine is sound (including non-linear). "Bang for the buck" Algor is hard to beat. NEiNastran is good competition as is COSMOS. Each have their strengths.
I am generally leary of anyone that says "Stay clear of ..." This is a competitive industry. If something didn't work, and wasn't getting supported technically, the package would have long since been out of business. NEiNastran is based on the Cosmic Nastran kernel. A good package, but it is still maturing. Teaming with FEMAP was smart because that gives it CAD capabilities and the ability to translate to a variety of packages. COSMOS has a very sound engine. Now that it is owned by the same company that owns SolidWorks, we will likely see continued growth in the interface beyond the current COSMOSWorks that is available. Algor has remained fairly independent. The greatest advantage, perhaps, is that there is one person to contact for all your needs, and they are very responsive. As for the question about highly non-linear materials, all of these packages (which I would consider mid-grade) have Odgen strain models in addition to the general hyperelastic models. The analysis code is well-understood and well implemented.
For a model your size, the p-element convergence codes (like Mechanica) are generally very effective. They reduce the number of nodes (and, therefore, calculation overhead) by orders of magnitude.
The higher end codes, like Mechanica, Ansys, and Abaqus, are excellent if you need to afford them. They are great for fracture mechanics and specialty applications, which it doesn't sound like yours qualifies. As for limitations on any of these or the other packages, most of the limitation is in your hardware, not the software.
I'm all for gaining additional capability, but remember, I'm a consultant that has to interface with many different people using a variety of packages...if you have the tools, learn how to use them, don't just assume you need new ones.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
http://web.peoriadesignweb.com/calculator - Online Engineering Spreadsheet Caclulators
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
Garland E. Borowski
Borowski Engineering & Analytical Services, Inc.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
With "bricks" don't you mean tetrahedral elements?
Bricks are commonly used to refer to hexahedral shaped elements.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
Mark
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
http://web.peoriadesignweb.com/calculator - Online Engineering Spreadsheet Caclulators
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
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.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
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.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
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.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
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!
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
Garland E. Borowski
Borowski Engineering & Analytical Services, Inc.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
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.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
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
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
What do you mean by
"minimal 3 - 2 - 1 supports"
Thank You
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
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.
RE: Abaqus, ANSYS, Algor, Mechanica which is the best?
thank you