Laboratory Exercises

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1 Laboratory Exercises 4 : 1

2 Lab 1A Inverted T Inverted T. Draw the solid object shown. Place the origin at the intersection of the faces with the holes in them. The front face is marked for you. Make sure all features are fully defined before extruding and rename all features. Note that the slot is off center and not through all. Do not have dimensions on the drawing you print out. (You will have to dimension the sketches in the part.) Save the part to your disk with a file name of yourlastname1, i.e. Ludin1. Bring the part into a three view drawing on a landscape title block. Also bring in an isometric view. With proper placement a 1:1 scale may be used. Fill in the title block with your name, date, lab section, lecture section and units. The drawing number is 8374, the title is Inverted T and the material is titanium. Save the drawing to your disk with a file name of yourlastname1, i.e. Ludin1. Submit a hard copy of the drawing (title block, not the part) and electronic copies of both the part and drawing. Save all your electronic files to a flash drive in case you need the files again.. 4 : 2

3 Lab 1B Inverted T Bar Inverted T Bar. Draw the solid object shown. Place the origin at the position shown in the drawing. This is a standard isometric view and the front face has been marked for you. Make sure all features are fully defined before extruding and rename all features. Note that the slot is off center and not through all. Do not have dimensions on the drawing you print out. (You will have to dimension the sketches.) Save the part to your disk with a file name of yourlastname1, i.e. Ludin1. Bring the part into a three view drawing on a landscape title block. Also bring in an isometric view. With proper placement a 1:2 scale may be used. Fill in the title block with your name, date, lab section, lecture section and units. The drawing number is 23475, the title is Inverted T Bar and the material is titanium. Save the drawing to your disk with a file name of yourlastname1, i.e. Ludin1. Submit a hard copy of the drawing (title block, not the part) and an electronic copy of both the part and drawing. Save all your electronic files to a flash drive in case you need the files again. 4 : 3

4 Lab 2 Model Drawing & Dimensioning Bring a Ruler to Lab For this lab you will be given a model to draw in SolidWorks. Do not write on or place any marks on the models. You are to get all the dimensions to the nearest.05 inch or 1/16 inch using a standard ruler. The 2 letter 2 number part number (Drawing number) is on the front face of the model; i.e. that face is the front face of the part. Assume all corners are sharp and holes are round and all but one angle is 90, i.e. there are no fillets or rounds. There will be one model per person. Plan your modeling carefully before drawing. Do a hand drawing with the dimensions to help you plan. Decide where you want the origin to be. Decide what plane you will have to draw on first. Drawing the model is much easier if you plan your strategy in advance. Make sure all features are fully defined before extruding and rename all features after extruding. When you are finished with the part check it carefully to make sure it represents your model. Make any necessary adjustments to the part. Save the part as yourlastname2. (The extension SLDPRT is added automatically.) Open the landscape titleblock obtained from the server to get the title box. Immediately use Save AS to save it as yourlastname2. (The extension SLDDRW is again added automatically. Avoid using the default name suggested by SolidWorks as an improper extension will be added to the name.) Bring in your model drawing to get a three view drawing and add an isometric model view in the upper right. Place them so that they are properly aligned for the paper. Do not use too large a scale as that results in a cramped drawing; 1:2 should be used. (See page 2:10 for proper scale factors.) The three view drawings should show hidden lines while the isometric view does not. Remember that the dimensions must be in their own layer and be a different color from the part. Use a scale so that the dimensioned drawings are not cramped. Display the dimensions to two decimal places to match the tolerance. Bring you dimensions into drawing with no views selected. Most of the dimensions will be in the top view. Do not accept the default placements of the dimensions, but move them to the best locations to clearly show all details. The one angled part should have an acute angular dimension. The depth of the hole needs to be included. Use the hole callout tool for this dimensions. Find the positions for the dimensions where the extension lines cross the smallest amount of the body. The hole location lines have to cross the body, but most of the others can be placed so that they don t. Fill in the title box except for next assembly. The title is Prototype Model, the drawing # (part #) is what is written on your model front, and the material is #2 Pine. The tolerance is ±.03. Save the solid model as yourlastname2 and the drawing as yourlastname2. (SolidWorks adds the proper extensions.) Submit both a hard copy of the dimensioned drawing and the electronic copies of both files. Use the ThawSpace drive on the hard drive to save the files OFTEN as you work. It is much faster than trying to save to other media. When you have finished your session, go to the desktop and drag the files to your saving media. Do not try to use the Save As function in SolidWorks to save to disks. The failure rate is very high with this mode. You need both files - the SLDPRT and the SLDDRW - present to make changes so keep them together. They are coupled and changes in one will affect the other. It is best to do your transfer at the end to avoid cluttering your device with the temporary and journal files used by SolidWorks. Return the model and ruler before leaving lab as other sections will need to use them. 4 : 4

