WEEK 5: Shaft Modeling (C51X01, C51X02) Revolved Features, Chamfer

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1 WEEK 5: Shaft Modeling (C51X01, C51X02) Revolved Features, Chamfer 1. Creating the Shaft Model 1. File> New> Part, Name: C51X01> OK 2. Insert> Revolve> Placement> Define> select TOP datum plane> Sketch 3. Draw a vertical centerline from the origin 4. Sketch> Options > Constraints, Turn off equal length > Checkmark 5. Sketch shaft geometry starting from the origin. Make sure that all lines are either vertical or horizontal. The curve must be closed. 6. Choose all dimensions and select Modify dimension icon. Activate Lock Scale and the first dimension (sd0) to Apply all diameter dimensions (0.627, 1.00, 0.75, 0.562, 0.62, ). First select dimension icon, select the line that will be dimensioned, select centerline, select the line again, and then click middle mouse button at the location that you want to put the dimension. This will make diameter dimension. Correct these dimension values. 8. Correct dimensions for the thread relief (0.06 wide and 0.04 deep) 9. Apply vertical dimensions (0.88, 1.00, 0.59, 2.27, 3.80, 1.00) as shown in the figure below. First make dimensions and correct their values. 5

2 10. Select the diameter dimension 0.62 and select modify dimension icon. Modify Dimension window will appear. Note that the dimension variable is sd21 and the value of the dimension is We will use this dimension to create Datum Plane later. 11. Click the checkmark to finish the sketch. 12. Verify the correctness of the revolved shaft and click the checkmark to make revolved shaft. 13. Rename the revolved feature to SHAFT 14. Insert> Chamfer> Edge Chamfer. Change chamfer type to D D and select Sets. Change D value to 1/16 and select References. In the graphic window, select Edge 1 and 2 (hold CTRL key to select multiple items) 15. In order to create additional chamfer, select *New Set, change the chamfer type to D D, change D value to 0.03, and select Edge Verify the correctness of the chamfers and click the checkmark to make chamfers. 6

3 Edge 1 Edge 3 Edge Insert> Model Datum> Plane. Choose TOP datum plane and provide sd21/2 as Offset value. Click OK to generate a datum plane. Note that sd21 is the diameter of the shaft and we want to offset the datum plane by the radius. When the diameter of the shaft is changed, the datum plane will automatically be moved. 18. Create a key seat by sketching on the created Dtm1 datum plane. Insert> Extrude> Placement> Define> Select Dtm1> Sketch 19. Sketch the cross section of key seat, as shown in the figure. First create two arcs on the centerline with the same radius and make two lines tangent to the arcs. Delete all duplicated dimensions while creating these constraints. Surface 2 Surface Select the checkmark to finish the sketch and utilize blind extrusion by in to remove material from the shaft. 21. Make a thread using Insert> Cosmetic> Thread. Thread window will appear. Select thread surface (surface 1), select start surface (surface 2), click Okay for direction, click Done for Blind depth, type in 0.88 and checkmark for thread depth, click checkmark again with DIAMETER = In order to change other parameters, select Mod Params. Pro/TABLE will appear. Modify the following values: THREADS_PER_IN: 20; FORM: UNF; CLASS: 3; PLACEMENT: A (external); METRIC: FALSE Choose File> Save and File> Exit to finish defining thread parameters. Choose Done/Return. Choose OK. 7

4 22. Right click on Cosmetic id in the model tree and select Setup note> Feature. Note window will appear. In the text area, type in 1/16 20UNF 3A X.88 THREAD DEPTH. Select Place >select TOP datum plane> Okay> select 180> Done> With Leader> Done> Choose edge of the top thread> Click middle mouse button to the location that you want to put the note. File> Save> OK 2. Creating Initial Drawing 1. Make a new drawing: File> New> Drawing, Name: C51X01> OK. Choose Empty with format option and select inbprow.frm. Select OK to make a new drawing. 2. File> Property> Drawing Options. Open eml2023inch.dtl file using Open icon. 3. In the Option section (at the bottom), type in tol_display and choose yes in the value section and select Add/Change and OK. This change will show tolerances in all dimensions. 4. Select Done/Return to close Menu Manager. 5. Insert> Drawing View> General. Click a location in the drawing that the view will be placed. Drawing View window will appear. 6. In order to place the shaft properly, first choose TOP in Model view names and click Apply. The shaft will be placed vertically. Next, select Angles method and type in 90 degree. Click Apply button. Now the shaft is properly located. 7. Select Scale> Custom Scale> Select View Display section. Select Hidden for Display style and None for Tangent edge display style. Click OK to create a general view. 9. Make horizontal and left profile views using Insert> Drawing View> Projection. Make sure the frontal view is selected first before projection. 10. Show dimensions using View> Shaw&Erase command. In Show/Erase window, select dimension icon and centerline icon. Click Show All> Yes> Accept All> Close. Note that all dimensions are shown in upper and lower limit values. 11. Double click one of diameter dimensions. Dimension property window will appear. Change tolerance mode to + symmetric and modify tolerance values according to the drawing in the workbook. 8

5 12. For the length dimensions, choose Nominal for the tolerance mode so that tolerance will not appear. 13. Modify dimensions associated with chamfers to.06 X.06 CHAMFER BOTH ENDS and.03 X.03 CHAMFER. 14. Erase dimensions associated with thread relief and add note.06 WIDE X.04 DEEP THREAD RELIEF. 15. Insert> Note> With Leader> Make Note. Select an edge that the note will be made and click middle mouse button on the location that the note will be made. Type in the content of the note and click the checkmark. Click the checkmark again to finish making the note. Repeat this process for all notes for chamfers, thread, and thread relief. 16. Insert trimetric view of the shaft using Insert> Drawing View> General with scale = Use Show&Erase to show centerline. 17. Save the drawing (C51X01.drw) and File> Close to close the drawing. Now the part window will be shown. 3. Save a Copy with Association and Changing Dimension 1. Choose Tools> Options. Option window will appear. 9

6 2. Type in rename_drawing_with_object at the bottom of Options window, and choose both in the value section. Select Add/Change and OK. Then, when the part file is saved to a different filename, all associated drawings will also change accordingly. 3. File> Save a Copy command to save the part file to a new name C51X02.PRT. Check the working directory and verify that two files (C51X02.PRT and C51X02.DRW) are created. 4. Close the current part file (File> Close) and open C51X02.PRT file using File> Open 5. In the model history window, click + sign in from of the SHAFT feature. S2D0001 will appear. Right click on S2D0001 and select Edit Definition command in the top down menu. The sketch of the shaft will appear. 6. In the shaft sketch window, change the dimension to (main length of the shaft). 7. Click the checkmark. Now the length of the shaft part is changed to Save the part file using File> Save. 8. Open the drawing file C51X02.DRW and verify the length of the shaft is changed to in the drawing file. 10

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