3-2 Parametric Modeling With SolidWorks - Computer Science

3-2Parametric Modeling with SolidWorksIntroductionIn the 1980s, one of the main advancements in solid modeling was the development ofthe Constructive Solid Geometry (CSG) method. CSG describes the solid model ascombinations of basic three-dimensional shapes (pdmitive solids). The basic primitivesolid set typically includes: Rectangular-prism (Block), Cylinder, Cone, Sphere, andTorus (Tube). Two solid objects can be combined into one object in various ways usingoperations known as Boolean operations. There are three basic Boolean operations:JOIN (Union), CUT (Difference), and INTERSECT. The JOIN operation combines thetwo volumes included in the different solids into a single solid. The CUT operationsubtracts the volume of one solid object from the other solid object. The INTERSECToperation keeps only the volume common to both solid objects. The CSG method is alsoknown as the Machinist's Approach, as the metho9 is parallel to machine shoppractices.) Primitive Solids I INTERSECT I

Constructive Solid Geometry Concepts3-3Binary TreeThe CSG is also referred to as the method used to store a solid model in the database. Theresulting solid can be easily represented by what is called a binary tree. In a binary tree,the terminal branches (leaves) are the various primitives that are linked together to makethe final solid object (the root). The binary tree is an effective way to keep track of thehistOl:v of the resulting solid. By keeping track of the history, the solid model can be rebuilt by re-linking through the binary tree. This provides a convenient way to modify themodel. We can make modifications at the appropriate links in the binary tree and re-linkthe rest of the history tree without building a new model.Terminal branchesUnion

3-4Parametric Modeling with SolidWorksThe Locator DesignThe CSG concept is one of the important building blocks for feature-based modeling. InSolidTflorks, the CSG concept can be used as a planning tool to determine the number offeatures that are needed to construct the model. It is also a good practice to create featuresthat are parallel to the manufacturing process required for the design. With parametricmodeling, we are no longer limited to using only the predefined basic solid shapes. Infact, any solid features we create in SolidWorks are used as primitive solids; parametricmodeling allows us to maintain full control of the design variables that are used todescribe the features. In this lesson, a more in-depth look at the parametric modelingprocedure is presented. The equivalent CSG operation for each feature is also illustrated.),.- Before going through the tutorial, on your own, make a sketch of a CSG binary treeof the Locator design using only two basic types of primitive solids: cylinder andrectangular prism. In your sketch, how many Boolean operations will be required tocreate the model? What is your choice of the first primitive solid to use, and why?Take a few minutes to consider these questions and do the preliminary planning bysketching on a piece of paper. Compare the sketch you make to the CSG binary treesteps shown on page 3-5. Note that there are many different possibilities in combiningthe basic primitive solids to form the solid model. Even for the simplest design, it ispossible to take several different approaches to creating the same solid model.

Constructive Solid Geometry ConceptsModeling Strategy - eSG Binary TreeI3-5

3-6Parametric Modeling with SolidWorksStarting SolidWorksI. Select the SolidWorks option on the Start menu or select the SolidWorks iconon the desktop to start SolidWorks. The SolidWorks main window will appear onthe screen.2. Select the New icon with a single click of the left-mousebutton on the Standard tool bar.% 3. Select the Part icon with a single click of the le.ftmouse-button in the New SolidWorks Documentdialog box.a 3D representation of.p. .!4. Select OK in the New SolidWorks Documentdialog box to open a new part document.:. Every object we construct in a CAD system is measured in units. We shoulddetermine the value of the units within the CAD system before creating the firstgeometric entities. For example, in one model, a unit might equal one millimeterof the real-world object; in another model, a unit might equal an inch. In mostCAD systems, setting the model units does not always set units for dimensions.We generally set model units and dimension units to the same type and precision.5. Select the Options icon from the Standard toolbar toopen the Options dialog box.6. Select the Document Properties tab.7. Select ANSI in the pull-down selection window under the Dimensioning standardpanel as shown.NotesBalloonsArrowsVirtual SharpsDimensioning standardExtension lines[ ;.;.Gap:D ; :;JiJ ;; nsdisplayoOn top0C) On bottom 0On the rightOn the leFtDatum Features8. Click Units as shown below. We will use the default MMGS (millimeter,gram, second) unit system.