5 Typical Prototype Model for Laboratory 2 4 : 5

6 Lab 3A Mounting Bracket Dimensioning Bring a Ruler to Lab Use SolidWorks to draw a solid rendering of the mounting bracket shown on the next page. The scale of the standard three view drawing is 1:1 and the units are millimeters. Change the units of the part to millimeters before you begin drawing. All numbers should be to the nearest millimeter. (Be sure you are using millimeters and not centimeters. A centimeter is about the width of your little finger.) Use the angular measurement in creating the sloped edge on the back side of your part. You are to measure the views to obtain the dimensions of the part features. To save time in lab, you may want to do the measurements before coming to class and to rough out the dimension layout on the next page. The views shown are correct, so your part should match the views, i.e. front is front, etc. Save the bracket as yourlastname3. Transfer it to a landscape title block drawing sheet with metric units added. Again, make sure that your sheet units are set to millimeters before your start importing views. Even though your part might have been done in millimeters, your sheet still has to be set to millimeters to give the proper units. Use the hole callout tool to dimension the counterbore, remembering to delete the THRU. (<hwthru>) Use an acute angle dimension to specify the sloped edge. There are a lot of dimensions so you will have to take care positioning them in the proper views in the proper places. The slots should be dimensioned to their center marks to properly locate them, not their edges. Show the front, top and right views completely dimensioned. Include an isometric view. Also include centerlines on any full circle when necessary. Properly scale the drawing. Add your name, lab and lecture section, a title (Mounting Bracket), drawing number , the scale, material (2014 Aluminum Alloy), date and the tolerance (±1) to your title block. When you are done, make sure that your drawing looks like drawing on the next page. Save the file as yourlastname3. Submit the dimensioned three view drawing hard copy and the two files. 4 : 6

7 Laboratory 3A Bracket 4 : 7

8 Lab 3B Mounting Bracket Dimensioning Bring a Ruler to Lab Use SolidWorks to draw a solid rendering of the mounting bracket shown on the next page. The scale of the standard three view drawing is 1:1 and the units are millimeters. Change the units of the part to millimeters before you begin drawing. All numbers should be to the nearest millimeter. (Be sure you are using millimeters and not centimeters. A centimeter is about the width of your little finger.) Use the angular measurement in creating the sloped edge on the left side of your part. You are to measure the views to obtain the dimensions of the part features. To save time in lab, you may want to do the measurements before coming to class and to rough out the dimension layout on the next page. The views shown are correct, so your part should match the views, i.e. front is front, etc. Save the bracket as yourlastname3. Transfer it to a title block drawing sheet with metric units added. Again, make sure that your sheet units are set to millimeters before your start importing views. Even though your part might have been done in millimeters, your sheet still has to be set to millimeters to give the proper units. Show the front, top and right views completely dimensioned. The slots should be dimensioned to their center marks to properly locate them, not their edges. Include an isometric view. Also include centerlines on any full circle when necessary. Properly scale the drawing. Add your name, lab and lecture section, a title (Mounting Bracket), drawing number , the scale, material (3003 Aluminum Alloy), date and the tolerance (±1) to your title block. When you are done, make sure that your drawing looks like drawing on the next page. Save the file as yourlastname3. Submit the dimensioned three view drawing hard copy and the two files. 4 : 8

