1. University of Puerto Rico at Mayagüez Department of Mechanical Engineering Introduction to NX 6.0 Tutorial 3 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 objective of this tutorial is to create the figure shown below using NX 6.0. The schematic drawing of the solid part can be seen below.

3. Problem Description For better understanding of the dimensions from the solid part, the original schematic drawing is included in the figure below.

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. Click on the Line Icon on the top left of your screen. Place the mouse on the screen and it will ask you the coords of where you want your line to start, for this case XC = -43 and YC = 9. Then press enter. It will ask you the length of the line and angle, which is 86 and 0 respectively. Afterwards just keep on making lines by clicking the end of your last line, then entering the length and angle in the order shown on the table. Once you have a sketch like the one to the left click on Finish Sketch.

6. 3 2 1 4 5 7 6 8 9 # 1 st Box 2 nd Box 1-439 2860 318270 413180 5290 660180 72270 813180 91890 Creating the Base Feature

7. Next step is to extrude the sketch. Click on the Extrude Icon beside the Sketch Icon. Click on Select Curve and click on the sketch. In the limits box put Symmetric Value and 70 mm as the Distance, then click OK.

8. Creating the Second Feature To create the second feature, invoke the Sketch tool from Feature toolbar and select the back face of the base feature as the sketching plane.

9. Creating the Second Feature Click on the Line Icon. Click the upper left corner of the base as the starting point of your line then write a length of 38 and an angle of 90. Then press enter. Click on the Circle Icon, which is beside the Arc Icon. Write the coordinate -50, 47 and diameter 40. The press enter. Do the same thing again but with coordinates 20, 100 and diameter 50. Click on the Arc Icon, which is beside the Line Icon. Then click on the Quadrant Icon shown on the Figure at the bottom and deselect all the other options. This is so we only have snaps on the quadrant points of the circles. Make an arc of radius 25 from top quadrant of the 40 diameter circle to the left quadrant of the 50 diameter circle.

10. Click on the Line Icon and throw a line from the right quadrant of the 50 diameter circle to the upper right corner of the base. Make another line from the upper left corner of the base to the upper right corner of the base to have a closed section to be able to extrude. Click on the Quick Trim Icon to cut out the extra lines. Click on the lines marked with an X on the figure to the left. X X Creating the Second Feature

11. Next, choose the Extrude button from the Feature toolbar and select the previous sketch. On the Limits section the parameters are: Start: 0 End: 12 On the Boolean drop down list, press Unite. After these Press Apply and then hit OK key.

12. Creating the Third Feature Invoke the Sketch tool to create the third feature. As previous steps, select the area were you want to draw the new figure (Front View) and select the Circle tool on the sketch menu. Create a circle at the same position of the second figure of Diameter = 50. After These steps, press Finish Sketch.

13. Choose the Extrude button from the Feature toolbar and select the previous sketch. On the Limits section the parameters are: Start: 0 End: 35 On the Boolean drop down list, press Unite. After these Press Apply and then hit OK. Creating the Third Feature

14. Creating the Fourth Feature Press the Sketch tool to create the Fourth feature. As previous steps, select the area were you want to draw the new figure (Front View) and select the Circle tool on the sketch menu. Create a circle at the same position of the second figure of Diameter = 40. After These steps, press Finish Sketch.

15. Choose the Extrude button from the Feature toolbar and select the previous sketch. On the Limits section the parameters are: Start: 0 End: 30 On the Boolean drop down list, press Unite. After these Press Apply and then hit OK. Creating the Fourth Feature

16. Click on the Hole Icon on the Top Center of your screen. Click on Specify Point and another screen will pop up. Choose the center of the 3 rd Feature. Then Click OK. Make sure you change all the necessary parameters like the figure to the side. Click on Select Body, then click on the 3 rd Feature. Click OK. Creating hole in 3 rd Feature

17. Click on the Hole Icon. Click on Specify Point and another screen will pop up. Choose the center of the 3 rd Feature. Then Click OK. Make sure you change all the necessary parameters like the figure to the side. Click on Select Body, then click on the 2nd Feature. Click OK. Now you have a hole through both features. Creating hole in 3 rd Feature

18. Creating hole in 4 th Feature The process for this hole is the same as before, but with a diameter of 20 mm. You should end up with the figure to the left.

19. Creating the base holes To create the four holes in the base feature, choose the Command Finder In the command finder search, write Pre-NX5 Hole and select the button from the matches list.

20. Enter the value of diameter of the holes as 10 in the Diameter edit box and select the top face of the base feature. After these steps, press Apply. Creating the base holes

21. Select these edges and edit it values Next, choose the Perpendicular option from the Positioning dialog box and select the base edges shown in the figure.

22. Similarly, create the remaining three holes. To know the require dimensions, please refer to the following drawing (Top view): This is the final model after creating all the four holes in the base feature. Creating the base holes

23. 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.

24. 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. Click on the solid model. On the Overall Element Size, choose 10 or less.

25. 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 holes as shown on figure. On the Element Size section, use at least 2mm and click ok.

26. Creating the mesh(cont). 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…

27. Creating the mesh (cont). Use the Mesh Control feature as shown in figure on the right. Use Number on Edge, on the Density Types section Select edge as shown on figure. On the Number of Elements section, use at least 25 and click ok. In order to see the number of elements before finishing the procedure, on the Preview section click on the icon shown in the figure.

28. Creating the mesh (cont). Use the Mesh Control feature as shown in figure on the right. Use Size on Edge, on the Density Types section Select round edge as shown on figure. On the Element Size section, use at least 2mm and click ok. In order to see the number of elements before finishing the procedure, on the Preview section click on the icon shown in the figure.

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