Parametric Modeling With Creo Parametric 5 - SDC Publications
Parametric Modeling withCreo Parametric 5.0 An Introduction to Creo Parametric 5.0 Randy H. ShihSDCP U B L I C AT I O N SBetter Textbooks. Lower Prices.www.SDCpublications.com
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Parametric Modeling with Creo ParametricChapter 1Parametric Modeling Fundamentals Create Simple Extruded Solid Models Understand the Basic ParametricModeling Process Create 2D Sketches Understand the "Shape before Size"approach Use the Dynamic Viewing commands Create and Modify ParametricDimensions1-1
1-2Parametric Modeling with Creo ParametricIntroductionThe feature-based parametric modeling technique enables the designer to incorporatethe original design intent into the construction of the model. The word parametric meansthe geometric definitions of the design, such as dimensions, can be varied at any time inthe design process. Parametric modeling is accomplished by identifying and creating thekey features of the design with the aid of computer software. The design variables,described in the sketches and features, can be used to quickly modify/update the design.In Creo Parametric, the parametric part modeling process involves the following steps:1. Set up Units and Basic Datum Geometry.2. Determine the type of the base feature, the first solid feature, of the design.Note that Extrude, Revolve, or Sweep operations are the most commontypes of base features.3. Create a rough two-dimensional sketch of the basic shape of the base featureof the design.4. Apply/modify constraints and dimensions to the two-dimensional sketch.5. Transform the two-dimensional parametric sketch into a 3D feature.6. Add additional parametric features by identifying feature relations andcomplete the design.7. Perform analyses/simulations, such as finite element analysis (FEA) or cutterpath generation (CNC), on the computer model and refine the design asneeded.8. Document the design by creating the desired 2D/3D drawings.The approach of creating three-dimensional features using two-dimensional sketches isan effective way to construct solid models. Many designs are in fact the same shape inone direction. Computer input and output devices we use today are largely twodimensional in nature, which makes this modeling technique quite practical. This methodalso conforms to the design process that helps the designer with conceptual design alongwith the capability to capture the design intent. Most engineers and designers can relateto the experience of making rough sketches on restaurant napkins to convey conceptualdesign ideas. Note that Creo Parametric provides many powerful modeling and designtools, and there are many different approaches to accomplish modeling tasks. The basicprinciple of feature-based modeling is to build models by adding simple features one ata time. In this chapter, a very simple solid model with extruded features is used tointroduce the general feature-based parametric modeling procedure.
Parametric Modeling Fundamentals1-3The Adjuster designStarting Creo ParametricHow to start Creo Parametric depends on the type of workstation and the particularsoftware configuration you are using. With most Windows and UNIX systems, you mayselect Creo Parametric on the Start menu or select the Creo Parametric icon on thedesktop. Consult your instructor or technical support personnel if you have difficultystarting the software.1. Select the Creo Parametric option on the Start menu or select the CreoParametric icon on the desktop to start Creo Parametric. The Creo Parametricmain window will appear on the screen.2. Click on the New icon, located in the Ribbon toolbar asshown.
1-4Parametric Modeling with Creo Parametric3. In the New dialog box, confirm the model’s Type is set to Part (Solid Sub-type).4. Enter Adjuster as the part Name asshown in the figure.5. Turn off the Use default templateoption.6. Click on the OK button to accept thesettings.7. In the New File Options dialog box,select EMPTY in the option list to notuse any template file.8. Click on the OK button to accept thesettings and enter the Creo ParametricPart Modeling mode. Note that the part name, Adjuster.prt,appears in the Navigator Model Treewindow and the title bar area of the mainwindow.
Parametric Modeling Fundamentals1-5Step 1: Units and Basic Datum Geometry Setups Units SetupWhen starting a new model, the first thing we should do is to choose the set of unitswe want to use.1. Pick File1. Use the left-mouse-buttonand select File in the pulldown menu area.2. Use the left-mouse-buttonand select Prepare in thepull-down list as shown.3. Select Model Propertiesin the expanded list asshown.2. Pick Prepare Note that the Creo Parametric menu system is context-sensitive, which means thatthe menu items and icons of the non-applicable options are grayed out (temporarilydisabled).4. Select the Change option that is to the right of the Units option in the ModelProperties window.