9 Laboratory 3B Bracket 4 : 9

10 Lab 4A Short Flange Section Drawing Shown on the next page is a half section isometric of a flange. Create this in SolidWorks. You are looking at the standard isometric view in the drawing (i.e. the top view is circular) so select a starting plane to replicate this view. Space probes have been lost due to drawings being backwards or in the wrong views! Get them right before you start. All needed dimensions are shown. Study the diagram for a while in order to become acquainted with the dimensions and where each goes. Part of this assignment is to properly interpret the diagram. Be sure to convert all necessary dimensions to diameters and dimension them from the centerline. (See lecture notes for proper dimensioning of concentric diameters.) Use a circular pattern to duplicate the holes after the first one was created by Hole Wizard. When you are satisfied with your solid part, transfer it over to a drawing with the top view as a named view. The drawing should be in portrait mode with a title block. Create a full section view following a diameter through a pair of the holes. Be sure your layer is set to none during the cutting. Make sure that your drawing looks reasonable before proceeding. Fully dimension the section view using a 10-point font and three decimal place accuracy. Your dimensions arrows should be.2 long with.1 tails. Include a tolerance of ±.005 inch. Scale your drawing appropriately. Call out the holes properly the notation in the sketch is not correct. Add center lines to the three holes in the section view, again making sure that they are in the none layer. After the dimensions are all inserted, turn off the dimension layer and place the following geometric dimension tolerances in another layer. The various referred surfaces are listed in the second drawing; surfaces 6 and 1 are treated as different surfaces. The numbers are not datum surfaces; they are only used to identify each surface. You have to assign datum letters in alphabetical order to the surfaces that require them. All GDT s will fit in the section view. Read the Style Sheet in this manual for how to place the GDT s. Surface 2 flat to.001 Surface 1 parallel to surface 2 to.002 Surface 7 perpendicular to surface 6 to.003 Surface 8 circular to.002 Surface 8 concentric to surface 4 to.002 Surface 4 cylindrical to.002 Surface 3 flat to.001 Surface 3 parallel to surface 2 to.002 Hole 5 perpendicular to surface 2 to.004 Surface 9 has an angularity to surface 1 to.005 Surface 7 circular to.002 In the title block type: your name, lab section, lecture section, title (Flange Section), date, drawing number (47FL024), next assembly (47FL012), material (brass) and scale. Print two copies of the drawing; one with only the coordinate dimensions showing and one with only the geometric dimensional tolerances showing and hand in. Save on your disk with the dimensions showing (turned on) and the GDT turned off. Your file name is yourlastname4 for both the part and the drawing. Submit both electronic files. 4 : 10

