CAM model parameterisation methodology and its further unification in Siemens NX environment

. The paper describes the methodology of mathematical CAD model parameterisation for the subsequent development of the control program (CP) in Siemens NX 2206, which allows in the process of changing the parametric CAD model to adapt not only the 3D model, but also to rebuild the control program, thereby significantly reducing the time for CP development. The application of methods of parametrisation of models in the article is shown in an example of simulators of blades of 3 stages. As a result, a parametric CAD model of the blade simulator, tooling for the product installation on the machine tool, for 3-axis CNC milling machining, automatically changing for each stage of the simulator were developed. A simulator manufacturing process based on the parametric model was developed and successfully implemented. The report formulated the basic provisions and rules for the design of single-type models for the subsequent development of universal control programmes for CNC machines.


Introduction
Many gas turbine engines (GTEs) are currently being designed, the most important element of which are blades. Steam and gas turbine blades tend to have a complex geometry, which makes them not only time-consuming to produce but also costly to produce. For this reason, during tests of engine prototypes (balancing, endurance tests, fatigue tests, etc.) simulators, rather than blades, are installed in the engine. Simulators are products made of the same material and have the same mass properties as the blade [1].
In some GTE designs, it happens that blades/simulators of several stages in one engine may be of the same type, in terms of geometry, i.e., have the same set of faces, ribs, surfaces, etc., but have different linear dimensions. In terms of production of this type of product, the manufacturing process for them will be the same, but changes in the elements of the necessary tooling and the required tools must be taken into account. At the same time for manufacturing of simulators on CNC machines it is necessary to design a set of mathematical models of these parts, and also to design models of tooling and to develop several one-type control programs (CP) [2].

Part family in NX
Like any modern CAD system, Siemens NX has various tools for model parameterisation. Parametric modelling (parameterisation) is modelling using the parameters of the model elements and the relationships between these parameters. Parametrisation allows to rebuild (by changing parameters or geometrical relationships) various products in a short time and to avoid fundamental errors in modelling. Parametric modelling differs significantly from conventional 2D or 3D drawing. The designer in case of parametric designing creates mathematical model of objects with parameters at which change of configuration of a detail, mutual movings of details in assembly and so forth takes place [3][4][5].
In Siemens NX this solution is called a family of parts. A family of parts is a collection of parts with similar shapes and dimensions that define it. Some types of blades, imitators, intermediate inserts, etc. also fall under this definition, for example a blade may have the same shape, but there are different dimensions, length of the working part, dimensions of the locking part, radii of the comet. This kind of model in NX is based on prepared templates and tables from which the possible dimensional values of the template are indicated. The main advantages of Siemens NX as a parametrization environment are [6].
The main advantage of NX can be called synchronous modelling technology. The functionality of the programme allows for direct manipulation of the geometry of solids. The meaning of this technical solution is based on the fact that it is possible to impose geometric and dimensional constraints on the body, leading to a transformation of the shape itself. This feature will not require changes to operations previously worked out in the construction tree [7].
-NX implements a large assembly design methodology, providing both top-down and bottom-up generation of the assembly model. This allows the creation of a model with any degree of nesting, which will consist of an unlimited number of components [8].
-One of the main criteria for choosing NX by many global companies is the presence of WAVE technology, which allows the associative linking of parts in a project and the management of these links [9].
-NX has a built-in CAM module for turning, milling, electrical discharge and additive machining, which works perfectly in conjunction with the CAD module and WAVE technology, allowing the design of a workpiece model in addition to the main part model, also to carry out the necessary additional geometrical constructions required to implement many CAM machining patterns [10].

