Introduction to 3Dmodelling Using Siemens NX 8.5

Introduction to 3DModelling Using Siemens NX 8.5

Michael Wang

ECE 480 - Design Team 5

3/28/2014

Abstract

Design team five is developing a 3D tactile display, capable of displaying images by raising an array of pins to varying heights. It will be able to receive image files, analyze and process the image in terms of color intensity, and then individually raise each pin in the array to the corresponding height. This technology will be extremely beneficial to blind students, who sometimes are at a disadvantage when taking courses such as calculus and physics, allowing them to more effectively grasp certain concepts (3D curves, waveforms, etc.). The device will also have a multitude of other practical applications, including basic images and maps. There are four main components of the device: the display, the XY table, the pin setter, and the software. The display is to be constructed using 3D printing technology, which requires the use of 3D CAD software. This allows for flexible and inexpensive prototyping and manufacturing. It is important for nearly all designers to understand the fundamental concepts and mechanics behind 3D modelling.

Keywords: Computer-aided Design, CAD, Siemens NX 8.5, 3D Printing, Constructive Solid Geometry, CSG, Modelling, Tactile Display, Braille,

Introduction

Computer-aided Design (CAD) refers to the use of computer programs to assist in both the process of designing and the actual design of physical models. It came be used to design curves, surfaces, solids in both two and three dimensions, as well as improving documentation and creating catalogs for manufacturing. The commercial CAD industry began in the late 1960’s, with a handful of companies developing proprietary mainframe computers and vector refresh graphics terminals (Weisberg). Modern day CAD modelling has evolved from 3D wireframe modelling (whereby each line of the model is manually inserted) to 3D solid parametric and explicit modelling (whereby features are added relative to existing features, such that relationships between model geometries are maintained – allowing designers to easily make changes to the part while retaining desired design attributes).

For this project, the principles of 3D solid parametric modelling were utilized in the design of the pin display matrix in Siemens NX 8.5. More specifically, the technique of Constructive Solid Geometry (CSG) was used to develop the final display matrix (shown in Figure 1). CSG combines the concept of simple Boolean operators (union, difference, and intersection) with simple geometric shapes (squares, spheres, cylinders, etc.) in order to model the desired part (Leadwerks). CSG is the most fundamental design paradigm of modern 3D modelling, as it is relatively easy to pick up, and calls for a less abstract design process when compared to more advanced methods, such as curve modelling and polygonal modelling. Seeing as this project does not require extremely complex models (human faces, curved surfaces, etc.), CSG was chosen as the design method of choice.

Figure 1. 3D Model of Pin Display Matrix

Objectives

The 3D model is a 16 x 16 pin array with individual 3D printed slabs, forming 16 rows of 16 pins. Each of these rows has individual slots for metal pins to prevent them from becoming misaligned. These plates are stacked together, and can be “locked” using two bolt screws on each side. The initial position of the sheets allow the pins to move easily while providing enough friction to remain at the desired height. After each pin is raised to its proper height, the bolt screws are tightened, locking the pins and ensuring that the heights will not change when the display is being felt.

Technical Details

The pin display matrix design for this project is a 16 x 16 hole assembly. It consists of a series of thin plates with semi-circle grooves linearly arranged; these grooves are designed such that the pins will be held static. The two outside plates are made significantly thicker, in order to minimize flex throughout the middle of the plates (therefore distributing tension on each pin more evenly), as well as to improve the durability of the entire assembly. The plates are held together via the larger diameter holes in the two side “ears” of each plate. A bolt is threaded through these ears, and springs are placed in between each plate around the bolt during the assembly process. The springs are used to further distribute tension evenly between plates, ensuring that each pin will require the same amount of force to move. There is also a small circular indented area around each ear hole, so that the springs located in this area are allowed slightly more space. A nut will be threaded onto the open end of the bolt to compress the plate assembly.

In addition to holding the plates together, the bolt and nut also function as a method to “lock” the pins in place. While it is necessary for the pins to be static without any externally applied force, when the display is still being refreshed, it is desirable for the pins to be able to move when the Z-axis actuator is repositioning the pins. Therefore, the display will have two modes: unlocked and locked. The display will be unlocked while the display is refreshing, such that pins will be moved when the Z-axis actuator presses on them, but the pins will still have enough friction to remain in the position they are set to. While the display is locked, the pins will not be able to be repositioned when subjected to forces of the magnitude capable of being achieved by the Z-axis actuator, as well as human fingers. The locked mode will be used after the display has been refreshed, allowing users to feel the display without the fear of repositioning any of the pins. The locked mode will be achieved by tightening the nuts to the point where the pins are no longer movable when reasonable forces are applied to them.

Implementation

Siemens NX 8.5 was used to create the 3D model in Figure 1. The model is comprised of a combination of extruded rectangles, holes, and edge blends. While an exhaustive tutorial on each step taken in the development of this model would be unnecessarily long and repetitive, a break-down of each major design step will be given as follows.

Step 1 - Datum Coordinate System

For 3D modelling, the datum coordinate system (DCS) is analogous the compass of a map. It is the fundamental positioning tool for the entire model. Since the desired part is to be 3D printed, the initial DCS is of less importance than if the part was designed to be machined (which involves intricacies beyond the scope of this application note). For 3D printing, the most important thing to remember is that the printer prints in layers, so operating costs can be reduced if the part is designed to minimize Z-axis height. The standard top-view DCS is shown in Figure 2. Additional DCS points will need to be added throughout the design of this part, and this will be discussed when necessary.