11 Lab 4 Short Flange Section Drawing Diagrams Surface Identification Diagrams for GDT 4 : 11

12 Lab 4B Tall Flange Section Drawing Shown on the next page is a half section isometric of a flange. Create this in SolidWorks. You are looking at the standard isometric view in the drawing (i.e. the top view is circular) so select a starting plane to replicate this view. Space probes have been lost due to drawings being backwards or in the wrong views! Get them right before you start. All needed dimensions are shown. Study the diagram for a while in order to become acquainted with the dimensions and where each goes. Part of this assignment is to properly interpret the diagram. Be sure to convert all necessary dimensions to diameters and dimension them from the centerline. (See lecture notes for proper dimensioning of concentric diameters.) Use a circular pattern to duplicate the holes after the first clearance hole was created by Hole Wizard. When you are satisfied with your solid part, transfer it over to a drawing with the top view as a named view. The drawing should be in portrait mode with a title block. Create a full section view following a diameter through a pair of the holes. Be sure your layer is set to none during the cutting. Also check that your drawing looks reasonable before proceeding. Fully dimension the section view using a 10-point font and three decimal place accuracy. Your dimensions arrows should be.2 long with.1 tails. Include a tolerance of ±.005 inch. Scale your drawing appropriately. Call out the holes properly the notation in the sketch is not correct. Add center lines to the three holes in the section view, again making sure that they are in the none layer. After the dimensions are all inserted, turn off the dimension layer and place the following geometric dimension tolerances in another layer. The various referred surfaces are listed in the second drawing; surfaces 6 and 1 are treated as different surfaces. The numbers are not datum surfaces; they are only used to identify each surface. You have to assign datum letters in alphabetical order to the surfaces that require them. All GDT s will fit in the section view. Read the Style Sheet in this manual for how to place the GDT s. Surface 2 flat to.001 Surface 1 parallel to surface 2 to.002 Surface 3 perpendicular to surface 10 to.003 Surface 3 cylindrical to.003 Surface 4 flat to.001 Surface 4 parallel to surface 1 to.002 Surface 5 circular to.004 Surface 12 circular to.004 Surface 8 angular to surface 1 to.006 Hole 6 perpendicular to surface 1 to.005 Surface 11 concentric to surface 3 to.004 Surface 11 perpendicular to surface 10 to.003 In the title block type: your name, lab section, lecture section, title (Flange Section), date, drawing number (57FL062), next assembly (57FL048), material (brass) and scale. Print two copies of the drawing; one with only the coordinate dimensions showing and one with only the geometric dimensional tolerances showing and hand in. Staple the coordinate dimensions drawing on top. Save on your disk with the dimensions showing (turned on) and the GDT turned off. Your file name is yourlastname4 for both the part and the drawing. Submit both electronic files. 4 : 12

13 Lab 4B Tall Flange Section Drawing Diagrams Surface Identification Diagrams for GDT 4 : 13

14 Lab 5A Metric Support Bracket Given the standard isometric sketch on the next page, create the metric part and bring it over to a standard three view drawing in landscape format. Use hole wizard and a linear pattern to create all the holes except for the large hole in the side. If you use hole wizard for the side hole you will not be able to add the necessary tolerances. You should not override any hole wizard values except for possibly the depth of the holes. There is a plane of symmetry so the origin must be somewhere on this plane. Include an auxiliary view and an isometric view on the drawing. Do not include a section view. Use a scale of 1:4. Fully dimension the detail drawing on a landscape title block. There are several errors in the dimensioning of the drawing (but not in the numbers) on the next page so do not just replicate what is there. You have to place the dimensions correctly and give the proper callouts. The units of the drawing are millimeters. Put your dimensions and GDT s in separate layers. Read the style sheet presented earlier in this manual to see how to present the information. Use the following information: 1. Use decimal dimensions with one decimal place unless otherwise noted on the drawing. Set the drawing to show the decimals by going to Tools: Options: Document Properties: Detailing: Trailing Zeros: Show. Include the special tolerances in the exact form as shown on the four dimension, i.e. limits, symmetric, bilateral, etc. Properly give the callouts for the counterbores, threaded holes and the blind positioning holes. Make sure the locating dimensions are put into the drawing for all the holes. Correct any other poor dimensioning practices in the sketch, there are several intentionally inserted in this sketch. 3. Include these GEOMETRIC TOLERANCES in a separate layer. (Label only the datums necessary for tolerancing. Use letters in alphabetical order, not numbers. The numbers in the lower drawing are for reference only and do not represent datum designations.) The control boxes and datums will not be able to be placed on the same views. Place all leaders on an edge not a face. The 65 degree angle (surfaces 11 and 2) must be "angular" within.06 to surface 8. (One leader will take care of both surfaces in the right view.) Surfaces 6 and 7 are parallel to 5 and 1 respectively by.02 (different reference datums). Surfaces 11 and 2 are flat to.01 The 20 mm diameter hole is positioned with respect to surfaces 1, 3 and 12 to.05. Surface 8 is perpendicular to 9 by.03. The blind clearance holes (non tapped) are circular to.06. Surface 4 is parallel to surface 9 to Fill in the title block in the drawing including: The material is Tool Steel L2. The title is Support Bracket. The part number is QRX3704. Next Assembly is ZDF Choose the appropriate tolerance for those dimensions not specified (see the style sheet). To get trailing zeros to show in metric views go to Tools: Options: Document Properties: Detailing. Change the selection for trailing zeroes from Smart to Show. Save your drawing as yourlastname5. Print two copies of the drawing; one with only the coordinate dimensions showing and one with only the geometric dimensional tolerances showing and hand in, stapled together with the coordinate dimension drawing on top. Save on your disk with the dimensions showing and the GDT turned off. Hand these in along with the part and the drawing on your disk. Reopen your files and recheck them before submitting them. Trimetric View of Support Bracket 4 : 14

