[Abstract:] Virtual prototyping technology is introduced into the design of drain pipe cleaning robot to evaluate the performances before the physical prototype is made. Taking the straight bevel gear as an example, the parameterized design based on Pro/E is discussed in detail. [Keywords:] Virtual Prototyping, Pro/Engineer, Drain Pipe Cleaning, Robot With the rapid development of the national economy, environmental pollution is becoming increasingly serious, and environmental protection issues are receiving increasing attention from all sectors of society. Urban sewage discharge is an important part of ensuring environmental sanitation and building modern civilized cities. Currently, the dredging of drainage pipes in most Chinese cities is still largely done manually, which is not only physically demanding and inefficient, but also exposes workers to harsh underground environments that are prone to explosions and other accidents. Literature review shows that pipeline robots, both domestically and internationally, are mostly used for inspection and repair of nuclear reactor pipelines and oil and gas pipelines, while research on drainage pipe dredging robots is still lacking. In light of this situation, we conducted research on a drainage pipe dredging robot and designed a virtual prototype on the Pro/Engineer platform. I. Design Scheme of Drainage Pipeline Dredging Robot The drainage pipe dredging robot adopts a four-wheel structure. The wheels are made of wear-resistant and corrosion-resistant synthetic rubber with treads to increase friction. The shape of the wheel contact point with the pipe wall perfectly matches the arc of the pipe wall to achieve as little gap contact as possible. The front of the vehicle is equipped with cutting tools to remove branches, calcifications, and other deposits from the pipe. The removed deposits are carried downstream to the inspection well by the water flow. II. Virtual Prototype Design of Pipeline Dredging Robot Virtual prototyping is an emerging technology in the field of design and manufacturing. This technology integrates product information into a computer-provided visual virtual environment using CAD/CAM/CAE technologies, enabling product simulation, analysis, and optimization before actual manufacturing. 2.1 System Structure of the Virtual Prototype for the Pipeline Dredging Robot The virtual prototype of the pipeline dredging robot combines pipeline dredging robot research with virtual prototyping technology. It studies and develops systems for kinematic and dynamic analysis, trajectory and path planning, and the interaction between the robot and its working environment in the robot design and manufacturing process. Through system simulation software, the system's motion is realistically simulated in a corresponding virtual environment. Design flaws can be easily modified on the computer, different design schemes can be simulated, and the system can be continuously improved until the optimal design scheme is obtained before a physical prototype is manufactured. 2.2 Design of Virtual Prototype for Pipeline Dredging Robot Using Pro/Engine The main function of Pro/Engineer is to perform parametric part modeling design. The functions it provides include solid modeling design, surface design, engineering drawing creation, part assembly, simple finite element analysis, mold design, circuit design, assembly part design, processing and manufacturing, reverse engineering, etc. This article takes bevel gear as an example to introduce the parametric design process of Pro/E in detail. The design steps are as follows. 1. Create a new part file (1) Create a new part file: “bevelgear”. (2) Uncheck the “Use default template” checkbox and select “mmns-part-solid”. 2. Set gear parameters and relationships (1) Open the 【Parameters】 dialog box and add gear parameters as shown in the table below. Name Type Value Description M Real number 3 Module Z Real number 25 Number of teeth of this gear ZASM Real number 45 Number of teeth of the gear meshing with it ALPHA Real number 20 Pressure angle B Real number 20 Tooth width HAX Real number 1 Tooth addendum coefficient CX Real number 0.25 Clearance coefficient HA Real number 0 Tooth addendum HF Real number 0 Tooth root height H Real number 0 Tooth total height DELTA Real number 0 Pitch cone angle DELTA-A Real number 0 Top cone angle DELTA-B Real number 0 Base cone angle DELTA-F Real number 0 Root cone angle D Real number 0 Pitch circle diameter DB Real number 0 Base circle diameter DA Real number 0 Tooth addendum circle diameter DF Real number 0 Tooth root circle diameter HB Real number 0 Tooth base height RX Real number 0 Cone distance THETA-A Real number 0 Tooth tip angle THETA-B Real number 0 Tooth base angle THETA-F Real