This eSeminar is part of a series of eSeminars being run globally which talk about the Power of the Portfolio. As such they tend to focus on the portfolio products such as Abaqus, Isight, fe-safe or Tosca. This replay of the eSeminar is about 50 minutes long and tries to look at some of the overlooked features in Abaqus. Some of topics covered are
- Automatic Contact Detection
- Threaded Contact
- Surface Smoothing
- Penalty method
- Job Diagnostics
- Error Indicators
- Pressure Penetration
The webinar was run live three times for different regions around the globe Please find below some of the Q and A from these sessions. If your question was not answered during the webinar or as part of this follow up then please contact your local office with the support question.
1) Does Simulia provide some general/default material library with some common, often used materials?
A) No. Simulia never provides any sort of material data.It is however possible for you to get material data from a 3rd party and store it in the material library functionality within Abaqus/CAE.
2) Contact diagnostics useful once you get past step 1, but is there any way to understand contact problems before step 1 has fully converged?
a) Contact diagnostics tend to give the whole model overview over the whole history of the analysis. Even if step 1 has not fully converged you should be able to open up the odb and have a look at the attempts that have been made before the analysis failed. Typically speaking in a static analysis having a displacement control as opposed to load control tends to help contact establish after which the user can shift to load control. For specific convergence issues please get in touch with your local support office. Also the default output behaviour has been changed in 6.14. The default output behaviour has been modified to output the last converged increment when convergence is not achieved. The output is written only if there are convergence difficulties beyond the first increment. This default behaviour is available for all general steps in Abaqus/Standard.
3) Are cylindrical elements available in Explicit?
a) Cylindrical elements are currently only available in Abaqus/Std.
4) Can you use cylindrical elements for buckling problems?
a) For an Eigenvalue buckling prediction analysis, yes you can use the cylindrical elements. Under this analysis type in the manual you can see under the elements section that any of the stress/displacement elements in Abaqus/Standard (including those with temperature or pressure degrees of freedom) can be used in an eigenvalue buckling analysis, with the exception that hybrid and contact elements cannot be used with the Lanczos eigensolver
5) Are the linked viewports in just CAE or in viewer as well?
a) Linked Viewports are available in both Abaqus/CAE and Abaqus/Viewer.
6) Does the automatic contact detection work with shell offsets and shell thicknesses for orphan meshes?
a) Yes, Automatic contact detection should take this into account for orphan meshes.
7) When max residual force is high comparing to avg. force and caused the run to diverge and die without SDI warning, what do we look for to resolve the issue?
a) When such a scenario occurs then the lack of SDI could indicate that contact is not the problem. In such a scenario checking the magnitude of loading, BCs, unit systems to ensure that we are applying the load that we think we are, and checking the incrementation size should help.
8) Can cylindrical elements be used to model steel components, say long pipelines?
a) Yes, they can be used to model pipelines. However element selection is also dependent upon the analysis conditions. You might want to consider that Abaqus also provides pipe elements to model beams with pipe cross-sections that are subject to internal stress due to internal and/or external pressure loading.
9) Can cylindrical elements be used to model non-circular cross sections? Eliptical cross sections?
a) Cylindrical elements are meant for modelling structures that are initially circular but are subjected to general nonaxisymmetric loading.
10) When requesting results for exterior surfaces only, how does that affect stress/strain results at nodes? Does this also mean I won't have access to integration point results?
a) This is effectively an output request. When this exterior option is toggled on when requesting results only the exterior nodes and surfaces will carry the results. The rest of the model in the interior will not store results and hence you would not have access to the integration point results for all the elements. It is essentially meant to be an odb size management option.
11) Exterior only field output applies to individual instance? How about for some instances embedded in another instance?
a) This option only applies to the whole model and cannot be applied to individual instances.
12) We use coating of membrane elements for stress recovery from the face of the solid element. Can that be replaced by exterior output option that you explained?
a) See answer 10. If that satisfies the output that you get from membrane elements then this can be used. However note that this can be only applied to the whole model and not to particular sets.
13) Can you please compare Penalty approach and *Contact Control- in addressing contact chattering issue?
a) They are both complementary to each other. I would recommend starting with the default penalty and then using contact control. Essentially both are operating on the stiffness values and are multiplicative in nature. If that does not work I recommend taking the contact control off and then trying order of magnitude changes in the values of the penalty stiffness.