15 Laboratory 5A Metric Support Bracket There are two symmetric counterbores for M12 Socket Head Cap Screw, 20 from the edges and 25 up from the bottom. The slot in the angled face is centered between the holes, not the face and is perpendicular to the face. The blind non-tapped holes are clearance holes for M10 rods. All fillets and rounds are 10 millimeters UOS. Holes on the angled faces are centered horizontally on the faces and are perpendicular to the faces. Balloon 12 is the back of the support, 5 the left side, 7 is left face of right projection, 8 is bottom of projection and 10 is bottom of main feature. 4 : 15

16 Lab 5B Support Bracket Given the standard isometric sketch on the next page, create the part and bring it over to a standard three view drawing in landscape format. Use hole wizard and a linear pattern to create all the holes except for the large hole in the side. If you use hole wizard for the side hole you will not be able to add the necessary tolerances. You should not override any hole wizard values except for possibly the depth of the holes. There is a plane of symmetry so the origin must be somewhere on this plane. Include an auxiliary view and an isometric view on the drawing. Do not include a section view. Use a scale of 1:4. Fully dimension the detail drawing. There are several errors in the dimensioning of the drawing (but not in the numbers) on the next page so do not just replicate what is there. You have to place the dimensions correctly and give the proper callouts. The units of the drawing are inches. Put your dimensions and GDT s in separate layers. Read the style sheet presented earlier in this manual to see how to present the information. Use the following information: 1. Use decimal dimensions with two decimal places unless otherwise noted on the drawing. Include the special tolerances in the exact form as shown on the three dimension, i.e. limits, symmetric, bilateral, etc. The side hole should be toleranced for an RC3 fit (+.0008) in unilateral format. 2. Properly give the callouts for the counterbores, threaded holes and the blind positioning holes. Make sure the locating dimensions are put into the drawing for all the holes. Correct any other poor dimensioning practices in the sketch, there are several intentionally inserted in this sketch. 3. Include these GEOMETRIC TOLERANCES in a separate layer. (Label only the datums necessary for tolerancing. Use letters in alphabetical order, not numbers. The numbers in the lower drawing are for reference only and do not represent datum designations.) The control boxes and datums will not be able to be placed on the same views. Place all leaders on an edge not a face. The 65 degree angle (surfaces 11 and 2) must be "angular" within.006 to 4 : 16 surface 8. (One leader will take care of both surfaces in the right view.) Surfaces 6 and 7 are parallel to 5 and 1 respectively by.002 (different reference datums). Surfaces 11 and 2 are flat to.001 The.750 diameter hole is positioned with respect to surfaces 1, 3 and 12 to.005. Surface 8 is perpendicular to 9 by.002. The blind clearance holes (non tapped) are circular to.004. Surface 4 is parallel to surface 9 to Fill in the title block in the drawing. The material is Tool Steel L2. The title is Support Bracket. The part number is QRX Next Assembly is ZDF Choose the appropriate tolerance for those dimensions not specified (see the style sheet). Save your drawing as yourlastname5. Print two copies of the drawing; one with only the coordinate dimensions showing and one with only the geometric dimensional tolerances showing and hand in, stapled together with the coordinate dimension drawing on top. Save on your disk with the dimensions showing and the GDT turned off. Hand these in along with the part and the drawing on your disk. Reopen your files and recheck them before submitting them. Trimetric View of Support Bracket