number 0 Tooth root angle BA Real number 0 Tooth tip width BB Real number 0 Tooth base width BF Real number 0 Tooth root width X Real number 0 Displacement correction coefficient (2) Open the 【Relation】 dialog box and add the relational formulas for spur bevel gears as shown below. Through these relational formulas, determine the values ​​of unknown parameters based on known parameters. HA=（HAX+X） HF=（HAX+CX-X）H=（2*HAX+CX）*M DELTA=ATAN（Z/Z_ASM）D=m*Z DB=D＊COS（ALPHA）DA=D+2＊HA＊COS（DELTA）DF=D-2＊HF＊COS（DELTA）HB=（D-DB）/（2＊COS (DELTA))RX=D/(2*SIN (DELTA)THETA_A=ATAN (HA/RX)THETA_B=ATAN (HB/RX)THETA_F= ATAN（HB/RX）DELTA_A=DELTA+THETA_ADELTA_B=DELTA+THETA_BDELTA_F= DELTA+THETA_FBA=B/COS(THETA_A)BB=B/COS(THETA_B)BF=B/COS(THETA_F) (3) Select the 【Edit】-【Regenerate】 option in the main menu to calculate the values ​​of each unknown parameter in the 【Parameter】 dialog box. 3. Create a bevel geometry curve (1) Translate the datum plane TOP to the right by 67.5 to create the datum plane DTM1. (2) Click and select the translation distance between the datum plane DTM1 and the TOP plane in the work area, add it to the 【Relation】 dialog box, and enter the relation: "＝D/(2＊TAN(DELTA))". (3) Create the datum axis A-1 through the intersection of the datum planes FRONT and RIGHT. (4) Create the datum point PNT0 through the intersection of the datum axis A-1 and the datum plane DTM1. (5) Click the [Sketch Reference Curve] icon in the right toolbox to open the [Sketch Reference Curve] dialog box. Select FRONT as the sketch plane and enter sketch mode. (6) Add parameter d2 to the [Relation] dialog box and then enter the relation "=90". Continue to add other parameters in the drawing using the same method. 4. Create the basic circle of the large end gear (1) Create the reference plane DTM2. Select the FRONT reference plane and curve 1 as references to create the reference plane. (2) Create the reference point PNT1. Create the reference point PNT1 that passes through the intersection of curve 1 and curve 2. (3) Click the [Sketch Reference Curve] icon in the right toolbox, select the reference plane DTM2 as the sketch plane, and enter the two-dimensional sketch mode. (4) Draw four concentric circles of arbitrary size in the sketch plane and draw a vertical line through the center of the circle. (5) Add the diameter parameter of the basic circle to the [Relation] dialog box and add the relation as shown below: D154=d/cos(delta) d155=da/cos(delta) d156=db/cos(delta) d157=df/cos(delta) Where, d154, d155, d156, and d157 represent the pitch circle, addendum circle, base circle, and root circle diameters, respectively. (6) Select the 【Edit】-【Regenerate】 option in the main menu to regenerate the gear basic circle dimensions and finally generate the gear basic circle. 5. Create the small end gear basic circle (1) Create the reference point PNT2 passing through the intersection of curve 2 and curve 3. (2) Click the 【Sketch Reference Curve】 icon in the right toolbox and select the DTM3 surface as the sketch plane. Then draw a concentric circle of arbitrary size and a vertical line passing through the center of the circle in the sketch plane. (3) Add the diameter parameters of each basic circle to the relation dialog box and add the relation as shown below: D158=(D-2*B*SIN(DELTA)/COS(DELTA)) D159 = (DA-2*BA*SIN(DELTA-A)/COS(DELTA)) D160 = (DB-2*BB*SIN(DELTA-B)/COS(DELTA)) D161 = (DF-2*BF*SIN(DELTA)/COS(DELTA)) (4) Select the [Edit] - [Regenerate] option in the main menu to regenerate the basic circle size of the gear, and finally generate the basic circle of the standard gear. 6. Create the involute of the large end gear (1) Create the coordinate system CS0. Click the [Sketch Reference Curve] button in the right toolbox to open the coordinate system dialog box, and select the reference point PNT1 as the reference for the placement of the coordinate system. In the [Coordinate System] dialog box, open the [Orientation] tab, select curve 4 as the positive direction of the Y-axis, select curve 5 as the positive direction of the X-axis, and generate the coordinate system CS0. (2) Create the coordinate system CS1. Open the 【Coordinate System】 dialog box again, select coordinate system CS0 as the placement reference for the new coordinate system, select 【Cartesian coordinate system】 in 【Offset type】, and finally generate coordinate system CS1. (3) Add the offset angle parameters of coordinate system CS0 and CS1 to the 【Relationship】 dialog box, and then enter the relation: "＝360＊COS(DELTA)/(4＊Z)+180＊TAN(ALPHA)/OI-ALPHA". (4) Open the Notepad editor and add the following involute equation: R=d156/2 theta=t＊60 x=r＊cos(theta)+r＊sin(theta)＊theta＊pi/180 y=r＊sin(theta)-r＊cos(theta)＊theta＊pi/180 z=0 After completion, select 【File】-【Save】 to save the settings, and finally create the gear involute. 