1-6Parametric Modeling with Creo Parametric5. In the Units Manager – Systems of Unitsform, the Creo Parametric default setting Inchlbm Second is displayed. The set of units isstored with the model file when you save. PickInch Pound Second (IPS) by clicking inthe list window as shown.6. Click on the Set button to accept the selection. Notice the arrow in the Units list nowpoints toward the Inch Pound Second (IPS) units set.7. In the Changing Model Units dialogbox, click on the OK button toaccept the default option to changethe units. Note that Creo Parametric allows usto change model units even after themodel has been constructed; we canchange the units by (1) Convertdimensions or (2) Interpretdimensions.8. Click on the Close button to exit the Units Manager dialog box.9. Pick Close to exit the Model Properties window.
Parametric Modeling Fundamentals1-7 Adding the First Part Features – Datum Planes Creo Parametric provides many powerful tools for model creation. In doing featurebased parametric modeling, it is a good practice to establish three reference planes tolocate the part in space. The reference planes can be used as location references infeature constructions.1. Move the cursor to the Datumtoolbar on the Ribbon toolbar andclick on the Datum Plane tool iconas shown.Datum planes In the Navigator Model Tree window and the displayarea, three datum planes represented by three rectanglesare displayed. Datum planes are infinite planes and theyare perpendicular to each other. We can consider theseplanes as XY, YZ, and ZX planes of a Cartesiancoordinate system.2. Click the model name, Adjuster.prt, in the Navigatorwindow to deselect the last created feature.
1-8Parametric Modeling with Creo Parametric Switching On/Off the Plane Tag Display1. Click on the View tab in the Ribbon toolbarto show the view related commands in Creo.2. Click on the Plane Tag Displayicon to toggle on/off the display ofthe plane tag. Note the other options available todisplay the Axis Tag and/or PointTag. On your own, experimentwith turning on/off thePlane Tag; set the datumplanes to display with theassociated names as shownbefore proceeding to thenext section.3. Click on the Model tab in the Ribbontoolbar to return to the Model toolbar asshown.
Parametric Modeling Fundamentals1-9Step 2: Determine/Set up the Base Solid Feature For the Adjuster design, we will create an extruded solid as the base feature.1. In the Shapes toolbar (the fourthgroup in the Ribbon toolbar), clickon the Extrude tool icon as shown. The Feature Option Dashboard, which contains applicable construction options, isdisplayed in the Ribbon toolbar of the Creo Parametric main window.2. On your own, move the cursor over theicons and read the descriptions of thedifferent options available. Note that thedefault extrude option is set to Extrude assolid.3. Click the Placement option andchoose Define to begin creating a newinternal sketch.
1-10Parametric Modeling with Creo ParametricSketching plane – It is an XY CRT, but an XYZ WorldDesign modeling software is becoming morepowerful and user friendly, yet the system stilldoes only what the user tells it to do. Whenusing a geometric modeler, we therefore needto have a good understanding of what itsinherent limitations are. We should also havea good understanding of what we want to doand what to expect, as the results are based onwhat is available.In most 3D geometric modelers, 3D objectsare located and defined in what is usuallycalled world space or global space. Althougha number of different coordinate systems canbe used to create and manipulate objects in a3D modeling system, the objects are typicallydefined and stored using the world space. Theworld space is usually a 3D Cartesiancoordinate system that the user cannotchange or manipulate.In most engineering designs, models can be very complex, and it would be tedious andconfusing if only the world coordinate system were available. Practical 3D modelingsystems allow the user to define Local Coordinate Systems (LCS) or User CoordinateSystems (UCS) relative to the world coordinate system. Once a local coordinate systemis defined, we can then create geometry in terms of this more convenient system.Although objects are created and stored in 3D space coordinates, most of the geometricentities can be referenced using 2D Cartesian coordinate systems. Typical input devicessuch as a mouse or digitizer are two-dimensional by nature; the movement of the inputdevice is interpreted by the system in a planar sense. The same limitation is true ofcommon output devices, such as CRT displays and plotters. The modeling softwareperforms a series of three-dimensional to two-dimensional transformations to correctlyproject 3D objects onto the 2D display plane.The Creo Parametric sketching plane is a special construction approach that enables theplanar nature of the 2D input devices to be directly mapped into the 3D coordinatesystem. The sketching plane is a local coordinate system that can be aligned to anexisting face of a part or a reference plane.Think of the sketching plane as the surface on which we can sketch the 2D sections of theparts. It is similar to a piece of paper, a white board, or a chalkboard that can be attachedto any planar surface. The first sketch we create is usually drawn on one of theestablished datum planes. Subsequent sketches/features can then be created on sketchingplanes that are aligned to existing planar faces of the solid part or datum planes.