17 Laboratory 5B Support Bracket There are two symmetric counterbores for 1/2 Socket Head Cap Screw,.75 from the edges and 1.0 up from the bottom. The slot in the angled face is centered between the holes, not the face and is perpendicular to the face. The blind non-tapped holes are clearance holes for 3/8 rods. All fillets and rounds are.4 inches UOS. Holes on the angled faces are centered horizontally on the faces and are perpendicular to the faces. Balloon 12 is the back of the support, 5 the left side, 7 is left face of right projection, 8 is bottom of projection and 10 is bottom of main feature. 4 : 17

18 Lab 6A Standard Flywheel For this lab, you are to replicate the flywheel as shown. Utilize the symmetries to minimize what has to be the base circle and extrude it up with a drawn. There is top/bottom symmetry, so just draw the top half and mirror about the middle. Start with 4 draft. Cut the well and extrude the central hub. Draw in one rib on the front plane with hidden lines showing. Since it is connecting to a circular face, use a revolve boss extrude 8º midplane. The rib should be positioned exactly as shown. Use the hole wizard to give a clearance hole for a 1/4 inch bolt. Find the proper clearance hole with the correct defaults. Do not change the default settings. Use one circular pattern tool to put the other four ribs and holes in. Use Hole Wizard for the central counterbore. A 1 inch heavy hex bolt gets you close. Override the defaults to get the proper dimensions. Then feature mirror the whole piece. Bring the part over to a portrait drawing. Show the top view and a full section front view (a full section is shown here) and an isometric view. The top, section and front must be aligned exactly as shown in the figure. Place the isometric wherever convenient. Completely dimension the flywheel. Do not just copy the dimensioning shown here the vertical dimensions are poorly chosen to describe the part fix them. Use hole callout to dimension the clearance holes and counterbore in the top view. The material is cast iron, the tolerance is ±.01, next assembly is 152CQ17 and part number is 152CI2901. Submit the hard copy of the drawing and the electronic copies of both the part and drawing. Label the files yourlastname6a. Solid works will add the proper extensions. 4 : 18

19 Lab 6B Tapered Flywheel For this lab, you are to replicate the flywheel as shown. Utilize the symmetries to minimize what has to be drawn. There is top/bottom symmetry, thus, just draw the top half and mirror about the middle. Start with the base circle on the top plane and extrude it up with a 6 draft; do not use a revolved extrude. Cut the well on the top face of the base with a draft angle of 6. Verify that the draft is in the proper direction before proceeding. In the bottom of the well sketch the center hub and extrude up with a 6 draft again. Draw in one rib on the front plane with hidden lines visible utilizing the convert entities and trim tools. Set the trim tool to Trim to Closest before trimming. Since the rib is connecting to circular faces, use a revolve boss extrude midplane and 6º (include a center line for the extrusion.) The rib should be positioned exactly as shown on the left hand side of the flywheel. Use the Hole Wizard to give a clearance hole for a 3/8 inch bolt. Find the proper clearance hole with the correct defaults. Do not change the default settings. Use one circular pattern tool to put the other eight ribs and holes in. Use Hole Wizard for the central counterbore. Since this counter bore is for holding a bearing rater than a standard fastener a dimensional override will be necessary. A 1 inch heavy hex bolt gets you close. Override the defaults to get the proper dimensions. Then feature mirror the whole piece. Feel free to inspect the model of the flywheel in the lab to help you understand the part. Bring the part over to a portrait drawing. Show the top view, a full section (a full section is shown here) of the front view and an isometric view. The top and section must be aligned exactly as shown in the figure. Place the isometric wherever convenient. Completely dimension the flywheel. Do not just copy the dimensioning shown here the vertical dimensions are poorly chosen to describe the part fix them. These were placed in the description to facilitate the use of the mirror command, but someone casting this will need full dimensions. Use hole callout to dimension the clearance holes and counterbore in the top view. The form of one of the callouts in the drawing is the outdated method. Correct it to be the current style. Add the geometric tolerance in the same display as the dimensions since there is only one, but remember to keep it in its own layer. The material is cast iron, the tolerance is ±.01, next assembly is 152CQ17 and part number is 152CI2901. Submit the hard copy of the drawing and the electronic copies of both the part and drawing. Label the files yourlastname6b. SolidWorks will add the proper extensions. 4 : 19

