Top Down Assembly Modeling Release Wildfire 2.0

Transcription

1 Top Down Assembly Modeling Release Wildfire 2.0 Note: Comprehensive Modeling Assignment This is a 30 point assignment as such takes the place of the final exam. Four Plate Mold Base, Inner Two Plates Begin by modeling up the LOWER MOLD BASE. (Material: AISI 4130 STEEL) Overall plate size is 8 by 5. Use relations to keep the datum planes centered inside the base. Create counter bores using the Sketcher option in the Hole Feature Option. Through holes have a diameter of Holes are located 2 inches and inches from center. The counter bore (from the bottom side) has a diameter of.875 and is.125 deep. These are patterned, which is why there are two 2 Holes reference shown in the figure below. 1

2 After finishing this part, begin an assembly. Insert - Component Assemble the part above. Mate the Lower Mold Base FRONT to ASM_FRONT, TOP to ASM_TOP, and RIGHT to ASM_RIGHT. We now wish to create a part, called the Upper Plate and is made of AISI 4130 Steel, that is fully referenced to the Lower Mold Base. To begin a part that references geometry in an assembly, select Insert - Component Create Select Locate Default Datums and Three Planes. Select the planes as directed on the next page. Spin the Lower Mold Base so the top surface of the plate is facing the front as shown below. This is to make it easier to select surfaces. Show all of the assembly features in the model tree by choosing Settings Tree Filters - Features. This will allow you to choose the datums from the model and not from the assembly. 2

3 o o You are prompted to Select first plane, which will also be used as a sketching plane. Pick the top surface of the plate (the one that is facing front at this point). o o The next prompt is to Select horizontal plane (will be TOP reference when sketching). Pick the MODEL Front datum plane. o o The final prompt is to Select vertical plane to be used for placement. Select the MODEL Right datum plane. o o You get a message that the Component has been created successfully. The components that are being referred to are the new datum planes for the Upper Plate. These are shown below. Right click on Mold_Base_2.PRT in the model tree and select Activate. If there is no Activate pick, this means the component is already active. Create a solid protrusion as shown on the following page using Insert Extrude to create solid geometry. Use Edge - Single. block now being created. to define the edges of the rectangular Notice that you are looking at the initial base from the bottom side. This is because the system is going to do a Mate when it automatically sets the constraints for locating the new component being created in context. Since 3

4 protrusions extrude out of the screen by default, the extrusion direction will need to be re-defined. Select the edges of the existing part to place reference lines. Sketch the Upper Plate using existing edges of the Lower Mold Base as well as the inside diameter circles as guides. The sketched lines will be aligned with the Lower Mold Base. The protrusion will be Blind, use a depth of Redefine the Direction After finishing, the result should be as shown below. Testing your result: Select Edit and pick on the protrusion on lower mold base, Mold_Base_1 (not on the upper mold base). Dimensions appear as shown. Change the 8 dimension to 16. Regenerate. 4

5 Both parts change to reflect the updated dimensions as shown on the following page. Since the holes were referenced from the center datums, they did not move. If the mold did not regenerated correctly, fix it so it does. When it regenerates correctly change the 16 back to an 8. It is possible to create a part with out starting from datum planes. The Shoulder Bushing will be used as an example. Start to create a part as before, except use Create Features This component is now Active, it is not necessary to activate it. Create a Revolved Protrusion, but when prompted to select the sketching plane, pick on the Datum icon to create a datum on the fly. Use the axis of the initial hole in the Lower Mold base as well as the Frontal Datum for references. Set the angle to 0. Sketch the revolved feature. Note that the inner bore is the only thing that needs to be dimensioned. Other edges are aligned to existing through hole and counter bore. 5

6 o o Upon selecting Done, the shoulder bushing is created. The model tree will appear similar to the following: After doing three Insert - Component Assemble operations with the Shoulder Bushing, Aligning surfaces and axis, the Shoulder Bushings are now located in the Lower Mold Plate (shown upside down with the Upper Plate hidden). 6

7 Turning our attention back to the Upper Plate, the holes in the base must have a counter bore in the top surface. If you select File Open to open the file, it will not appear in the working directory since it has not been saved yet. To activate the part window, select File Open pick in the Look In box and select In Session. Pick on the Upper_Plate file to open 7

8 Create a hole (Coaxial) representing the counter bore making sure to use the upper surface of the plate for reference purposes. o The upper surface is opposite the side that has DTM3 associated with it. o Remember, DTM3 is mated to the top side of the lower mold base. The hole diameter is.875 with a depth of.25. You can use Edit Feature Operations - Copy New Refs - Select Dependent to locate the other three counter bores. The only new reference that needs be chosen during this operation is the axis on the through holes. All other dimensions remain the same. Jumping back to the assembly, the screen appears as: Modifying the long dimension of the lower mold base to 10 will result in: 8

9 o o The holes will not change until dimensional modifications are made to the location on the Lower Mold Base. (The Lower Mold Base is shown upside down in the figure below for visibility purposes.) Notice how these holes were created for this particular model. Since they were patterned in two directions, if dimensional modifications are to be made to both the and dimensions they must be made simultaneously. Leader Pin creation. o o The Leader Pins were created in exactly the same way as the Shoulder Bushings. Note the sketch below. The definition of the pins requires no dimensions at all. The entire part is a function of the two mold bases and the bushing. 9

10 Screen Capture and print the following two images as shown: Finished leader pin assembled into the other three holes. Changing: The length of the base from 8 to 12. The location of the holes (from center) from to The distance between the holes from to The thickness of the Upper Plate from to

11 Results in: Screen Capture and print the above image Create and turn in drawing files for the bushing and ejector pin. Notice the only view available in the part file is the Default. (Front, Side, Top, etc., are missing.) When creating the drawing file, o select Empty with Format o o select the Browse button and select a_horiz_english.frm. if an assembly file is open, make sure the appropriate part file is listed in the Default Model box. If not, use the Browse button to locate the appropriate file. 11

12 o o Enter Part name, drawn by, material, and part number. Add the front view. Change Type to Preferences. (See figure below) Change Default Orientation to User Defined. Edit the appropriate X or Y coordinate. Select OK. o Add adjacent view(s). When finished, change the Default View back to isometric. (Utilities, Environment Default Orient Isometric.) Make sure your drawings are properly dimensioned! Part of the grade on this assignment will be the dimensioning of the parts! 12