Could anybody prepare complete kit of solvers for PPM/ Calculix to solve large problems . So far I have used several variants of 2.19 and 2.20 for windows os without success . I stiil can not resolve model with 4,5 milion of nodes even using Iterative solvers (error in u_realloc: allallocating memory) I have also searched in calculix forum and found dynamici8.exe but it also doesn’t work
best regards
The most complete package for ccx 0.20 can be found here: PrePoMax
If this (especially Pardiso) doesn’t work then it’s unlikely that any other (especially older) version will work.
I think that it would be better to keep this discussion on the CalculiX forum. There it’s much more likely that someone will help with your problems related purely to the solver.
Do you really need a model with 4.5 million of nodes?
1 Like
It will be very hard to reduce model. Similar model was calculated in Creo simulate but this is completely different software( also calculated as solid ,not shell ) .
Sometimes one has to “invest” some time simplifying the CAD (remove small features, holes…), or the FEA model (swithing to shell or beams models, replacing contacts with TIE or fusionating bodies in CAD) in order to have a model that can be solved in a razonable time with the available resources (soft, hard, human time…)
this model is totally simplified in my opinion (exept of shells). In real this structure has ca 65 ton weight and ca 40 m lenght
Then probably you should consider using shell and beam elements, maybe even using other solver as Mecway that allow you to work with different kind of beams and real shells.
I have made sample as one solid - cuboid , then meshed with solid elements . I have obtained over 3 million elements and over 4,249 million nodes , next step was adding material properties bonduary conditions applied forces . Finally model was solved without any problems . I assume that solver is not problem. What you think ?
1 Like
I think (not quite sure if I remember correctly) allocation of necessary memory for computation is based on the highest node number in the model. If you add a single node with a very high number, you might get that error, even for small models. So If the node numbering of your model is not continious, you might have some very high node numbers that cause the problem. Maybe there ist a way to renumber all nodes?
Maybe what i meant were element number. See the Last couple of Posts Here…Why is Moment load in conjunction to Pressure and Gravity not solving for more than 10mins on 6 cores - #19 by datsnl
Finally I have solved large problem by using pardiso with additional settings
but results are very strange total “0” stresses displacements and so on
best regards
When the solver gets out of memory, it fails to writte the results. Definitely you must use shell element in such kind of structures.
It seems there is some symmetry ¿isn’t it?
Maybe you can take some advantage of it.
Loads are not symmetric … acc to eurocode
I have question for 64 gb ram is it possible to solve linear static model with 4,5 millions of nodes I mean ooc version for pardiso or less convenient Iterative cholesky ?
best regards
I would recommend simplifying the model or using a coarser mesh and then using sub-modelling to analyze the critical parts of the model PrePoMax & CalculiX - Submodel - YouTube
I have solved this large model by using iterative solver (Cholesky) but I have noticed some problems see attached photos Have You got any idea how to solve it
best regards
Enable adjustment and increase tolerance for this tie constraint.
I am interested in the time it took to solve such a large model.
Ca 30 hours model was reduced to ca 2,5 million nodes