Parametric Modeling Fundamentals1-11Defining the Sketching PlaneThe sketching plane is a reference location where two-dimensional sketches are created.The sketching plane can be any planar part surface or datum plane. Note that CreoParametric uses a two-step approach in setting up the selection and alignment of thesketching plane. In the Section Placement window, theselection of the sketch plane and theorientation of the sketching plane areorganized into two groups as shown in thefigure. The Sketch Plane can be set toany surfaces, including datum planes. TheSketch Orientation is set based on theselection of the Sketch plane.1. Notice the Plane option box in theSketch window is activated, and themessage “Select a plane or surface todefine sketch plane.” is displayed inthe quick help tip and also in themessage area.2. In the graphic area, selectDTM2 by clicking on anyedge of the plane as shown. Notice an arrow appears onthe left edge of DTM2.The arrow directionindicates the viewingaligned direction of thesketch plane. The viewingdirection can be reversedby clicking on the Flipbutton in the SketchOrientation section of thepop-up window.
1-12Parametric Modeling with Creo ParametricDefining the Orientation of the Sketching PlaneAlthough we have selected the sketching plane, Creo Parametric still needs additionalinformation to define the orientation of the sketch plane. Creo Parametric expects us tochoose a reference plane (any plane that is perpendicular to the selected sketch plane) andthe orientation of the reference plane is relative to the computer screen. To define the orientation of the sketching plane, select the facingdirection of the reference plane with respect to the computer screen.The selected sketching plane,DTM2, will be aligned parallelto the 2D computer screen.We will orient the sketchingplane by setting the positiveside of DTM3 to face towardthe bottom edge of thecomputer screen.1. Notice the Reference option box inthe Sketch Orientation window isnow activated. The message “Selecta reference, such as surface, plane oredge to define view orientation.” isdisplayed in the message area.2. In the graphic area, select DTM3 byclicking on one of the datum planeedges as shown in the above figure.3. In the Orientation list, pickBottom to set the orientation of thereference plane.
Parametric Modeling Fundamentals1-134. Pick Sketch to exit the Section Placement window and proceed toenter the Creo Parametric Sketcher mode.5. To orient the sketching plane parallel to the screen, the Sketch View icon in theDisplay View toolbar is available as shown. Note the orientation of the sketchingplane is adjusted based on the setup on the previous page. Creo Parametric will now rotate the three datum planes: DTM2 aligned to the screenand the positive side of DTM3 facing toward the bottom edge of the computer screen. The orientation of the sketching plane can be very confusing to new users. Readthrough this section carefully again to make sure you understand the steps involved.
1-14Parametric Modeling with Creo ParametricStep 3: Creating 2D Rough Sketches Shape Before Size – Creating Rough SketchesQuite often during the early design stage, the shape of a design may not have any precisedimensions. Most conventional CAD systems require the user to input the precise lengthsand location dimensions of all geometric entities defining the design, and some of thevalues may not be available during the early design stage. With parametric modeling, wecan use the computer to elaborate and formulate the design idea further during the initialdesign stage. With Creo Parametric, we can use the computer as an electronic sketchpadto help us concentrate on the formulation of forms and shapes for the design. Thisapproach is the main advantage of parametric modeling over conventional solidmodeling techniques.As the name implies, rough sketches are not precise at all. When sketching, we simplysketch the geometry so it closely resembles the desired shape. Precise scale or dimensionsare not needed. Creo Parametric provides us with many tools to assist in finalizingsketches, known as sections. For example, geometric entities such as horizontal andvertical lines are set automatically. However, if the rough sketches are poor, much morework will be required to generate the desired parametric sketches. Here are some generalguidelines for creating sketches in Creo Parametric: Create a sketch that is proportional to the desired shape. Concentrate on theshapes and forms of the design. Keep the sketches simple. Leave out small geometry features such as fillets, rounds,and chamfers. They can easily be placed using the Fillet and Chamfer commandsafter the parametric sketches have been established. Exaggerate the geometric features of the desired shape. For example, if thedesired angle is 85 degrees, create an angle that is 50 or 60 degrees. Otherwise, CreoParametric might assume the intended angle to be a 90-degree angle. Draw the geometry so that it does not overlap. The sketched geometry shouldeventually form a closed region. Self-intersecting geometric shapes are not allowed. The sketched geometric entities should form a closed region. To create a solidfeature, such as an extruded solid, a closed region section is required so that theextruded solid forms a 3D volume. Note: The concepts and principles involved in parametric modeling are verydifferent, and sometimes they are totally opposite, to those of the conventionalcomputer aided drafting systems. In order to understand and fully utilize CreoParametric’s functionality, it will be helpful to take a Zen approach to learning thetopics presented in this text: Temporarily forget your knowledge and experiencesusing conventional computer aided drafting systems.
