1. University of Puerto Rico at Mayagüez Department of Mechanical Engineering Introduction to NX 6.0 Tutorial 2 Modified by (2011): Dr. Vijay K. Goyal and Dr. Ricky Valentin Associate Professors Juan Reines, Graduate Student Michael Jr. Cruz, Undergraduate Student Department of Mechanical Engineering University of Puerto Rico at Mayagüez

2. Problem Description The model consists of six different features. The base feature will be created using the sketch created on the YC-ZC plane. The next step is to create the joint feature at the top face of the feature. The third feature is the cylindrical feature that will be created on a datum plane offset from the top face of the second feature. The next feature is the hole in the cylindrical feature. The last two features are the holes on the base feature of the model. The following are required to complete this tutorial: Create the base feature of the model. Create the second feature with the Unite option, using the sketch drawn on the top face of the base feature. Create a new datum plane at an offset of 40 from the top face of the second feature. Draw the sketch of the fourth feature on the offset plane and extrude it using the Unite operation. Create the remaining holes in the model.

3. Problem Description The model’s schematic drawing with dimensions are given as follows.

4. Go to Sketch, click on the drop down menu in the Sketch Plane rollout and choose Create Plane then click on the Full plane tool and choose from the drop down menu under Plane the YC-ZC plane, pick Absolute and click OK, on the Offset and Reference menu then pick a reference and click OK. Creating the Base Feature

5. Hit Sketch Left click on the Line feature and create a sketch with the base dimensions After finishing the sketch left Click the Finished Sketch to complete the sketch. Select the Extrude option Creating the Base Feature

6. Select curve Select the Symmetric Value option from the Start drop-down list in the limits rollout. Enter 30 in the Distance edit box, located below the Start drop- down list; the value in the Distance edit box, located below the End drop-down list, automatically change to 30. Ok Select Curve Symmetric Value Distance=30mm ok Base Creating the Base Feature

7. The second feature is also an extrude feature that will be created using the unite operation. The sketch for this feature will be drawn on the top face of the base feature and will be extrude using the Unity Extended option. Select the top face of the base feature and invoke the Sketcher environment. Make sure the X-axis of the new sketching plane point toward the right of the drawing window. Click: Ok Select Planar face ok Creating the Second Feature

8. Draw the sketch for the feature and add the required constraints and dimensions, as shown in figure below. Finish Sketch Creating the Second Feature 1.Draw a circle with a 16mm radius with a distance of 88mm from the edge of the component as shown in the picture. 2.Create two lines joining the sides of the circle with the edge of the component. Make sure the lines have the “Tangential” Constraint applied to them. 3.Utilize the “Quick Trim” feature to get rid of the excess curves.

9. Hit the Extrude option and on Select Curve left click the created sketch. From the Boolean Operations drop down list select the Unite option. Left click on the End option and select until extended and selected the bottom face as a reference for the extrude. Hit Ok. Creating the Second Feature

10. The feature is now created. We can proceed to the third feature. Creating the Second Feature

11. Creating the Third Feature The third feature is created on a datum plane created at an offset of 40mm from the top face of the second feature. Click on: Datum Plane At Distance from the drop – down list in the Type rollout and select the top face of the second feature

12. Enter 40 in the Distance edit box and choose Ok from the Datum plane dialog box. (The New Plane is crated) Creating the Third Feature

13. Invoke the sketcher environment using the new datum plane. You can define the orientation of the X-axis of the sketching plane using one of the straight edges of the model. Draw the circle for the third feature. Make the circle concentric with the curve in the second feature and then make a curve and circle of equal radius. As a result, you will not have to apply any dimension to the sketch. Creating the Third Feature

14. Click on: Finish Sketch > Extrude Select the sketch Unite from the Boolean Reverse Direction 60 in the end edit box Ok.

15. Change the current view to the Isometric view and hide the sketch. The model after creating the cylindrical feature is shown in figure below. Creating the Third Feature

16. Creating the Remaining Feature Create the remaining feature which are holes. To Create these holes, you need to extrude the sketches using the subtract operation. Hit Sketch. Select the offset datum plane. Draw a 22 diameter concentric circle. Hit Finish Sketch.

17. Select Extrude. Select the Created sketch as the extrude curve. Under Boolean Operations select substract. Type 60 on distance. Hit Ok. Creating the Remaining Feature

18. The feature is now created. Creating the Remaining Feature

19. The next step of the Fourth feature is to create the Holes on the base feature. Let’s start with the top face holes. Click Sketch. Select the top face as the sketch ground.

20. Start by creating a circle of diameter 6. Impose the constraints as indicated in the dimension’s sketch. Hit Finish Sketch. Left click on Extrude. Select the created sketch as the curve and select Subtract from the Boolean Operations Drop down list. Type 10 on the Distance tool box. Creating the Remaining Feature

21. The last feature is also a hole. Left click on the Sketch feature. Select the rear face of the base feature as the sketch ground.

22. Creating the Remaining Feature Draw two circles of diameter 12. Apply the required constraints.

23. Creating the Remaining Feature Hit the Extrude option. Select the existing sketch as the curve. Under Boolean Operations select subtract and type 8 as the extrude distance. Hit Ok. The feature is now created. The model is complete.

24. Final Model For Tutorial Creating the Remaining Feature

25. Creating the mesh On the top left corner select the drop down of Start and select Advanced Simulation. On the Simulation Navigator right click on tutorial_1.prt Select New FEM and Simulation. Make sure Structural is selected on the Analysis Type section and hit ok. On the Solution Type you can select the constrain you want, on our case select SESTATIC 101 – Single Constraint and click ok.

26. Creating the mesh Use the 3D Tetrahedral Mesh feature as shown in figure on the right. This feature is available on the _prt_fem1 Session on the Simulation File View. On the Type section, select CTETRA(4) On the Overall Element Size, choose at least 6. Click on the solid model and ok.

27. Creating the mesh (cont). Use the Mesh Control feature as shown in figure on the right. Use Size on Face, on the Density Types section Select hole as shown on figure. On the Element Size section, use 2mm or less and click ok.

28. Use Update Finite Element Model feature shown on the figure in order to regenerate the mesh. Now the element size on the orifice will become smaller… Creating the mesh (cont).

29. Do the same procedure with the other holes of the model as shown on the figure. Remember to use Size on Face on the Density type section.

30. Creating the mesh(cont). Finally, use Mesh Control to refine the mesh on the edge that connects the plane with the circular contour as shown. On the Density Types section, select Size on Edge. Pick both edges as shown in the figure. To see the amount of extra nodes added to the edge being selected, click on the icon shown on the figure.

31. Creating the mesh(cont). When the meshing procedure is done, you can appreciate the different element densities on the solid model. Choose File > Save All from the menu bar to save the file.