Development of the Transmission Tower Virtual 3D Model for Structural Analysis in ANSYS

Making a 3D model is a complex process of transformation of real structure into virtual model with necessary idealization. The starting points are geometry, supports, loads, expected displacements and deformations [1-3]. The starting point for structural and modal analysis is adequate virtual 3D model. Scientific paper [4] presents methods for 3D modelling of a machine in Solid Works Motion. It provides a good model for conducting static and dynamic analysis of desired machine at the very beginning of development process. Those virtual analyses will show the potential behaviour of machine parts during exploitation [5-8]. Electric power transmission tower is a lattice steel structure. It is built out of, by size different, but standard shape `L` and `U` profiles. The first step in virtual model building is to form a matrix of key points. Key points are all spots of importance, like starting and ending point of every line, points of support, points where the load is applied, or points where two steel parts are bolted. The difficulty is that all key points must have distinguished address. It is formed by point coordinates in the Cartesian coordinate system. When all key points are defined, it is important to link them with lines. Every line presents one `U` or `L` profile on the real structure. When a line model is formed, an adequate cross section should be assigned to every line. That is how a virtual part is formed. Every virtual part must have material properties assigned (density, Young's modulus, Poisson's ratio...) [9]. After those steps, a virtual model is ready for pre-processing. The tower consists of four main ‘L’ profiles, which start from the base plane, from the square vertices, and join, in a single point at the top of the tower. Between those main ‘L’ profiles, a side braces are bolted.


INTRODUCTION
Making a 3D model is a complex process of transformation of real structure into virtual model with necessary idealization.The starting points are geometry, supports, loads, expected displacements and deformations [1][2][3].The starting point for structural and modal analysis is adequate virtual 3D model.Scientific paper [4] presents methods for 3D modelling of a machine in Solid Works Motion.It provides a good model for conducting static and dynamic analysis of desired machine at the very beginning of development process.Those virtual analyses will show the potential behaviour of machine parts during exploitation [5][6][7][8].Electric power transmission tower is a lattice steel structure.It is built out of, by size different, but standard shape `L` and `U` profiles.The first step in virtual model building is to form a matrix of key points.Key points are all spots of importance, like starting and ending point of every line, points of support, points where the load is applied, or points where two steel parts are bolted.The difficulty is that all key points must have distinguished address.It is formed by point coordinates in the Cartesian coordinate system.When all key points are defined, it is important to link them with lines.Every line presents one `U` or `L` profile on the real structure.When a line model is formed, an adequate cross section should be assigned to every line.That is how a virtual part is formed.Every virtual part must have material properties assigned (density, Young's modulus, Poisson's ratio...) [9].After those steps, a virtual model is ready for pre-processing.The tower consists of four main 'L' profiles, which start from the base plane, from the square vertices, and join, in a single point at the top of the tower.Between those main 'L' profiles, a side braces are bolted.

KEYPOINTS DEFINITION
In order to form a correct key point matrix, it is necessary first to numerate all points.It has to be done, because, later, every line will be formed out of two key points (starting and ending keypoint), and every line that is formed will have its own number.In order to avoid confusion (more than three hundred and fifty points were made), and to be capable to meaningfully read analysis results, it is of extreme importance to do this numeration very carefully.
It would be very hard to manually insert three coordinate values for every of 350 key points.That is why a small computer program was written, to automatically generate all needed key points.Idea was to use the theory of triangle similarity for generating key points.
Eight base key points were defined manually.The base key points were defined through following command: The letter `K` in at the beginning of the command line orders key point generation.The first number shows the key point address, and following three values represent key point coordinates in the Cartesian coordinate system.Graphically, the result is shown in Figure 2. The following code was used to generate the keypoints on the four main 'L' profiles.It is a kind of 'FOR' loop, where the counter 'j' goes from 1 to 41.The letter 'K' defines key point generation.Then, there is a short code for key point address generation (J*BR+1).Then, three short codes that follow make the desired key point coordinates.

Figure 3. Key points of four main 'L' profiles
In the same manner, all other key points were defined.Final key point matrix is shown in Figure 4.

Figure 4. Key points of four main 'L' profiles
Between those key points, both main lines and side braces were generated.

ASSIGNMENT OF CROSS-SECTION
In this process, a BEAM188 element was used.The BEAM188 element is suitable for analysing slender to moderately stubby/thick beam structures.This element is based on the Timoshenko beam theory.Shear deformation effects are included.
BEAM188 is a linear (2-node) beam element in 3-D with six degrees of freedom at each node.The degrees of freedom at each node include translations in x, y, and z directions, and rotations about the x, y, and z directions.Warping of cross sections is assumed to be unrestrained.
The beam elements are well-suited for linear, large rotation, and/or large strain nonlinear applications.
BEAM188 includes stress stiffness terms, by default, in any analysis.The provided stress stiffness terms enable the elements to analyse flexural, lateral and torsional stability problems (using eigenvalue buckling or collapse studies with arc length methods).
BEAM188 can be used with any cross section defined.Elasticity and isotropic hardening plasticity models are supported for calculations (irrespective of cross section subtype) [10].
With the following commands, used standard `L` profiles were configured in ANSYS: SECT,40,BEAM,L SECD,0.040,0.040,0.004,0.004`SECT 40` is a code name for that kind of profile.It is of `L` shape (predefined in Ansys) and its dimensions are 40mm x 40mm, with wall thickness of 4mm.Similar code was written for the `U` shape cross section.
After completion of the cross section assignment, a final result of a defined 3D model is shown in Figure 5.

Figure 1 .
Figure 1.Real transmission tower structure