20 Lab 6B Tapered Flywheel 4 : 20

21 Lab6C Elliptical Bottle Create the bottle shown below in SolidWorks using the shell feature to hollow it out. The wall thickness is.25 inch. Create the main bottle first. The main shape of the bottle is an ellipse. To create an ellipse go to Tools : Sketch Entities and select the ellipse. Click in the sketch where you want the origin to be and then drag to the right to set the semi-major axis. Click again on the origin and drag up to set the semi-minor axis. With smart dimensions dimension the full major axis length and the full minor axis length. Use a relation to make the right vertex horizontal with the origin. Keep the origin on the central axis. The transition to the neck should be made using a loft feature note that the neck is circular. Fillet all three edges with a.5 inch radius. After the rounding, apply the shell command to the top plane of the mouth. Finally apply a round to the top face of the neck. Bring the right view to a landscape drawing with a title block. Show the right view, a full section front view and an isometric view (as shown below). The isometric view should be displayed with Tangent Edges with font on. Select the drawing, right click on the green border, choose Tangent Edges and then the proper selection. Do not dimension the drawing. Fill in the title block leaving the Tolerance, Next Assembly and Material blank. The part number is CPBC2704. Submit a hard copy of the drawing and the two electronic files. Name your files YourLastName6C and staple the hard copy to the flywheel with the flywheel sheet on top. 4 : 21

22 Lab6D Rectangular Bottle Create the bottle shown below in SolidWorks using the shell feature to hollow it out. The wall thickness is.1 inch. Create the main bottle first. Keep the origin on the central axis. The neck should be made using a loft feature. Before adding the mouth, fillet all faces with a.25 inch radius. Extrude on the mouth and fillet the joint between the mouth and neck to.1 inch. The last thing to do is to apply the shell command to the top plane of the mouth. Bring the right view to a landscape drawing with a title block. Show the right view, a full section front view and an isometric view. The isometric view should be displayed with Tangent Edges with font on. Select the drawing, right click on the green border, choose Tangent Edges and then the proper selection. Do not dimension the drawing. Fill in the title block leaving the Tolerance, Next Assy and Material blank. The part number is CPBC2704. Submit a hard copy of the drawing and the two electronic files. Name your files YourLastName6D and staple the hard copy to the flywheel with the flywheel sheet on top. 4 : 22

23 Lab7A Bowl Assembly Bring Text Book to Lab Do three part drawings of the bowl, lid and fastener. The shell command must be used to create the insides of the bowl and cover. Use the Hole Wizard to create the counter sink clearance hole and the tapped blind hole. (See the Hole Wizard write up in chapter 2. Use the tables in the text book to determine all the relevant dimensions for the screw. (If more than one size is given use the minimum dimension.) A rotational extrude should be used for the screw. The head height is not to be used. The screw and tapped hole should have cosmetic threads. Assemble the parts in an assembly drawing, completely mate all the parts (6 mates) and then show them in an exploded view. The explosion should be large enough to see the top of the bottom center post. Transfer the assembly to a landscape drawing with a title block and bill of materials. The part numbers are 721BA7A, 721BA7B and 721BA7C. The names of the parts are bowl bottom, bowl cover and screw fastener respectively in order of importance. The drawing number is 721FA723 and the title is Bowl Assembly. There is no material, next assembly nor tolerance. Name the files yourlastname7a, B, C, D and E. Submit a printout of the assembly drawing with title block filled in and the five files on disk. 4 : 23

