Introduction:
The flexible body preparation for multibody applications (Component Mode Synthesis method), can be define into the Altair Simulation platform in different ways:
- Directly on MotionView client application, if is available the FE bulk data or different CMS formats (.h3d, .mnf), through the FlexBodyPrep tool.
- Using HyperMesh to prepare the input deck for Optistruct
- Using SimLab & Optistruct
In this article will be explained how to prepare the flexible body using the way 2 (HM + Opti) by exploring different options then control the amount of data content of the flexible body file, so control the size of the file.
All the different CMS results, are able to describe the deformation between the interface nodes, so produce the same results in terms of multibody simulation (if are not used for contacts), but the results details, varying related on what the used result file contains.
All the files used into this document is in available on the Community Altair Model Exchange: Bulk data example for flexible body creation (CMS) https://community.altair.com/sys_attachment.do?sys_id=5fee04c9976a8e1ce3b0361e6253af88&view=true
Starting model (model 00):
The model used is a mesh of a rod where the elements used are 3D tetra.
All the considerations done on this document are valid also with different type of mesh, who can be defined with different types of elements and related to that, different options described on this document, can be used and the level of reduction of size of the result files, can be different.
The model into HM appears as:
This model is composed by around 193000 elements (Tetra4), and 48000 nodes.
The center of the RB elements, is used as interface node for CMS.
Minimum setup for CMS run (model 01):
Starting on the inital model, the minimum info the define on the model are:
1- Define the interface nodes --> this is done by an ASET constraint placed on the related nodes.
These constrains are placed into a proper load set (can be named ASET), the DOF set are the modes who can be exited when the flex body will be used into the mechanism (by default all the 6 DOF for each interface node). The set of DOF constrained will produce the set of static modes of the CMS method.
2- Define an additional load collector to specify the CMS method and parameters used for the case. To the load collector created is assigned the CMSMETH solver card as below.
Trough that, is possible to define CMS method used (CB is Craigh-Bampton, can be used also CC) and the upper limit or the number of additional modes to compute (Eigen-modes) to represent the body deformation due to the internal force and mass distribution of the component.
3- Specify the units of the bulk data used. This is done by defining the solver card DTI_UNIT where is possible to specify the units used for the mesh and the associated properties (material, elements).
This is used by MotionView and MotionSolve to scale the model related to the units used into the multibody environment.
4- Into HM there isn’t a specific loadstep for CMS, but can be defined by the GLOBAL_CONTROL_CASE card.
This card is used to specify the CMSMETH card to use, where the CMS parameters are stored. The interface node specified as ASET, will be automatically taken in account (don’t use other constraints on the model).
After this definition, the model is ready to run on Optistruct who calculate the modal representation (CMS) of the model who can be used as is into the multibody environment (Rod_CMS_01.fem).
By default, the result file is an .h3d file, and contains the modal displacements, stress and strain of all the nodes and elements of the model.
For this model, the size of the result file (.h3d) is around 272MB.
Reduce the type of results on the result file (model 02):
Starting from the previous model, is possible to reduce the type of results stored into the result file by remove the stress and the strain who are by default stored.
For that is needed to specify the GLOBAL_OUTPUT_REQUEST solver card, where can set NO or NONE into the Option field.
In this case, the result file will store only the modal displacements on the component (Rod_CMS_02.fem is the related input deck).
In this way, for this model, the result file size is around 36MB.
Reduce the model visualization using PLOTEL (model 03):
Starting from model 02, is possible to define PLOTEL elements on the features of the component and store the results (displacements) only on those elements.
1-Create the PLOTEL: the model has solid elements then first extract the faces from the model and then extract feature edges from the faces. Then can be deleted the faces.
2- Define the MODEL solver card to define as only the PLOTEL elements are used to represent the model. Can be also avoid to visualize the rigid elements.
After these operations the model is ready to run (Rod_CMS_03.fem is the related input deck).
In this case, the result file size is less than 3MB.
Create a skin where the results are computed (model 04):
Starting from model 02, is possible to define a skin mesh on the solid elements to use as result visualization.
1-Extract faces from solid mesh
2-Assign to those elements a very small property (Thickness) and/or material (low stiffness and density) to don’t modify the component stiffness and mass.
3-Create a SET_GRID and a SET_ELEM sets with only the nodes and the elements of the skin component.
4-Use those sets into a MODEL solver card to define where to evaluate and show the results.
After these operations the model is ready to run (Rod_CMS_04.fem is the related input deck).
In this case, the result file size is around 19MB (only modal displacements).
Full results on skin (model 05):
Starting from model 04, remove the GLOBAL_OUTPUT_REQUEST to have all the results (modal displacements, strain & stress) on the skin.
After that, the model is ready to run (Rod_CMS_05.fem is the related input deck).
In this case, the result file size is around 77MB.
NOTE:
From a structural point of view on the skin is always reach the maximum level of stress or strain in all the loading conditions. Then this kind of result is enough for any kind of structural evaluation, also for durability analysis who can be used directly the flexible body results computed by MotionSolve.
CMS without visualization (model 06):
Is possible to reduce at the minimum the size of the flex body representation without store any model visualization but only the modal deformation between the interface nodes.
Starting from model 05 (or any other model, like model 01) use the MODEL solver card to set NONE on each option.
After that, the model is ready to run (Rod_CMS_06.fem is the related input deck).
In this case, the result file size is around 0.1MB.
The model is usable into MotionView & MotionSolve, but is not visualized. The behavior, in terms of motion analysis, is the same as the other models.
Coarsen skin mesh to compute results (model 07):
Like model 04, is created a skin mesh but not by extracting the faces of the solid mesh, but through the coarsen meshing tool. In this case, the resultant mesh contains the number of elements who is needed, by controlling the size and the simplifications who can be done. Is possible to apply this method not only to solid mesh but also to shell elements.
1-Staring from model 02, use the coarsen mesh tool with proper parameters. Use Retain input mesh.
2-Assign to those elements (coarsen component) a very small property (Thickness) and/or material (low stiffness and density) to don’t modify the component stiffness and mass.
3-Create a SET_GRID and a SET_ELEM sets with only the nodes and the elements of the coarsen component.
4-Use these sets into a MODEL solver card to define where to evaluate and show the results.
After these operations the model is ready to run (Rod_CMS_07.fem is the related input deck).
In this case, the result file size is around 2MB (only displacements).
All results on the coarsen skin mesh (model 08):
Is the model 07 without the GLOBAL_OUTPUT_REQUEST card.
After this operation the model is ready to run (Rod_CMS_08.fem is the related input deck).
In this case, the result file size is around 5MB.
Recap:
The ways described into this model, to control the contents and the size of the result file for a CMS analysis, are the most commonly used, but not the only ones definable into HM for Optistruct. Additional and a combination of parameters are available to select which results are interested to compute and store and in with elements is needed to store.
Here a summary of the model described.