Tài liệu 21 brake rotor udf and family table

ME-430 Introduction to Computer Aided Design BRAKE ROTOR USING UDF & FAMILY TABLE Pro/ENGINEER Wildfire 2.0 Dr. Herli Surjanhata In a system window, create a new directory called Brake_rotor under ME-430 directory (e.g. J:\PTC_Working_Dir\ME-430\Brake_rotor) if this has NOT been done. From File pull down menu, select Set Working Directory. Select Working Directory dialog box appears 1 Select the ME-430\Brake_rotor directory to highlight it and select OK. All files created in this session will be stored in ME-430\Brake_rotor directory. Note: You can also create a new directory by selecting . CREATE A UDF PART Pick the Create a new object icon . 2 Type in udf_rotor for the name of the new part. Click OK. CREATE A BASE FEATURE – A Solid Disk Protrusion Create the base feature – Pick the Extrude Tool icon . In the dashboard, click -> . 3 Pick Front datum plane as Sketch Plane. For Sketch Orientation Reference pick RIGHT datum plane, and set Orientation to Right. This option is default option! Then click the Sketch button . Click the Close button in the References dialog box. 4 Click on . Draw a circle centered at the origin of coordinate system. Dimension the circle for 10 inches as shown below. Click on . Change the depth of protrusion to 1.0. Choose both sides protrusion icon . 5 Click Click . and select Standard Orientation. CREATE THREE HOLES USING CUT PROTRUSION Click on . Click on the axis of the disk. While press and hold down Ctrl key, click on TOP datum plane. Set Offset - Rotation to 0.0 Click on OK. A new datum plane DTM1 will be created. 6 Create the base feature – Pick the . Extrude Tool icon In the dashboard, click on the Remove Material icon . -> Next, click . Pick the front surface of the disk as Sketch Plane. For Sketch Orientation Reference pick DTM1 datum plane, and set Orientation to Top. Then click the Sketch button . Pick on the horizontal line (thru default coordinate system) that represent DTM1 datum plane. Pick on the circle. Click the Close button in the References dialog box. Draw two centerlines, and dimension it as shown below. 7 Zoom in to the right portion of the disk. Draw and dimension three circles of 0.25 in. as shown below. 8 Click on . Choose on Through All icon for Options. 9 Click on . CREATE CHAMFERS Pick the Chamfer Tool icon . Pick the right edge of the handle. Change the chamfer option to Angle x D. Enter the Angle value of 30 degrees. Enter the D value of 0.05 in. Pick on six circular edges of the three holes as shown. Click on . 10 The part shown above will be used to create the User Defined Feature (UDF) and the UDF will be created in the vented brake rotor. Instances of the brake rotor will be created that are 10, 11, 12, and 13 inches in diameter. These instances will contain different cross drill patterns. CREATE UDF Tools -> UDF Library Click on Create. Enter cross_drill for the UDF name. Then click on . 11 Click Stand Alone -> Done Choose Yes to the prompt “Do you want to include reference part?”. Select DTM1, the hole feature, and the chamfer in the Model Tree. Done -> Done Return For the axis prompt, enter Select the center axis of the rotor. Hit [Enter]. For the datum prompt, enter Select the angular reference plane. Hit [Enter]. For the front rotor surface prompt, enter 12 Select the cross drill placement surface. Hit [Enter]. For the outer surface prompt, enter Select the outside surface. Hit [Enter]. For the back rotor surface prompt, enter Select the rear rotor surface. Hit [Enter]. Click on Done/Return to complete the prompts. Select Family Table. Click on Define. The Family Table dialog box appears. Click on . Click on the cut (holes) to display the dimensions. 13 Zoom into the area where the three holes are located. 14 Pick on Ø.25, and enter hole_diam for the symbol. [Enter] Pick on 1.75, and enter offset for the symbol. [Enter] Pick on 0.75, and enter spacing for the symbol. [Enter] 15 Click OK. Click on . 16 Enter the values as shown in the figure. Repeat the same technique to complete the Family Table as shown below. Click OK to complete the Family Table. OK -> Done/Return. Create a relation for the spacing. Tools -> Relations The Relations dialog box appears. Enter the relation in the editor; “d34=d33”. Note that your parameters may be different from this tutorial. The relation that has been created is d34=d33. 17 Click on OK. Save and close UDF_ROTOR.PRT. CREATE A ROTOR PART Pick the Create a new object icon . 18 Type in rotor for the name of the new part. Click OK. CREATE A BASE FEATURE – A Hollow Disk Protrusion Create the base feature – Pick the Extrude Tool icon . In the dashboard, click -> . 19 Pick Front datum plane as Sketch Plane. For Sketch Orientation Reference pick RIGHT datum plane, and set Orientation to Right. This option is default option! Then click the Sketch button . Click the Close button in the References dialog box. 20