Engineering Innovation Center Fabrication Shop Basic CAD Training
Introduction The Engineering Innovation Center Fabrication Shop was established for support of undergraduate student course work. Every effort will be made to make the shop available for these projects. Students of Engineering who desire to use this equipment for educationally-related activities are required to attend training. 8/30/2016 Engineering Innovation Center 2
Overview All images and instructions pertain to SolidWorks 2015 Creation of part Fully defined sketches Extrusions Features Drawing Dimensions Hole Callouts Section Views Expectations for Fabrication 8/30/2016 Engineering Innovation Center 3
Begin Start up SolidWorks Start a new Part File Make sure you are working in Inches In the bottom right-hand corner it should say IPS If not click on MMGS and change it to IPS Alternatively you can go to Options>Document Properties>Units and select IPS 8/30/2016 Engineering Innovation Center 4
Navigation Rotation, orbiting, panning and general movement can be controlled by the mouse in combination with the keyboard To pan simply hold control and middle click To orbit hold middle click and move the mouse To see standard views press spacebar and select a view If at any time your model disappears press f to fit the model to the workspace 8/30/2016 Engineering Innovation Center 5
Sketches The basis for any part Should always be fully defined before moving on Should be referenced to origin Relations/Constraints further define sketch geometry Under Defined Sketch Fully Defined Sketch 8/30/2016 Engineering Innovation Center 6
Create a Sketch Start a Sketch Pick a plane Start at origin 8/30/2016 Engineering Innovation Center 7
Dimension/Constrain Dimensions and constraints define sketches Use the Smart Dimension tool to Define length, angle, radius or diameter. Relations/Constraints further define sketches Note: To constrain multiple entities hold control as you select them 8/30/2016 Engineering Innovation Center 8
Replicate This Sketch Construction lines are not crucial Make sure fully defined before moving on If not fully defined check relationship to origin or relations between lines To change between units click on IPS or MMGS in bottom right-hand corner 8/30/2016 Engineering Innovation Center 9
Extrude Extrusions make a 2D sketch into a 3D model Select the extrude command Pick sketch profile and extrude to 2.270 inches 8/30/2016 Engineering Innovation Center 10
Design Tree Organization Organization helps with future editing or modifying of features Good CAD practice is to descriptively rename everything To rename a feature simply double click on it in the design tree Here the extrusion has been renamed MainBody This will allow anyone collaborating on the design to easily recognize which operation was used to create the part 8/30/2016 Engineering Innovation Center 11
Hole Wizard Allows you to create: Slots Counterbores/Countersinks Threaded(Tapped) Holes Complex Holes Tapered Tap Holes Hole locations easily defined by sketches Allows hole callouts within drawings to be done with one click 8/30/2016 Engineering Innovation Center 12
Sketch Defined Hole Locations Start a sketch on this plane Dimension sketch points to define hole locations Note: Points have been constrained to be horizontal/vertical 8/30/2016 Engineering Innovation Center 13
Hole Wizard Parameters Start the Hole Wizard Select Positions The Position operation will require a plane or face to start the hole at Select the plane that we sketched on If your sketch is not visible right click on it in the design tree within the workspace and make it visible 8/30/2016 Engineering Innovation Center 14
Placing Holes Its as easy as point and click Simply pick each of the sketch points previously defined At this point and time the holes might not look how you want them. Switch back over to the type tab on the left hand side Notice the sketch points are black indicating that the hole locations are fully defined 8/30/2016 Engineering Innovation Center 15
Hole Definition The holes on this particular part are classified as #8-32 UNC This means that the holes will be tapped or threaded Select the Straight Tapped Hole Using the drop downs select the specified thread classification End conditions can be modified under the End Condition tab Set end condition to Through All 8/30/2016 Engineering Innovation Center 16
Center Holes Replicate this sketch of two points on the uppermost surface of the solid Dimension them to be.325in apart Check if fully defined If not fully defined constrain the left point to the origin and both points to be parallel 8/30/2016 Engineering Innovation Center 17
