Hello, I have evaluated the Von Mises results on a dummy model formed by two solid compenents and a screw with pretension by comparing Abaqus vs Calculix
On Abaqus the Von Mises stress under the screw’s head are much lower.
Why is there this difference?
Hard to say without seeing both models, we don’t know how you defined them and how they differ. There are some special considerations for pre-tension modelling, especially in CalculiX.
1 Like
that doesn’t fit my experience, I reproduced a model from Abaqus demonstration problems manual (based on a paper) showing good correlation: Bolt connection with pretension - #8 by JuanP74
1 Like
So you run this model in both Abaqus and ccx? Can you share a picture of the results that are so different?
I think ccx hard contact is not the same as in Abaqus.
1 Like
Is there some initial interference fit .
ajudt=NO is not ccx command.
1 Like
Initially, you’ve mentioned a model with 2 components and a screw between them. Did you expand it now? We would need more screenshots from both models (in CalculiX and Abaqus) to compare them or, possibly, the whole input decks to find out what causes the differences in results.
True. One must ensure that the contact and surface behavior are equivalent. Also, you need to ensure that there are no other contacts or boundary conditions that could cause a problem in ccx. It’s easier to help if the model can be shared and looked into.
I share[quote=“jbr, post:9, topic:2197, full:true”]
True. One must ensure that the contact and surface behavior are equivalent. Also, you need to ensure that there are no other contacts or boundary conditions that could cause a problem in ccx. It’s easier to help if the model can be shared and looked into.
[/quote]
No this is the layer of hexa elements that I create because a lot of video on youtube prompt this solution to avoid that during pretensio the c3d10 elements execeed deformation.
However yes it is adjust=No, I found it in the ccx manual
In PrePoMax, you have to use the boundary layer feature on compound bolt part for pre-tension section because of this requirement of CalculiX:
Furthermore, the user should make sure that the [pre-tension] surface does not contain edges or vertices of elements which do not have a face in common with the surface. Transgression of this rule will lead to unrealistic stress concentrations.
So basically, PrePoMax has to create a layer of wedge elements because they will all have their faces on the pre-tension surface (some tetrahedrons would have their vertices/edges on the pre-tension surface without sharing a face with it).
1 Like
Yes, I created it on prepromax from tool and create boundary layer.
deformed shape correlates pretty well so the discrepancies are related to element formulation and mesh density. In those respects calculix elements are not the same as abaqus so you shouldn’t expect same accuracy with same mesh. In both of your pictures due to stress concentrations and mesh density I’d say nor ccx neither abaqus can be considered accurate at that location. You need to refine if you need to know it with accuracy. Do not forget that in .frd file the results are always nodal averaged.
1 Like
Is that exactly the same mesh (from the same .inp) or just recreated with the same settings ?
To obtain accurate contact results with such notches, you will need much more refined mesh: Uniformly distributed load over selected edge - #4 by fteddy - General Questions - PrePoMax
But contact settings will also be important. I would check contact results (especially PEEQ but also other) too.
1 Like
maybe, it can try to disable Avg.75% plot setting in Abaqus before going further since the mesh look similar.
1 Like
Averaging in Abaqus can be disabled (won’t help here since CalculiX always uses averaging in .frd results so only comparison with .dat file stresses could be made) or set to a different % (also 100%).
indeed CalculiX always use averaging by extrapolated from integration point, but as i understand Avg.75% in Abaqus will exclude in extrapolation when some element contributes differ greater than 25% with another element sharing common nodes.
If the relative difference between contributions at a node is greater than the threshold percentage you set, Abaqus/CAE will not average the contributing values and your results will appear discontinuous at that node. Use a higher percentage to produce a smoother, more continuous effect.
another possible reason is in contact at curved surface, Abaqus may have some treatment to improve but CalculiX has not. Maybe using quadratic element with midside node fit to geometry can give insight about discrepancy.