Assembly Receiver/Hitch/Ball/Pin to use for CAD LAB 5A and 5B:

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1 MECH 130 CAD LAB 5 SPRING 2017 due Friday, April 21, 2016 at 4:30 PM All of LAB 5 s hardcopies will be working drawing layouts. Do not print out from the part file. We will be using the ME130DRAW drawing sheet layout for our drawings generated from the SolidWorks part we will be building. Lab 5A and 5B will require you to download 1 part (the receiver) from the class webpage to use in conjunction with the three parts you built for Lab 4. You will make an Assembly and then create a drawing layout for 5A and 5B. Lab 5C requires you to build a part from scratch and then create a specified working drawing layout. All drawings are printed at SCALE 100%. THERE IS A TOTAL OF 3 HARDCOPIES (5A, 5B, 5C) for this entire lab. DO NOT FORGET TO DO 5C Instructions for it can be found in the PDF online if you did not pick up that separate set of instructions. Assembly Receiver/Hitch/Ball/Pin to use for CAD LAB 5A and 5B: Download the Receiver part (called HUSKER_RECEIVER.SLDPRT) from the class web page. You will be using this part file in addition to your Hitch/Ball/and Pin Parts created for Lab 4. It is a good practice to have all of the files in a single folder and to have deleted the annotations (Do NOT delete DIMENSIONS) used for Lab 4. UTILIZE THE ASSEMBLY TEMPLATE FOR OUR CLASS: ME130ASSEM.asmdot found on the class webpage DOWNLOAD like you did for parts and drawing document templates. Insert the Receiver first. Remember to click the OK button which is the GREEN CHECKMARK (in order to have it fixed.) Insert the components (hitch/ball/pin) each separately into the assembly. You will need to mate the parts in a logical fashion. VERY IMPORTANT TO NOTE: some of these illustrations do NOT show exactly what your parts/sizes or what the parts going into the assembly are named. Illustrations just give the GENERAL look of the assembly. Always look at your given drawing layout assigned to determine YOUR lab s resultant assembly. Receiver and Hitch Mates (THREE of them) (1) Coincident Principal Planes (2) Parallel Principal Planes (3) Coincident Axes. 1 2 Mate #3) View temporary axis and make the Axis of the two holes (one in receiver and one in hitch) to be coincident. REV 1 S17_LABFIVE_original.doc Page 1 of 10

2 Hitch and Ball Mates (Need two of them so hexagon of ball does not spin) (1) Coincident Edges (2) Coincident Principal Planes Mate #1) Edge of hitch s hole will be coincident with edge of ball s projection Started like this Mate #2) Principal planes are coincident or parallel depending on how you built the ball. Notice the orientation of the hexagon on the hitch needs to follow what is shown in the final hardcopy (it may not be shown in the proper orientation here) Hitch and Pin Mates (3 of them) (1) Coincident Axis (2) Distance Mate (3) Parallel principal planes View temporary axis as needed Mate #1) the Axis of the hitch and the axis of pin should be coincident Mate #2) Face of receiver and face of pin set to be a specific distance (.5000 ) apart. This may need to be checked on. Mate #3) Principal plane of pin and plane of Hitch made Parallel so that the pin doesn t spin in the hole. Note the orientation of the pin from the given orthographics in your resultant drawing layout, S17_LABFIVE_original.doc Page 2 of 10

3 IMPORTANT to note: UPON ASSEMBLY YOU WILL NOTICE THAT THE PIN IS TOO SMALL OF DIAMETER AND other issues with curvature. EDIT THE PART AND Change the original circle within the 1 st Swept Feature (FOR SWEEP) to a DIAMETER OF.875 Change the hexagon sketch for the 2 nd Swept feature from n.7500 to a n (This change should take care of any warning that may pop up.) Open Part Open Part in Positon Edit the part (in context) Pin is highlighted in tree then right click will bring up pop-up menu, top folder icon will open part Next to it is the Open Part in Position YOU WILL ALSO NEED EDIT THE HITCH PART AND CHANGE the HOLE the pin enters it should also have a DIAMETER OF.8750 Once everything is assembled, you ll need to create an Exploded View. IMPORTANT: You should explode the assembly in the assembly file in order to have the option of including the exploded view in the drawing file. The exploded view is used for one of the hard copies so you can look at the picture there to see the general ideas/directions Step1: The pin is moved 6 out along its main axis. Step 2: The hitch and ball are both selected and then moved out of the receiver 5. (They should move together have both selected before pulling them away) Step 3: Ball is then moved up 3. Once the exploded assembly has been completed, save the Assembly. Then start a new drawing for each of specific drawing layouts which involve assembled views. S17_LABFIVE_original.doc Page 3 of 10