Figure 2. Datum Coordinate System

Step 2 – Basic Sketching

3D modelling starts off as 2D modelling. Sketches are 2D drawings that can be given depth (extruding). There are a variety of sketching tools available to create different shapes. Create the base rectangle of the part by using the Rectangle tool, found in the toolbar located at the bottom of the NX window (Figure 3). The rectangle dimensions were calculated beforehand. For the Y axis, since each hole is 2.6mm center-to-center, 2.6mm * 16 holes = 41.6mm; an extra 0.5mm was added for the top and bottom edges of each plate, such that the top and bottom holes for each plate are not on the very edges. This results in a Y axis measurement of 42.6mm. The X-axis was calculated by adding 5mm to each side of the Y-axis calculation: 42.6mm + 5*2mm = 52.6mm. 5mm was chosen as a reasonable thickness to add to the end plates. Thus, a 52.6mm by 42.6mm rectangle was created as the basic shape of the part (Figure 4).

Add two additional sketches to the initial sketch. One is a point (indicated by the “+” in Figure 3), to be copied into the 16 x 16 array of holes. The other is another rectangle, with width centered at the aforementioned point. This rectangle will be the basis for the channels that run between the plates. See Figure 5 for details.

Figure 3. Toolbar: Rectangle

Figure 4. Basic Rectangle Sketch

Figure 5. Additional Point and Rectangle Sketches

Step 3 – Instance Geometry

The Instance Geometry command is a very powerful tool. It can be used to copy existing features of a part/sketch according to user specified parameters (distance between copies and number of copies, as well as where to place copies). The first step is to choose the type (along a path, vector, mirrored, or rotated). For this part, instance geometry objects will always be translated. Next, select the object that should be copied (in this case it is the point created in the latter portion of Step 2). The direction should also be specified at this point (for this it is the X-axis – select the X-axis vector that appears on the new DCS that appears). Since each hole should be 2.6mm C-C, set distance as 2.6mm and the number of copies as 15 (for a total of 16 points). This should result in a sketch identical to Figure 7.

Do another Instance Geometry command in order to copy the 16 points 16 times, this time in the Y-axis direction. This should result in an array of 16 x 16 points. These points will eventually be turned into the holes for pins in the display. Finally, invoke yet another Instance Geometry command, this time using the thin rectangle also created in the latter portion of Step 2, in the X-axis direction. The final result is shown in Figure 8.

Figure 6. Instance Geometry Dialog Box

Figure 7. Sketch after First Instance Geometry of Point

Figure 8. Final Sketch after Instance Geometry Commands

Step 4 – Extruding

Invoke the Extrude (X) command. It can be found in a toolbar near the top of the NX window. A dialog box will appear (Figure 9). Select the initial rectangle sketch as the Section, and the Direction vector as the Z-axis. This will extend the sketch upwards in the Z direction, creating a rectangular box. Since the part should be approximately one inch tall, make the end distance 25mm.

Sketch and extrude two additional rectangles on the sides of this first rectangle. Make sure to change the Boolean operator to “Union,” to ensure that NX recognizes these two “ears” as attached to the initial rectangle (otherwise, it is possible that the ears will be 3D printed detached from the main box). This will result in the part shown in Figure 11.

Figure 9. Extrude Dialog Box

Figure 10. Part after Extruding Initial Rectangle

Figure 11. Part after Extruding “Ears”

Step 5 – Holes

Invoke the Hole command. It is located in the same toolbar as the Extrude command. The Hole dialog box should appear (Figure 12). While specifying points, NX should automatically select all 256 points after manually selecting a few of the previously sketched points. Make the diameter of each hole 1.6mm (the diameter of each pin), and change the Boolean operator to Subtract. The Subtract operator will remove the material that intersects with the selected body. Select the large initial rectangle as the body. This will subtract material from the initial rectangle. While the dialog box is still open, the part should refresh to display the desired changes (Figure 13).

Figure 12. Hole Dialog Box

Figure 13. View of Part with Hole Dialog Box Open

Step 6 – Finishing Up

Using a combination of the previously covered commands, the rest of the part is easily generated. The Show and Hide command may also be necessary to access the interior of the part, to create the ear hole indentations for increased spring space. The Show and Hide command can be accessed by navigating the Edit menu (Edit -> Show and Hide). Hiding certain plates will allow an easier to access view of interior plates (Figure 14).

Figure 14. View of Indented Ear Holes on Interior Plates

Results and Recommendations

As can be seen in Figure 15, the 3D model generated using Siemens NX 8.5 was properly printed. While the 1.6mm diameter holes in the assembly exhibit the proper amount of force upon unmodified pins, the eventual goal of the project is to use tumbled pins (which results in less sharp edges and therefore a more pleasant experience for the end user). These tumbled pins are marginally smaller in diameter than the un-tumbled pins, but the difference is enough to result in inadequate friction to maintain the desired pin heights. This will be fixed in the final design by decreasing the diameter of the holes in the display assembly. Furthermore, since the springs located between each plate are only approximately the same length, there are sometimes inconsistencies with the tension applied upon the pins throughout the entire display. The springs must be trimmed because there do not currently exist commercially available springs that are as short as necessary to fit in between the plates (there is a clearance of 0.4mm without taking the indented area into account – this value increases to 1.4mm otherwise). A more precise method of trimming the springs must be developed for the final design. Overall, the design of the 3D display is a success, and only minor revisions need to be made before bringing the conceptual design into the final stages of this project.

Figure 15. 3D Printed Part

References

Leadwerks. 2006. What is Constructive Solid Geometry?

Weisberg, David. 2008. The Engineering Design Revolution.