Parametric Modeling Fundamentals1-15 The Creo Parametric SKETCHER and INTENT MANAGERIn previous generation CAD programs, construction of models relies on exactdimensional values, and adjustments to dimensional values are quite difficult once themodel is built. With Creo Parametric, we can now treat the sketch as if it is being doneon a napkin, and it is the general shape of the design that we are more interested indefining. The Creo Parametric part model contains more than just the final geometry. Italso contains the design intent that governs what will happen when geometry changes.The design philosophy of “shape before size” is implemented through the use of theCreo Parametric Sketcher. This allows the designer to construct solid models in a higherlevel and leave all the geometric details to Creo Parametric.In Creo Parametric, previously known as Pro/ENGINEER, one of the more importantfunctionalities is the Intent Manager in the 2D Sketcher.The Intent Manager enables us to do: Dynamic dimensioning and constraintsAdd or delete constraints explicitlyUndo any Sketcher operationThe first thing that Creo Parametric Sketcher expects us to do, which is displayed in theReferences window, is to specify sketching references. In the previous sections, wecreated the three datum planes to help orient the model in 3D space. Now we need toorient the 2D sketch with respect to the three datum planes. At least two references arerequired to orient the sketch in the horizontal direction and in the vertical direction. Bydefault, the two planes (in our example, DTM1 and DTM3) that are perpendicular to thesketching plane (DTM2) are automatically selected. Note that DTM1 and DTM3 arepre-selected as the sketchingreferences. In the graphics area,the two references are displayedwith two dashed lines. In Creo Parametric, a 2D sketchneeds to be Fully Placed withrespect to at least tworeferences. In this case, DTM1 isused to control the horizontalplacement of geometry, whereDTM3 is used to control thevertical placements.
1-16Parametric Modeling with Creo Parametric Next, we will create a rough sketch by using some of the visual aids available, andthen update the design through the associated control parameters. Move the graphics cursor to the Lineicon in the Sketching toolbar. A helptip box appears next to the cursor toprovide a brief description of thecommand. The Sketching toolbar provides tools for creating the basic 2D geometry that can beused to create features and parts.Graphics Cursors Notice the cursor changes from an arrow to an arrowwith a small crosshair when graphical input isexpected.1. As you move the graphics cursor, you will seedifferent symbols appear at different locations.2. Move the cursor near the intersection of the tworeferences, and notice that the small crosshair attachedto the cursor will automatically snap to the intersectionpoint. Left-click once to place the starting point asshown. Notice the small geometric constraint symbolnext to the cursor; indicating the first line endpoint isCoincident with the intersection point.Constraint Symbols3. Move the cursor along the vertical reference andcreate a short horizontal line by clicking at a locationto the right side of the starting point as shown.Notice the geometric constraint symbol, a shorthorizontal line, indicating the created line segmentis Horizontal.
Parametric Modeling Fundamentals1-17Geometric Constraint SymbolsCreo Parametric displays different visual clues, or symbols, to show you alignments,perpendicularities, tangencies, etc. These constraints are used to capture the design intentby creating constraints where they are recognized. Creo Parametric displays thegoverning geometric rules as models are built.Verticalindicates a line segment is verticalHorizontalindicates a line segment is horizontalEqual Lengthindicates two line segments are of equal lengthEqual Radiiindicates two curves are of equal radiiTangentindicates two entities are tangent to each otherParallelindicates a segment is parallel to other entitiesPerpendicularindicates a segment is perpendicular to other entitiesSymmetryindicates two points are symmetricalPoint on Entityindicates the point is on another entityorPoint 3Point 1Point 21. Complete the sketch asshown, a closed regionending at the startingpoint (Point 1). Watch thedisplayed constraintsymbols while sketching,especially the EqualLength constraint, ,applied to the two shorthorizontal edges. Note that all segments areeither vertical orhorizontal.2. Inside the graphics area, click twice with the middle-mouse-button to end thecurrent line sketch.