4 CAD LAB 5A: Assembly Orthographics with Detail & Sectioned Views. Specifics: Orthographics of ASSEMBLY are at Scale 1:5 and the automatic scale found in the titleblock should reflect that. Hidden Lines are visible in all views except the sectioning. Tangent Edges are Removed in all views. Section A-A is at middle of ball. Don t exclude anything from the section view. Do not show hidden lines. You will also need to Break Alignment once it has been placed. Right Click on the View get the options shown. Modify the hatching (uncheck the Material crosshatch option) for the Ball, the Pin and the Hitch. See the settings shown at right. Accept the default hatching of the receiver. Detail of Pin is a SCALE of 1:2 it should look like what is shown, the detail circle size can vary but it should have same style (connected) & be approximately as shown. Include dimensions and annotations as shown (including text/arrows inside or outside) and to precision shown document is set to.001 Scale 1:5 S17_LABFIVE_original.doc Page 4 of 10 Ball Hitch Pin

5 CAD LAB 5B: Revised PIN Orthographics /Exploded PICTORIAL View Scale 1:1 Specifics: Orthographics of Pin are at Scale 1:1 and the automatic scale found in the titleblock should reflect that. Only include the two views (front and left) as shown (they should be aligned) Tangent edges are Removed. Hidden Lines are Removed Exploded View is only possible if the assembly had an Exploded View done (see earlier page of this document) Scale 1:4 for exploded TRImetric view Shaded with edges (turn on lights if you need to) Tangent Edges with Font Insert Model Items to get dimensions of the PIN. Source should be Entire Model. You can use the pull-down of VIEW>HIDE/SHOW>ANNOTATIONS to manipulate their display. You can also Hide unwanted dimensions by highlighting the dimension and then doing a right-click to get the pop-up menu needed or you Move a model dimension from one view to other by SHIFT-Drag This button is what it means by select the type of Model Item you want Dimensions>Marked for drawing The dimension is highlighted and then will want to select Hide from the pop-up menu. Adjust precision (using document global setting to 3-decimal) and placement of dimensions to be as shown. Adjust arrows inside or out. Include all additional annotations. S17_LABFIVE_original.doc Page 5 of 10

6 THIS IS JUST A DUPLICATION OF 5C HANDED OUT EARLIER CAD LAB 5C: Build Radially Symmetric Object Create the part You will need to assign a Copper material TO THE PART and then start a new SolidWorks drawing you will print out the drawing at 100%. SOME OF THE ILLUSTRATIONS SHOWN WILL NOT MATCH THE ICONS FOR Solidworks 2016 SCALE 1:2 Specifics: Orthographics are at a Scale of 1:2 and the automatic scale found in the titleblock should reflect that. Delete the right side view and then create a Sectioned View (remains aligned as shown) using a cutting line through the middle of the object. o Sectioned View should not have hidden lines displayed. o Leave the Material crosshatch setting CHECKED ON Tangent edges are removed in all views except for the rotated view that has them displayed as phantom. Use an auxiliary view to show the projection at the 30 angle, true size. MAINTAIN ALIGNMENT Under Options and the Document Properties tab change the precision of dimensions to.01 o Dimensions should also be placed as shown, including whether arrows inside/outside of extension lines. o Add a centermark on the auxiliary view, its tool is found in the annotation tab. Include all notes as shown. The rotated view) will need to be saved in the part file before it can be placed in the drawing. It is placed with a SCALE 1:3 and is displayed without hidden lines but with tangent edges shown as font. In order to build the part, please refer to the drawing above for some of the sizes and specifications. ALSO there are additional SKETCHES/SIZES SHOWN ON THE FOLLOWING PAGES! S17_LABFIVE_original.doc Page 6 of 10

7 Here s are the various sketches and methods to use for the part. Assume sizes are in inches. Be sure that Merge Results is always CHECKED ON. A circle of Ø inches with its centerpoint at the origin. Shown is the resulting cylinder in isometric. Insert three additional reference geometry planes. Each are parallel to the Front principal plane. They are spaced as.50, 1.5, and 3.0 inches from the Front Principal plane Here are the sketches when complete (the next page shows each specific sketch. S17_LABFIVE_original.doc Page 7 of 10

8 Here are the 3 sketches to use for the profiles for the loft. Slot sketched on Plane 1 Slot sketched on Plane 3 Sketch On Plane 2 Here is the isometric pictorial result after doing a CIRCULAR PATTERN FEATURE. S17_LABFIVE_original.doc Page 8 of 10

9 Continuation of sketches and methods. Sketch on the Top Principal Plane. Circle to use for Extrude with a THIN FEATURE option. Depth of 1.00 inches MIDPLANE Thickness of.30 inches Create a sketch on the bottom face and use CONVERT ENTITIES to get a single circle to use for Extrude (THIN feature) Sizes (Blind distance of.2500 inches and Thickness as.4000 inches) as indicated below. Use a SINGLE fillet feature Radius of.1000 inch to round and fillet the two edges needed (refer to sheet layout detail). S17_LABFIVE_original.doc Page 9 of 10

10 Completion of part INSERTING A 30 REFERENCE plane TO DRAW ON Viewing Temporary Axis is important so that you can select the Axis of the cylinder for the second reference. Sketch on the plane, this type of sketch will work (piece will come in with a hole in it) There are 3 lines, 1 arc tangent to both horizontal lines, and an 8-sided polygon centered with the arc. EXTRUDE IT MIDPLANE a thickness of.40 Save a rotated view of the object to use in the sheet layout! Don t forget to assign a material to the part before doing the drawing. It is COPPER. S17_LABFIVE_original.doc Page 10 of 10

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