24 Lab7B Box Assembly Bring Text Book to Lab Do three part drawings of the box, cover and fastener. The shell command must be used to create the insides of the bowl and cover. Use the Hole Wizard to create the counter sink clearance hole and the tapped blind hole. (See the Hole Wizard write up in chapter 2 to get the proper selections for the tapped holes.) Due to the diagonal nature of the holes it is easiest to use Hole Wizard twice rather than a linear pattern for the second hole. To position the tapped holes make them concentric with the edges of the peg they are in. Use the tables in the text book to determine all the relevant dimensions for the screw. (If more than one size is given use the minimum dimension.) A rotational extrude should be used for the screw. The head height is not to be used. The screw and tapped hole should have cosmetic threads. Assemble the parts in an assembly drawing, completely mate all the parts (9 mates) and then show them in an exploded view. The explosion should be large enough to see the top of the bottom posts. Transfer the assembly to a landscape drawing with a title block and bill of materials. The part numbers are 175BX254, 175BX268 and 175BX524. The names of the parts are box bottom, box cover and screw fastener respectively in order of importance. The drawing number is 175BX986 and the title is Box Assembly. There is no material, next assembly nor tolerance. Name the files yourlastname7a, B, C, D and E. Submit a printout of the assembly drawing with title block filled in and the five files on disk. 4 : 24

25 Assembled Box Dimensions 4 : 25

26 Laboratory 8A Piston Assembly You will be making a dynamic assembly of a piston in a cylinder or since everything is rectangular this arrangement is often called a slider-crank. For this laboratory you are to create four parts, a cylinder unit, piston (slider), a crank and a connecting rod. The connecting rod will be 3 inches long and the crank arm 1 inch. If done carefully, all you will need to do is to change the length dimension to get one from the other. All the dimensions are given on the next page. When the parts are finished, bring them into a working assembly. When the crank is rotated, the piston will be moved back and forth. If you pick the wrong mates, the assembly will not move. You will need 7 mates. Bring the unexploded assembly into a dimetric view in the drawing with a title block and bill of materials. The diametric view is used since all the parts are visible in this view. The part numbers are SC2801 thru SC2804 with names of cylinder, piston, crank and connecting rod in order of importance. Complete the title block and turn in the hard copy. The Drawing number is SC5925 and the Title is Cylinder - Piston. You will need to turn in six electronic files the four parts, the assembly and the assembly drawing. Name them yourlastname8a through 8F. Name the files properly when you create them as the names may not be changed once the assembly is started. Dimetric View of Piston in Cylinder 4 : 26

27 4 : 27

28 Laboratory 8B Slider Crank For this laboratory you are to create four parts, a base unit, slider a crank and a connector arm. The conning arm will be 8 inches long and the crank arm 3 inches. If done carefully, all you will need to do is to change the length dimension to get one from the other. When they are finished, bring them into a working assembly. When the crank is rotated, the slider will be moved back and forth. If you pick the wrong mates, the assembly will not move. You will need 7 mates. Bring the unexploded assembly into an isometric view in the drawing with a title block and bill of materials. The part numbers are 152SC801 thru 152SC804 with names of base, slider, crank and connecting rod in order of importance. Complete the title block and turn in the hard copy. The Drawing number is 152SC925 and the Title is Slider Crank. You will need to turn in six electronic files the four parts, the assembly and the assembly drawing. Name them yourlastname8a through 8F. Name the files properly when you create them as the names may not be changed once the assembly is started. Slider Crank Mechanism Slider Base Support Crank Arm You need a 3 inch crank arm and an 8 inch connecting arm 4 : 28

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