Table of contents
In this blog, we’ll demonstrate a transport simulation of steel rod bundles (Figure 1) in Abaqus. During the transportation of bundles, many rods are packed in a bundle and several bundles are placed on top of one another. The contact modeling with contact pair is complex and not practical for such a big model with many parts in it. Therefore, the General Contact modeling method is used. Furthermore, an interesting method to place the bundles on top of one another such as ‘create instance from models’ is used. The packing straps usually fails at weld points; therefore, connector failure modeling is used to model the weld points failure.
Figure 1: Steel rod bundles (left) and transportation of bundles (right).
To demonstrate the transport simulation of bundles, five different parts (Figure 2) such as steel rod, steel strap, steel rope, wooden block and U-shape containers have been created in Abaqus. In reality, the bundles are placed on wooden blocks or steel bars. Since the failure of straps at weld points for maximum load is interesting, only vertical lift or drop of the bundles are simulated. Six bundles will be placed on top of one another, and maximum load will be carried by bottom of the bundle and failure would takes place for the straps of the bottom bundle.
Figure 2: A bundle assembly in Abaqus
The following dimensions and information are used to create geometries:
The solid rods are modeled as 3D-Wire and assigned with beam element section. For the current example, 3D-Wire with beam element modeling is very practical since it reduces total number of elements when compared to 3D-Solid model with volume elements. Hence, the total calculation time can be significantly minimized.
Figure 3: A single rod created from 3D-Wire then assigned as beam section (left) and a bundle contain many rods (right).
Straps must be rolled over the rods once and welded at the ends.
In reality, steel straps or textile ropes are used to pack the rods during the transportation. In the current example, steel straps are used. Straps are modeled as 3D-Shell and shell section has been assigned.
Figure 4: A strap created from 3D-Shell.
Three U-shaped containers
Height: to hold six bundles
Figure 5: A U-Shaped container created from 3D-Shell.
The containers are useful while transporting and to store the bundles, they hold the bundles firmly. In current example, containers are modeled as 3D-Shell and assigned with shell section.
Steel ropes are modeled to lift the bundles. In general, the ropes are tied to the crane end and lifted with bundles and the bundles are placed in containers. However, in the current example only ropes are modeled and at the end of ropes displacement boundary conditions are applied to lift the bundle. These steel ropes are created from 3D-shell option and assigned with shell section.
Figure 6: A steel rope created from 3D-Shell.
For the current example, a bundle has 24 rods and tied with seven straps and transported with the help of two ropes.
The rods are generic steel with linear and plastic material properties.
The straps, steel rope and containers are generic steel material with linear properties.
The wooden blocks are also defined with linear material properties.
There are no special meshing techniques used in the current example, and homogeneous solid, shell and beam meshing are performed for all parts.
Table 1: Element type
Figure 7: Shell mesh for straps (left) and Solid mesh for wooden blocks (right)
Figure 8: Shell mesh for steel ropes (left) and Shell mesh for containers (right)
In terms contact interaction, General contact with friction (µ=0.15) is used in the example. General contact method is easier to define in Abaqus. Since there are many rods and other parts, the contact pair definition and surface selection would be time-consuming. So, General contact is more practical in current example.
When using a general contact including self-contact, it is necessary to reduce the contact thickness of shell and beam elements depending on the thickness and element size. Otherwise, the shell or beam structure will become impossible to fold or to find contact. Automatic thickness reduction is common in Abaqus, and solver writes the warning message into status file(.sta). However, one can avoid the thickness reduction by excluding the self-contact surfaces of shell or beam from general contact definition and by assigning a contact control (NOPERIMSELF) over Edit Keyword.
The excluded self-contact surfaces from the general contact would look like below in Keyword Editor,
and the contact control is,
*CONTACT CONTROLS ASSIGNMENT, CONTACT THICKNESS REDUCTION=NOPERIMSELF
One can also exclude the surfaces in Abaqus/CAE (Figure 10) itself,
Figure 9: General contact definition in Abaqus/CAE
Figure 10: Excluded surfaces from General Contact
Figure 11: Contact controls in Edit Keywords
Containers do not play a big role in current transport simulation evaluation. Hence, containers are modeled as rigid body and the reference point of the rigid body is constrained in all directions.
Figure 12: Rigid body definition for containers
Generally, connectors are used to model connector machine elements such as bolts, screws, joints, and weld points. Though, the appearance of connector is not very realistic as 3D-model, but the behavior is same as 3D-model. The main advantage of connector is modeling is simple and required less calculation time when compared to 3D-modeling.
If one willing to define a precise spot-welding failure, then must get characteristic values from physical test as a function of direction of load with different loading state and the combination of the loading type (Figure 13).
Figure 13: Failure forces for spot-weld points
Additionally, in Abaqus, you’re able to model weld points using weld connector section. However, weld type connector section will not provide options to define elastic or elastic-plastic properties. With weld section, one can just define the forces/moments as a failure criterion (Figure 14) without elastic property.
Figure 14: Welding connector section in Abaqus
To assign elastic-plastic properties, one must use other type of connector section (for example bushing) and along with failure criterion as forces/moments. The stiffness matrix components of the connector sections are formulated as follows:
If poison’s ratio is not considered:
A bushing connector section definition with elastic properties in Abaqus is shown as:
Figure 15: Bushing connector section in Abaqus
Once the connector section is created, then it must be assigned through a wire-feature or fasteners (Figure 18) to where the connector/joints must be modeled. In the current example, fasteners are created since they were easy to create multiple times without any reference points, and attachment points can be used in fasteners. Attachment points option under interaction module creates several weld points along the edge direction with the help of edge parameters (Figure 16). For each strap, three rows of weld points are created and each row as three weld point along the edge.
Figure 16: Attachment points
Figure 17: Fastener definition in Abaqus
Figure 18: Fastener definition in Abaqus
Figure 19: Fastener definition in Abaqus
Self-weight of the components is considered in the transport simulation. Hence, the gravity load is defined.
Figure 20: Gravity load definition
Following boundary conditions are applied to containers, wooden blocks, and steel ropes.
Containers are modeled as rigid body and reference point is fixed (degree of freedoms are constrained in all directions)
Figure 21: BC on Containers
Wooden blocks are generally placed on the ground surface and fixed rigidly, then bundles are placed on the blocks. Hence, the DOF of blocks are constrained in all directions.
Figure 22: BC on Wooden Blocks
Displacement boundary conditions to the edge of steel ropes applied in such a way that the bundles can be lifted or dropped (to place on wooden blocks or on bundles) vertically (Y-direction in global co-ordinate system).
Figure 23: BC on Ropes
Initially, the straps are rolled over the steel rods with gaps. Hence, to hold the rods tightly, the straps are tightened during the simulation and pre-tension effect has been brought. To bring the pre-tension effect for the straps, the straps are heated to [Equation] in the initial step and then cooled to [Equation]. Because of this process, the straps will be compressed and hold the rods tightly.
Figure 24: Predefined field (Initial temperature)
Figure 25: Predefined field
Further sections of the transport simulation such as assembly, step definition and results will be demonstrated in the second part of this blog.
Discover our library of free, detailed Abaqus tutorials