Creating and using a part family
It is possible to create a pattern family based on a pattern pattern (template) by using NX's built-in spreadsheet to create a type table that describes the entire pattern family. The following terminology is used when creating a pattern family: -pattern template file: the part of NX in which the pattern geometry on which the entire family is based is created and described with parameters and attributes; -family table: the table of type dimensions and other parameters that is stored in the part of NX that serves as the template (pattern); -family members: the part of NX with "Read Only" access, which stores the description of one of the parts in the family, made from the pattern and one string of parameter values taken from the template table; -family of parts: the part family [11].
In order to create a part family, a number of sequential steps must be followed: -create a pattern part in which to define the parameters that will be used to create the family members [12].
The definition of the parameters in the sketch is given by both constraints (tangency, perpendicularity, parallelism, etc.) and linear constraints, each linear and angular dimension is assigned a cell with an identification number, in NX this looks like <p#> where p is the prefix, # is the size number of Fig. 1.
In addition to the constraints in the pattern sketch, it is also necessary to parameterise the solid modelling tools (drawing, rotation, hole, etc.) Fig. 2. In contrast to the sketch, the parameters for e.g., drawing are set implicitly; for this purpose, in the drawing dimension setting field, you must find the "function" item, where the number of the drawn dimension will be displayed. Elements such as "chamfer", "edge rounding" must be parameterised in the same way [13].   An example of a table is shown in Fig. 4, it is possible to create a table with the required product parameters: parameters are specified in columns, family members in rows. The parameters can be expressions or various Boolean operations, also material data, presence/absence of items, etc. It is also possible to import Excel table [14].
To further design the NC in the CAM module, a workpiece model has to be built. As described above, synchronous simulation technology is implemented in NX. To create a workpiece, it is necessary to make an associative copy of the model-template, further geometric transformations will be performed in it without affecting the geometry of the parent model, and the associative copy will inherit all changes of the parent. Figure 6. Next, 2 planes parallel to the sketch plane of the template model should be created at the required distance. After that, using the tool of synchronous modeling "to replace the face, we should draw the previously formed faces of the part, on the face, lying in the previously created planes, Fig. 5 [15]. Thus, a workpiece model was obtained that is fully associative with the template model. Parameterisation of the milling operation. To further design the part, a new assembly file must be created in which the template model file must be added. Also, if there is a tooling model, it can also be loaded as a component in the machining file Fig. 6 [16]. Then an associative copy of the part and workpiece from the pattern part file should be created in the assembly file using the WAVE technology supported in NX. By its structure, WAVE elements will be children in relation to the pattern file and when changes are made to the parent model, the child copies will also be associatively changed. Thus, it will be possible to make any changes (for NC design) in associative copies of the part, without influence on the part itself. Also, if there are tooling models, it also needs to be loaded as a WAVE copy, for zero point linking or reference geometry setting Fig. 7 [17]. Next, the part and workpiece geometries must be defined in the machining module, as well as the location of the DSCs. It is best to specify only the workpiece geometry and the part geometry directly in each operation, as for some operations it is better to use additional geometry as the part, to optimise the toolpath, due to the limitations of the templates in Figure  8. In order for the NC to be unified, for each family member, i.e., not to require any additional actions, after activating a new family member, it is necessary to meet the requirements of the design of operations: -The machining elements (part, workpiece) must be children, in relation to the pattern part file and be fully associative with it.
-The parts must have the same set of faces, edges and points, and calling the pattern family members must transform the existing set of geometric elements, rather than generating new elements.
-Uniform geometric constraints in the model and family members.
-All additional constructions, in the form of planes, sketches, additional solid elements, must be fully referenced to the associative copy of the machined part and when converting the model, these referencies must be preserved better to implement them with synchronous modelling.
-In milling operations templates, mode parameters, machining strategy, must be fully referenced to the part or to the complementary geometry, parameters such as cutting levels, must be referenced to the existing faces of the part.
-A nomenclature for the tools to be used, suitable for the machining of the whole family size, should be developed in advance. This will ensure constant cutting modes and tool paths, constant cutting depths and widths of cut on each family member.

Adaptive milling operation
To avoid tool collisions with machined workpiece surfaces, create an additional geometry that replicates the workpiece geometry, with offset faces, and select it as the Adaptive Template part, so the toolpath will eliminate undercuts on the workpiece surfaces. The depth and width of cut must be set with respect to the modes for the cutting tool and workpiece material. Fig. 9-10. The cutting levels are set from the top face of the workpiece, to the bottom face [18].  Level contour milling is a finishing operation for the machining of flat surfaces using a level cutting template. It is recommended for the machining of inclined surfaces. Since the surface to be machined is above the vice, it is not necessary to set the reference geometry. Either the original part or an associative copy with simplified geometry must be specified as the part to optimize the toolpath. Next, select cutting areas The depth of cut should be set in relation to the cutting tool and workpiece material (Fig. 11). Figure 12 show the visualized result of machining 3 representatives of a family of parts in NX. As can be seen from the figures, there are no undercuts and unprocessed surfaces on all surfaces of the simulators, as all trajectories were built based on the geometry of the family members, and adapted according to changes in the parameters of the part surfaces. These NC data were also tested directly on the machine. The resulting products were checked using an optical scanner. A comparison of the deviations between the data obtained and the mathematical model data is shown in Figure 13. The reports show that the deviations do not exceed the maximum deviation range; the blue areas are the result of an error in the machine zero-point reference and the cutting tool length reference.

Basic requirements for the development of a unified NC
 The machining elements (part, workpiece) must be child of the pattern part file and be fully associative with it.  Parts must have the same set of faces, edges and points, and the calling of the pattern family members must transform the existing set of geometrical elements, and not generate new elements.  Uniform geometric constraints in the model and family members.  All additional constructions must be fully referenced to the associative copy of the machined part and these referencing must be preserved when the model is transformed.
 In milling operation templates, mode parameters, machining strategy, must be fully referenced to the part or to elements of additional geometry.  The nomenclature of tools to be used, suitable for the machining of the entire family size, should be worked out in advance.

Conclusions
A methodology for part parameterisation in NX has been developed during the research, with further adaptation of the control program, to change the members of the part family. The basic principles of building 3D model, constructing additional geometry, and developing NC were formulated.
-The parameterisation technique allows to reduce time for development of 3D model and construction of additional geometry of a product, which is a multiple of the number of parts in the family.
-Reduced modelling errors -Designing one NC for all members of a family -Unification of the technological process for the entire product range