Use of 3D Parametric Models in the Automotive Component Design Process

The process of design, development and production of cars has been strongly influenced by the use of computer technology since the 1980s. The philosophy of CAD (Computer Aided Design) and CAM (Computer Aided Manufacturing) approaches has become an integral part of the automotive industry. These technologies have shortened the innovation cycle in car model lines to 6-8 years. In the middle of this cycle, the so-called facelift of the model line is employed, when there are certain shape changes of the exterior and interior of the car or the equipment is expanded with new or improved elements. CAx systems enable changes to be made in such a short period of time. This article deals with the design of a fully parametric CAD model of a car interior element. Specifically, it is part of the door pull handle. The advantages of connecting a fully parametric model to a spreadsheet were pointed out. This link has a significant impact on the speed and flexibility of change processes on product models. The model was created in the Part Design volume modeler in the CAD system CATIA V5 Release21, which is used mainly in the automotive and aerospace industries. The parameters of the model were linked to the MS Excel spreadsheet.


creatIng a 3d parametrIc model of the plastIc cover door pull handle
We discuss the importance of using the control parameters of the 3D model in the process of adjusting the shape and wall thickness of this handle cover (Fig. 2) manufactured as a plastic mold.
Before designing the cover, the parameters were defined. The length of the door pull handle can be modified by changing the value of the parameter representing the length dimension "Rear length", the total depth of the body by changing dimensions are defined in the Formula Editor improvement (Fig. 4).
The parameters defined in this way were assigned to specific values of parameterized distances in the profile sketch. The dimension values that   were only changeable in a particular Sketch become variables that can be changed at any time by changing a parameter value in the product tree without having to enter the Sketcher environment. In the following part, we will show how these Parameters can be linked to a spreadsheet and control the model using the values entered in the spreadsheet. By assigning the name of the parameter of the parameterized dimension, the so-called Relations, which are also shown in the product tree (Fig. 5).
In the Constraint Definition window (Fig. 6), the numerical value of the "dimensioned length" parameter of 200 mm is replaced by the predefined length parameter "Rear length" (Fig. 6). Selecting the f(x) icon edits the Formula Editor dialog box. In the top line of the Formula editor is the left side of the equation representing the CAD interpretation of the defined dimension, to which we assign the right side of the equation that will be represented by the length parameter "Rear Length" (Fig. 7).
Analogously, the "Outside length" and "Inside length" parameters were assigned to the numerically defined values of the sketch dimensions. The "Thickness" parameter assignment was defined in the Edit Parameter dialog box of the Shell command (Fig. 8). Subsequently, in the Formula editor, the CAD interpretation of the dimension was assigned the "Thickness" parameter, which represents the wall thickness of the molding (Fig. 9). Four controlled parameters described by formulas (1-4) determine the variable geometry of the plastic mold (Fig. 3).

model control by ms excel
At first we select Creation of a Design Table  command and Defining model control parameters which will be linking to MS Excel. The selected parameters have been defined in order to control the dimensions of the model geometry (Fig. 11).
This step redirects us to the MS Excel environment, where we have the option to add values to individual parameters. This creates a dimensional database for the model (Fig. 12). The dimension database can be modified at any time. The model can then be controlled in a spreadsheet by parameter values (Fig. 13). Two different shapes for setting different parameter values in MS Excel are shown in Figures 14 and 17.

derIvatIon of the shape of the cavIty and the mold Insert
Due to the associativity between the 3D parametric model and the derived negative and positive shape of the mold parts, the functionality of publishing the geometry of the model, the so-called Publications. In such a case, the import of the whole Part is not required for the model of the cavity and the insert, but only the so-called  (Fig. 15), which is a link to the original model. In this case, any change to the model will affect every other model where the Publications link appears. In Negative and Positive, the Publication is displayed as Solid.1. On the basis of the model, the shape of the cavity (Fig. 16 left) and the mold insert (Fig. 16 -middle) were derived by using Boolean Operations Remove and Remove Lump function.

stl data generatIon and productIon usIng 3d prIntIng technology
The geometric data from CATIA were exported to STL (Standard Triangle Language) format.
The STL of the model as loaded into the Z-Suite software (Fig. 18), where the material (ABS) was defined, the printing strategy was determined and the parameters influencing the print quality and time were set (Fig. 19). On the basis of these settings, a control code was generated for the Zortrax M200 3D printer.
The model was set up in the printing space to achieve the best possible quality of the surface of the printed model. Due to the fact that the model is hollow inside and has different reinforcing ribs, it was necessary to print the supporting structures of the model, which were physically removed after printing. The model was printed at a reduced size. Printing took 6 hours when the print layer height was set to 0.19 mm. The physical printout of the model is shown in Figure 20. conclusIon This paper demonstrates that a CAD model based on predefined parameters is flexibly   Fig. 18. STL format imported in the Z-Suite software changeable in real time. Model control can still be "automated" by connecting a CAD system to a spreadsheet. An important advantage is that the changes in shape are reflected not only in the shape of the part but also in all assemblies where the reference to the part in the form of so-called "Publication" occurs.
As a result of the work, we confirmed that the parameterization of the model makes sense especially in the first stages of finding the shape of the model, when it is necessary to perform a number of repetitive operations that are necessary to achieve the result. Such an approach saves time and resources invested in product development.

acknowledgments
This work was supported by VEGA 1/0110/18 "Research and development in the area of reverse engineering and rapid prototyping focused on innovations of constructional parts designed for the experimental vehicles and transport equipment".