Center Holes Now, using HoleWizard, create a #8-32 tapped hole that extends thru all 8/30/2016 Engineering Innovation Center 18
Center Holes (Reamed) In a similar fashion create a straight hole that is reamed to.2495in This is accomplished by selecting the hole function. Then, using standard drill sizes, select 1/4in and check the show custom sizing box 8/30/2016 Engineering Innovation Center 19
Circular Pattern To make creating a circular pattern easier we will turn on axes Click the glasses dropdown at the top of the workspace Select the view temporary axes icon Hover mouse over options to see what they are Click the linear pattern dropdown under the feature tab Select Circular Pattern 8/30/2016 Engineering Innovation Center 20
Circular Pattern Parameters We are going to create a circular pattern of the center #8-32 tapped hole We have already defined the radius of the pattern in the starting sketch Under the Features and Faces make sure the #8-32 hole is selected In the first box you need an axis or circular feature to revolve around Select the axis of the reamed hole Make sure the equal spacing check box is selected Set the pattern amount to 3 8/30/2016 Engineering Innovation Center 21
Result This is the finished model ready to be inserted into a mechanical drawing 8/30/2016 Engineering Innovation Center 22
Drawings Drawings allow you to communicate the features of your model to: The public Machinists Investors Anyone After creating your model select the new dropdown and click create new drawing from part/assembly Always use A(ANSI) landscape 8/30/2016 Engineering Innovation Center 23
Placing Views Paste views into the drawing workspace by clicking and dragging them from the right-hand side Arrange a descriptive view as the parent model view Drag and click to any side to place projected views 8/30/2016 Engineering Innovation Center 24
Arranging Views Arrange views by dragging Placed views will move according to the parent view with the exception of isometric views Scale can be adjusted on the left-hand side while a view is selected Views should be arranged in an esthetically pleasing way Delete the initial hole callouts in order to place more descriptive ones Dimensions and annotations can be added in a similar fashion to dimensions in the modeling environment Within the drawing using the dimension tool will not change the dimension but rather display the previously defined dimension 8/30/2016 Engineering Innovation Center 25
Drawing Practices Even if you prefer to model in millimeters/centimeters always complete drawings in inches Place dimensions between views as much as possible Avoid crossing lines Pick a reference edge and try to stick to it Include all needed dimensions Your part should be able to be created without the need for a solid model (using just the drawing) 8/30/2016 Engineering Innovation Center 26
Title Block The title block is all of the information in the lower portion of the page Title block can be edited by right clicking on white space and selecting edit sheet format Drawing number should not be part description, it should include information for reference eg. (ENGR112_01) Your name goes on the uppermost line above drawing title Material, Finish and Tolerances are crucial pieces of information DO NOT FORGET THEM! When finished editing the title block return to the drawing view by clicking the icon in the top right-hand corner of the workspace 8/30/2016 Engineering Innovation Center 27
Practice Recreate this drawing 8/30/2016 Engineering Innovation Center 28
Extra Resources Solidworks https://www.youtube.com/channel/uctwawpoxebyszlh1 rrpzwfw https://www.youtube.com/user/innovasystemsuk Autodesk https://www.youtube.com/user/autodeskmfg https://www.youtube.com/user/autodeskfusion360 https://www.youtube.com/user/autocadexchange 8/30/2016 Engineering Innovation Center 29
Conclusion Unsafe practice or obvious abuse of equipment constitutes a danger to people and damages equipment. Therefore the Fabrication Shop Manager or any person observing an unsafe act should stop unsafe practices in the Fabrication Shop. Students violating any of these rules will have their Fabrication Shop privileges revoked for a period of at least two weeks. Longer periods may be assessed, depending upon the judgment of the Fabrication Shop Manager and the Engineering Innovation Center Facility Manager. 8/30/2016 Engineering Innovation Center 30