The objective of this tutorial is to show how to use the Multi-Domain technique.
The model used is a low speed pole impact on a bumper system. Note that the model is
finely meshed (average mesh size = 2mm) in the region of the pole impact and
coarsely meshed (average mesh size = 10mm) elsewhere. 図 1.
In order to run this analysis using Multi-Domain technique, we have to split this
model into two domains, one containing the finely meshed region and the other
containing the rest. A node to node link (/LINK/TYPE4) is then
specified at the boundary between the two domains.
These domains will be created using a pre-processor (using HyperCrash in this tutorial) and the options specific to
Multi-Domain analysis will be added to the input decks through a text editor. A
Multi-Domain main input file will also be created using a text editor.
Set the User profile to RadiossV2022 and the Unit system to kN mm ms.kg.
Set User Interface style as New.
Set your working directory to where the downloaded file is located.
Click Run.
Click File > Import > Radioss.
In the input window, select monodomain_0000.rad.
Click OK.
Create Input Files
Click Model > Control Card to set the Control Cards, as shown in the following images:
図 2.
図 3.
図 4.
Click the Tree tab and select
the subsets
of the fine-meshed region (subsets BB_fine1 (21),
BB_fine2 (24), and fine_mesh
(69)), then right-click, then click Export
Selection.
図 5.
In the Export Selection window, select the option to
Add model’s control card not linked to any part,
toggle Export geometry and select ALL POSSIBLE
RELATED ENTITIES.
図 6.
Click Ok.
Save the file as fine_mesh.
This will write the file
fine_mesh_0000.rad.
Click Model > Control Card and enter the following Control Cards:
図 7.
Click the Tree tab and select
the
subsets/spotwelds of the coarse-meshed region, then
right-click Export Selection.
In the Export Selection window, select the option to
Add model’s control card not linked to any part,
toggle Export geometry and select ALL POSSIBLE
RELATED ENTITIES.
図 8.
Click Ok.
Save the file as coarse_mesh.
This will write the file
coarse_mesh_0000.rad.
Define the Links between Two Domains
In the original single model, the fine meshed region is connected to the coarse meshed
region at both ends. When this model is split into two domains, we have to create a set
of nodes in both the domains and link these node sets through the Starter option
(/EXTERN/LINK). This option has to be added to the two Starter
input files using a text editor. 図 9.
Open the Starter file coarse_mesh_0000.rad and add the
option /EXTERN/LINK, as shown below:
図 10.
Two external links through node sets 1001 and 1002 have been added to
this domain. These node sets were already defined in
monodomain_0000.rad and exported to the two domains in
Step 1.
Open the Starter file fine_mesh_0000.rad and add the same options.
Create a RAD2RAD input file input.dat defining the two domains and specifying the connections between them.
図 11.
The input files are now ready to be run using the Multi-Domain
technique.