1-18Parametric Modeling with Creo Parametric Creo Parametric’s Intent Manager automatically places dimensions and constraintson the sketched geometry. This is known as the Dynamic Dimensioning andConstraints feature. Constraints and dimensions are added “on the fly.” Do not beconcerned with the size of the sketched geometry or the displayed dimensionalvalues; we will modify the sketched geometry in the following sections.Dynamic Viewing FunctionsCreo Parametric provides a special user interface, Dynamic Viewing, which enablesconvenient viewing of the entities in the display area at any time. The Dynamic Viewingfunctions are controlled with the combinations of the middle mouse button, the [Ctrl] keyand the [Shift] key on the keyboard.Zooming – Turn the mouse wheel or [Ctrl] key and [middle-mouse-button]Use the mouse wheel to perform the zooming option; turning the wheelforward will reduce the scale of display. Hold down the [Ctrl] key and pressdown the middle-mouse-button in the display area. Drag the mouse verticallyon the screen to adjust the scale of the display. Moving upward will reduce thescale of the display, making the entities display smaller on the screen. Movingdownward will magnify the scale of the display.CtrlZoom Middle mouse buttonPanning – [Shift] key and [middle-mouse-button]Hold down the [Shift] key and press down the middle-mouse-button in thedisplay area. Drag the mouse to pan the display. This allows you to repositionthe display while maintaining the same scale factor of the display. Thisfunction acts as if you are using a video camera. You control the display bymoving the mouse.PanShift Middle mouse button On your own, use the Dynamic Viewing functions to reposition and magnify the scaleof the 2D sketch to the center of the screen so that it is easier to work with.
Parametric Modeling Fundamentals1-19Step 4: Apply/Modify Constraints and Dimensions As the sketch is made, Creo Parametric automatically applies geometric constraints(such as Horizontal, Vertical and Equal Length) and dimensions to the sketchedgeometry. We can continue to modify the geometry, apply additional constraintsand/or dimensions, or define/modify the size and location of the existing geometry. Itis more than likely that some of the automatically applied dimensions may not matchwith the design intent we have in mind. For example, we might want to havedimensions identifying the overall-height, overall-width, and the width of the insidecut of the design, as shown in the figures below.Current SketchSketch in mind
1-20Parametric Modeling with Creo Parametric1. Click on the Normal Dimension icon in theSketching toolbar as shown. This commandallows us to create defining dimensions.2. Select the inside horizontal line by leftclicking once on the line as shown.2. Pick the insidehorizontal line as thegeometry to dimension.3. Place the dimensionbelow the selected line.3. Move the graphics cursor below the selected line and click once with the middlemouse-button to place the dimension. (Note that the value displayed on your screenmight be different than what is shown in the above figure.)4. Click again with the middle-mouse-button to exit the Edit Dimension mode.5. Pick the right verticalline as the geometry todimension.6. Place the dimensiontoward the right side. 5. Select the right verticalline.6. Place the dimension, byclicking once with themiddle-mouse-button, ata location toward the rightof the sketch. The Dimension commandwill create a lengthdimension if a single lineis selected.Notice the overall-height dimension applied automatically by the Intent Manager isremoved as the new dimension is defined.
Parametric Modeling Fundamentals1-21 Note that the dimensions we just created are displayed with a different color thanthose that are applied automatically. The dimensions created by the Intent Managerare called weak dimensions, which can be replaced/deleted as we create specificdefining dimensions to satisfy our design intent.7. Select the top horizontal line as shown below.8. Select the inside horizontal line as shown below.9. Place the dimension, by clicking once with the middle-mouse-button, at a location inbetween the selected lines as shown below.7. Pick the top line as the1st geometry to dimension9. Place the dimensionin between the twoselected lines.8. Pick this line asthe 2nd geometry todimension10. Click again with the middle-mouse-button to exit the Edit Dimension mode. When two parallel linesare selected, theDimension commandwill create a dimensionmeasuring the distance inbetween. Examine the establisheddimensions andconstraints in the sketch.Is the sketch fullydefined? Or should weadd additionaldimensions?
