first of of all PrePoMax seems to have the best Interface from all Free FEM Program which i really like.
I am a Beginner in Non Linear FEM Calculations but i want to learn it better.
I am currently try to recalculate some examples from our civil engineer for better understanding.
Model:
Clamp out of an extruded Aluminium Profile 2mm thickness which will be later fixed onto another profile.
Sorry i can just upload one image and one links, so i have put here all pictures inside and the prepomax files on wetransfer::
Material: EN-AW 6063 T66 Aluminium
RP0.2=200N/mm²
RM=245N/mm²
A=8%
For the calculation another safety factor 1.1 will be applied (Eurocode)
200/1,1=181,82
245/1,1=222,72
Our civil engineer is using commercial products from Civil Engineering etc.
He is using for each mesh with thin walled models a mesh with minimum 3 elements over the thickness. For contacts he is using for surface springs (not possible like Ansys and more easy).
What i have done until now (see PDF in wetransfer):
A=Contact Areas modelled into 3D Program with 0.001mm depth that it can be selected in FEM program, there will sit in reallity washers/nuts
B=Contact Areas modelled in 3D Program with 0.001mm depth that it can be selected in FEM.
There will be applied surface springs later
Spring Stiffness on B:
Non linear Geometry on:
Concentric Force each 550N applied to Areas A:
But i am not getting any results, if i remember correct it was everytime message like: No Results found etc.
Would be great if someone could help me.
Many thanks in Advice!
That’s why there are issues with meshing (mentioned in the pdf file). You should create a surface partition instead. It can be easily done in FreeCAD. Other CAD software usually allows it in some ways too.
I edited now to Surface Tractions, unfortunatley i am getting now error:
Error in u_realloc: error allocating memory
Guess it is my shitty home pc? I can try tomrrow with good hardware.
Surface partition:
I am working with Inventor, may you have a links?
For Freecad i also did not found on google may its a little bit otherwise called?
You may have to reduce the mesh density, it’s way too dense for tests. But you should also set the number of CPUs for parallel processing and maybe switch the solver to Pardiso.
I found now out how split function in Inventor will work, remeshed with overall 10.000elements.
Used Surface Tractions instead of Concentrated force and it worked fine.
I am having in the office a new Intel i7-13700k with E-Cores, do you recommend to turn E-Core off in Bios?
Is my plasticy defintion fine?
Its True Strain right?
How should i enter yield stress at zero plastic strain?
Aluminium is given with RP0.2 in all Eurocode definitions: The 0.2% offset yield strength (0.2% OYS, 0.2% proof stress, RP0.2, RP0,2) is defined as the amount of stress that will result in a plastic strain of 0.2%
Or should i enter RP0.2 as 0? i guess i does not really matters.
SO
181.81 0 [%]
222.73 0.08 [%]
If you had yield strength (stress at zero plastic strain) then it should have been the first. But if you only have RP0.2 then you can assume it corresponds to zero plastic strain and enter it as the first value with 0 strain to be followed by the tensile strength, for instance.
thanks make sense. Often, the yield strength of materials is not pronounced and therefore cannot be clearly determined in tensile tests. In these cases, the so-called replacement yield strengths or yield strengths are determined. As a rule, the yield strength is determined at 0.2 % plastic elongation, hence the designation of the parameter with Rp
Its typical for Aluminium.
Had today some good results on the FEM workstation.
Without activating E-Core i got some problems (PC hanging up).
What is interesting and what i don´t understand:
Calculation works fine with Mesh lets say 300.000pcs, but when i am making the mesh more fine lets say with 700.000pcs i am getting no results found (no settings changed just the mesh size).
Why? Should i change solver to Paradiso?
Issues with larger meshes in CalculiX have been reported several times. Pardiso seems to be the best choice. But you should always make sure that you really need such a dense mesh. Ask yourself:
Can it be refined only locally while leaving much coarser mesh away from the regions of interest ?
Can symmetry be used ?
Can shell elements be used ?
Do the results change significantly when the mesh is refined to the current level ?
It’s better to start from the other limit, from the coarser mesh to the more refined one.
With the latest additions of gmsh, this problem could be easily mapped and meshed from a shell using hexa elements, at least four elements thru the thickness, and have those bolt holes refined with 6 or 10 rings. If done correctly, you could even create a script to run your mesh sensitivity analysis without much effort.
Thanks very much!
I found out that Paradiso Solver works on Workstation great with 1.3Mio Elements in quite 10-20min calculation time, difference arround 20N/mm² to lets say 300.000 Elements (which is also quite good mesh).
I also found now out that i have to enter the true engineering stress and strain instead of the Engineering strain from Eurocode. Could someone please check from this link if i have done it correct?
I am sorry for the units and crazy numbers.
From Eurocode definition:
RP0,2=fok=200N/mm² (yield strength)
fuk=245N/mm² (tensile strength)
Safety factor ym=1,1 to fok und fuk.
Strain=8% from Eurocode
Interesting for me is that no difference is in calculation results with true stress vs. engineering stress in a high density mesh?
For me also interessting:
Our Structural Engineer is using SOFISTIK as commercial FEM solver, he is also using spring elements as contact simulation. From what i understand is that he can use the springs as tension or compression only. As i saw from his material definitions SOFISTIK is also using engineering stress instead true stress.
From his results: 0.9mm instead of 0.6mm deflection (ok we need to compare spring stiffness)
His stresses are about 40N/mm² lower (arround 180N/mm²) (he don´t go much into plastic areas) were my results are quite on the tensile strength with ~220N/mm². He is using also a quite high density mesh with currently unknown spring stiffness (i tried different ones to reach almost the same deflection).
Can somebody explain the difference between Surface spring and the compression only constraint?
As far as i could understand instead of surface spring i should more use the compression only?
Sorry for that many question, many thanks in advice!
PS: is also planed to have a tension only constraint (e.x. simulation the spring stiffness of a screw or bolt anchor etc? on a surface?).
Looks good at a first glance. Btw. there are online calculators that convert engineering and true stress.
Surface spring acts in both directions - it’s just a bunch of spring elements with a specified stiffness. Compression-only constraint, as the name suggests, acts only in one direction. Internally, it uses GAP elements that are basically primitive contact elements. You should always use this constraint with NLGEOM enabled.
Try setting very low compression stiffness and high tensile force for compression-only constraint.
ok thanks, so as i learned everytime use compression only constrain with NLGEOM.
Will check the next days with workstation, with high density mesh i got Iteration error with compression only constraint and paradiso. But its working quite good with less density mesh on my shitty home pc.
Great community thanks!
I will check out Version 2.0 Release.
-Elongation is the length change of the specimen at failure divided by the initial reference length. Outside the necking zone the strain stops at the value reached at ultimate load. Inside the necking zone, the strains are higher. The elongation is not usable as it is an average over the whole reference length.
-Your hardening model should be valid up to the maximum plastic strain occurring in the model. To be safe, it is recommended to limit plastic strain.
As suggested by EN 1993-1-5 .
C.8 limit state criteria
NOTE 1: The National Annex may specify the limiting of principal strain. A value of 5% is
recommended.