7. Create the small end gear involute (1) Create coordinate system CS2. Select PNT2 as the reference for placing the coordinate system, select curve 6 as the positive direction of the Y-axis, select curve 7 as the positive direction of the X-axis, and finally create coordinate system CS2. (2) Create coordinate system CS3. Select CS2 as the reference for placing the coordinate system, and finally generate coordinate system CS3. (3) Select the offset angle parameter between coordinate system CS3 and CS2, and add it to the 【Relation】 dialog box, and then enter the relation: "＝360＊COS(DELTA)/94＊Z)+180＊TAN(ALPHA)/PI-ALPHA". (4) Open the 【Curve: From Equation】 dialog box, select coordinate system CS3 and the 【Cartesian】 option. Add the following relation in the opened Notepad: R=d160/2 theta=t＊60 x=r＊cos(theta)+r＊sin(theta)＊theta＊pi/180 y=r＊sin(theta)-r＊cos(theta)＊theta＊pi/180 z=0 After completion, select 【File】-【Save】 to save the settings. Finally, generate the involute. 8. Mirror the involute (1) Create a reference point PNT3 that passes through the intersection of curve 8 and curve 9. (2) Create a reference axis A-2 that passes through reference point PNT1 and is perpendicular to the reference plane DTM2. (3) Create a reference plane DTM4 that passes through the reference axis A-2 and reference point PNT3. (4) Create a reference plane DTM5 that is offset from DTM4 by an angle of -3 and passes through A-2. (5) Add the angle parameter between reference planes DTM4 and DTM5 to the 【Relation】 dialog box, and then enter the relation: "=360*COS(DELTA)/(4*Z)". (6) Select DTM5 as the mirror plane to mirror the large end involute of the gear. (7) Mirror the small end involute using the same method. 9. Create the first gear tooth (1) In the main menu, select [Insert] - [Sweep Blend] - [Extend] to open the [Menu Manager]. In the [Blend Options] menu, select [Sketch Section], [Perpendicular to Original Trajectory], and [Finish]. In the [Sweep Trajectory] menu, select [Sketch Trajectory]. Select the reference plane FRONT as the sketch plane, and then place the sketch plane using the default parameters. (2) In the right toolbox, click the [Use Edge] button to open the [Type] dialog box. Select the [Single] radio button and use the trim button in conjunction with the drawing tools to draw the sweep trajectory line. (3) According to the system prompt, enter the z-axis rotation angle: "0" in the message input window. (4) In the right toolbox, click the [Use Edge] button to open the [Type] dialog box. Select the [Single] radio button and use the trim and fillet buttons in conjunction with the drawing tools to draw the large end tooth profile of the gear. (Note that equal radius constraints should be added at the two fillets). (5) According to the system prompt, enter the z-axis rotation angle: "0" in the message input window. (6) Use a similar method to draw the small end tooth profile, and finally generate the gear tooth structure. (7) Open the relation dialog box and add the following relation in the dialog box: If hax<1 d207=0.31*m d217=0.31*m endif if hax>=1 d207=0.2*m d217=0.2*m endif Where, d207 and d217 are the chamfers of the tooth profile curves of the large and small ends of the gear. 10. Copy and array gear teeth (1) Use the rotation copy method to copy the gear teeth created in the previous step, with a rotation angle of "360/z", and finally generate the second gear tooth. (2) Use the array method to array the gear teeth, with a total array feature count of 24. (3) Add the rotation angle parameter when rotating and copying the gear teeth to the [Relation] dialog box, and then enter the relation: "＝360/z". (4) Add the distance parameter from the first tooth to the third tooth to the [Relation] dialog box, and then enter the relation: "＝z-1". 11. Create a cone (1) Click the [Rotate] button in the right toolbox to open the design icon panel. Select the reference plane FRONT as the sketch plane, accept the system default parameters to place the sketch plane, and enter the two-dimensional sketch mode. (2) Use basic drawing tools to draw the two-dimensional shape of the cone. Finally, generate the bevel tooth structure. (3) Add the bevel tooth large end length parameter to the [Relation] dialog box, and then enter the relation: "=0.8*h". 12. Add decorative structure 13. Change gear parameters In the main menu, select the [Tools] - [Parameters] option to open the [Parameters] dialog box. Modify the number of teeth to 39, the module to 2.5, and the tooth width to 15. After modification, select the [Edit] - [Regenerate] option in the main menu to regenerate the model according to the modified parameters. Finally, generate the model as shown in Figure 2.