1-22Parametric Modeling with Creo ParametricModifying the Dimensions in a Sketch1. Click on the Select icon in the Operationstoolbar as shown. The Select command allowsus to perform several modification operations onboth the sketched geometry and dimensions.2. Modify the overallheight-dimension.2. Select the overall height dimension ofthe sketch by double-clicking withthe left-mouse-button on thedimension text.3. In the dimension value box, thecurrent length of the line is displayed.Enter 3 as the new value for thedimension.4. Press the ENTER key once to acceptthe entered value. Creo Parametric will update the sketch using the entered dimension value. Since theother dimensions are much larger, the sketched shape becomes greatly distorted.5. Click on the Undo icon in the Quick Access toolbar to undo the Modify Dimensionperformed.
Parametric Modeling Fundamentals1-236. In the pull-down menu area, click on thedown-arrow on Select to display the optionlist and select the All option as shown.(Note that using the hotkey combinationCrtl Alt A can also activate this option.)7. In the Editing toolbar, clickon the Modify icon as shown. With the pre-selection option, all dimensions are selected and listed in the ModifyDimensions dialog box.8. Turn off the Regenerate option by unchecking the option in the Modify Dimensionsdialog box as shown.
1-24Parametric Modeling with Creo Parametric9. On your own, adjust the dimensions as shown below. Note that the dimensionselected in the Modify Dimensions dialog box is identified with an enclosed box in thedisplay area.10. Inside the Modify Dimensions dialog box, click on the OKbutton to regenerate the sketched geometry and exit theModify Dimensions command.Repositioning Dimensions1. Confirm the Select icon, in the Operationstoolbar, is activated as shown.2. Press and hold down the left-mouse-button onany dimension text, then drag the dimension to anew location in the display area. (Note the cursoris changed to a moving arrow icon during thisoperation.)
Parametric Modeling Fundamentals1-25Step 5: Completing the Base Solid Feature Now that the 2D sketch is completed, we will proceed to the next step: creating a 3Dpart from the 2D section. Extruding a 2D section is one of the common methods thatcan be used to create 3D parts. We can extrude planar faces along a path. In CreoParametric, the default extrusion direction is perpendicular to the selected sketchingplane, DTM2.1. In the Ribbon toolbar, click OK to exit the Creo Parametric2D Sketcher. The 2D sketch is the first element of the Extrudefeature definition.2. In the Feature Option Dashboard, confirm the depth value option is set as shown.This option sets the extrusion of the section by Extrude from sketch plane by aspecified depth value.3. In the depth value box, enter 2.5 as the extrusion depth.4. In the Dashboard area, click Accept toproceed with the creation of the solid feature.5. Use the hotkey combination CTRL D to resetthe display to the default 3D orientation. Note that all dimensions disappeared from the screen. All parametric definitions arestored in the Creo Parametric database, and any of the parametric definitions can bedisplayed and edited at any time.
1-26Parametric Modeling with Creo ParametricThe Third Dynamic Viewing Function3D Dynamic Rotation – [middle mouse button]Press down the middle-mouse-button in the display area. Drag the mouse onthe screen to rotate the model about the screen.Middle mouse button3D Rotation On your own, practice the use of the Dynamic Viewing functions; note thatthese are convenient viewing functions at any time.ZoomMouse WheelZoomCtrl Middle mouse buttonPanShift Middle mouse button
Parametric Modeling Fundamentals1-27Display Modes: Wireframe, Shaded, Hidden Edge, No HiddenThe display in the graphics window has six display modes: Shading with Edges,Shading with Reflections, Shading, No Hidden lines, Hidden Line, and Wireframeimage. To change the display mode in the active window, click on the display modebutton in the Display toolbar to display the list as shown. Shading With Reflections:The second icon in the display mode button group generates a moreenhanced shaded image of the 3D object. Shading With Edges:The first icon in the display mode button group generates a shadedimage of the 3D object wi
the design process. Parametric modeling is accomplished by identifying and creating the key features of the design with the aid of computer software. The design variables, described in the sketches and features, can be used to quickly modify/update the design. In Creo Parametric, the parametric part modeling process involves the following steps: 1.
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