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ME-430 INTRODUCTION TO COMPUTER AIDED DESIGN Automated Design of Involute Gear – using Surface Features Pro/ENGINEER Wildfire 2.0 Dr Herli Surjanhata Create a both sides solid protrusion for base feature of involute gear as shown below: Create gear parameters by From Tools pull down menu, select Parameters and enter the following: Parameter Diametral_pitch Type Integer Value Continue to create the following parameters: Parameter no_gear_teeth AGMA_quality tooth_form root_fillet_radius pressure_angle Type Integer Integer String Real Number Real Number Value 39 10 20 DEG INV – AGMA Full-Depth 0.0375 20.0 Create relations for the gear parameters From Tools pull down menu, select Relations Enter the following: pitch_dia_gear = no_gear_teeth/diametral_pitch Continue to enter the following relations addendum = dedendum = outside_dia_gear = root_dia_gear = whole_depth = circular_pitch = tooth_thickness = 1/diametral_pitch 1.25/diametral_pitch pitch_dia_gear + 2*addendum pitch_dia_gear - 2*dedendum addendum + dedendum pi/diametral_pitch circular_pitch/2 To view parameters and verify the relations select Show pull down menu, then pick Info Click this “Quick Sash Control” to switch to part graphics area Click the OK button when done From Tools pull down menu, select Relations Pick the cylindrical protrusion in the graphics area The parameter of dimensions appears Type in the following relation in the last line of the editor of Relations window Add the following relations: d1 = theta_4 = theta_1 = base_rad = phi_p = theta_2 = theta_3 = alpha = fr = rd = outside_dia_gear 360/(2*no_gear_teeth) 360/(4*no_gear_teeth) 5*pitch_dia_gear*cos(pressure_angle) sqrt((pitch_dia_gear/(2*base_rad))^2-1) 180/pi*phi_p - atan(phi_p) theta_4 - theta_1 - theta_2 theta_2 + theta_1 root_fillet_radius root_dia_gear Click the OK button when done Click on to regenerate the model Rename the coordinate system, From Edit pull down menu, select Set Up -> Name, pick the coordinate system and enter the new name involute_csys Create a datum curve for the involute tooth profile Select the Insert a Datum Curve icon From Equation -> Done Pick the INVOLUTE_CSYS -> Cylindrical The text editor appears, and enter the following equations: phi = t*sqrt((outside_dia_gear/(2*base_rad))^2-1) r = base_rad*sqrt(1+phi^2) theta = (180/pi*phi - atan(phi)) - alpha z=0 Preview the curve and select OK INVOLUTE CURVE Create a second datum curve for the root of the tooth Select the Sketched Datum Curve Tool icon Pick datum FRONT for the sketching plane and accept default for reference orientation Click Sketch In addition to the default references, carefully pick the inside endpoint of the involute datum curve Sketch a center line through the INVOLUTE_CSYS and create an angular dimension from datum TOP Sketch a second centerline through the INVOLUTE_CSYS that is also aligned to the inside end point of the involute datum curve Second centerline First centerline 10 Enter the following text in the Table: SPUR GEAR PARAMETERS TOOTH FORM: &TOOTH_FORM AGMA QUALITY FACTOR DIAMETRAL PITCH NUM GEAR TEETH GEAR PITCH DIAMETER GEAR OUTSIDE DIAMETER GEAR ROOT DIAMETER ROOT FILLET RADIUS ADDENDUM DEDENDUM WHOLE DEPTH TOOTH THICKNESS CIRCULAR PITCH &AGMA_QUALITY &DIAMETRAL_PITCH &NO_GEAR_TEETH &PITCH_DIA_GEAR &OUTSIDE_DIA_GEAR &ROOT_DIA_GEAR &ROOT_FILLET_RADIUS &ADDENDUM &DEDENDUM &WHOLE_DEPTH &TOOTH_THICKNESS &CIRCULAR_PITCH To modify the Text Style, from Format pull-down menu, select , then pick the text you want to modify Text Style – Click OK – Text Style window appears, and make the necessary changes e.g select the desired font Click Apply and OK buttons 46 The resulted table is shown below: Show the dimensions – diameter of the hole, chamfer, and thickness (face width) of the gear Click 47 Select the Dimension button – see Figure Make sure under Show By, Feature is selected Right click the hole on the FRONT view Pick From List OK Click Accept All button Close Repeat the same procedure for showing dimension of gear thickness (face width) Use Model Tree or Pick From List to choose the protrusion Show the dimension of chamfer – again use Model Tree to select the chamfer Show the axis as the center lines 48 Click Select the Axis button – see Figure Make sure under Show By, Feature is selected Model Tree – Pick the protrusion Extrude OK Click Accept All button Close Modify the chamfer dimension text Click 45° x 05 using left-mouse button, then right click mouse button, and select Properties Dimension Properties window appears Select Dimension Text tab Edit the note to read: 49 Click OK button Show dimension tolerances on the drawing 50 From File drop down menu, select Properties Select Drawing Options The system Preferences window opens with the window drawing setup Scroll down to locate the parameter tol_display Change the value of this to YES 51 Select the Add/Change button, then Apply -> Close Pick the 1.00 width dimension, then right-mouse click the graphics area Properties Change the Tolerance mode to Nominal, and setup the following: 52 First, make sure to change Number of Decimal Places to Click the OK button Pick the 1.00 width dimension, then right-mouse click the graphics area Properties Change the Tolerance Mode to Limits, and setup the following: 53 Repeat the same procedure for the hole dimension – see Figure below for setup: 54 55 Add a surface finish symbol to the bore (hole) surface 56 From Insert pull-down menu, select Surface Finish Retrieve From the Open dialog box, select machined -> standard1.sym Click Open 57 58 Click Open button Entity – Pick the lower edge of the bore hub in the section view Enter 32 for the roughness height Hit Enter -> OK to return to previous menu For the last part of this exercise, enter the necessary information in the title block 59 60