Constructive Solid GeometJ)' ConceptsDet.31lingDimensionsNotesBalloonsVwtual 5h.9rpsAnnotations [lispl.:.',,,,3-7Unit systemo r'lw::, (meter! hlogram.1second)() CGSsecond)o ·1r·I'G::,5econd 1(centimeter, gr.9m,{rnilhHleter, gram,() IP'3 (Inch, pound, second:1OCustc,mAnnotations Font9. Enter 3 in the Decimal places box under the LenRth units options to define thedegree of accuracy with which the units will be displayed.GRID and SNAP Intervals Setup1. Click Grid/Snap as shown below. We will use the default MMGS (millimeter,gram, second) unit system.,---- -- ------------------------! Document Properties - GridlSnap1 ; .3:.che:: } .DimensionsNotesBalloonsArrowsVirtual Sharps DI play03. UncheckgridDash" Automatic scaling 1aJ()rgnd spacing:Annotations Displa'/Annotations Font"S'Units 'linor-linespet' major:Snap points per minor:ColorsMaterial PropertiesImage Qualit . .Plane Display1. Grid/SnapGo To S\'stem Snaps2. Check the Display grid checkbox under the Grid options.3. Uncheck the Dash checkbox under the Grid options.4. Set the Major grid spacing to 50mm under the Grid options.5. Set the Minor-lines per major to 5 under the Grid options.6. Click OK in the Options dialog box to accept the selected settings.

3-8Parametric Modeling with Solid WorksY Note that the above settings set the grid spacing in SolidWorks. Although the Snapto grid c;Jtion is also available in SolidWorks, its usage in parametric modeling is notrecommended.Base FeatureIn parametric modeling, the first solid feature is called the base feature, which usually isthe primary shape of the model. Depending upon the design intent, additional features areadded to the base feature.Some of the considerations involved in selecting the base feature are: Design intent - Determine the functionality of the design; identify the feature that iscentral to the design. Order of features - Choose the feature that is the logical base in terms of the orderoffeatures in the design. Ease of making modifications - Select a base feature that is more stable and is lesslikely to be changed.).- A rectangular block will be created first as the base feature of the Locator design. Eile ditD. SketchI':iew nsertIrrd [r.,()Smarttr.\ DimensionI. Select the Sketch icon in the control area by clicking oncewith the left-mouse-button to display the Sketch toolbar inthe CommandManager.2. Select the Sketch button on the Sketch toolbar to create a newsketch./3. Move the cursor over the edgeof the Top Plane in thegraphics area. When the TopPlane is highlighted, click oncewith the Ieft-mouse-button toselect the Top Plane (XZPlane) as the sketch plane forthe new sketch.FrofltPlcme------------Top Plor;E --- ./:,----------.----------------.

Constructive Solid Geometry Concepts3-94. Select the Rectangle command by clicking once with the left-mousebutton on the icon in the Sketch toolbar.o5. Create a rectangle ofarbitrary size by selectingtwo locations on thescreen as shown below.I.-1"c t c Jj Sketch Entities6. Inside the graphics window, click once with theright-mouse-button to bring up the option menu.o7. Select Select to end the Rectangle command."LineCircle Centerpoint ArcI) [,Smat'l "fDiroension .8. Select the Smart Dimension command by clicking once with the leftmouse-button on the icon in the Sketch tool bar.9. The message "Select one or two ed.c;es/vertices and then a text location" is displayedin the Status Bar area at the bottom of the SolidWorks window. Select the bottomhorizontal line by left.,.c1icking once on the line.6. Select the horizontalline as the geometryto dimension.7. Pick a location belowthe line to place thedimension.10. Move the graphics cursor below the selected line and left-click to place thedimension. (Note that the value displayed on your screen might be different than whatis shown in the figure above.)II. Enter 75 in theMod?!v dialog box.12. Click OK in the Mod?fjl dialog box.

p3-10Parametric Modeling with SolidWorks13. On your own, create the vertical sizedimension of the sketched rectangle asshown.14. Click the OK icon in the Proper(vManager, or hit the [Esc] key once, to end theSmart Dimension command.Modifying the Dimensions of the Sketch1I1It1I[trjt ------ 'IInj1. Select the dimension that is to theright side of the sketch by doubleclicking with the left-mouse-buttonon the dimension text.···········1I. Seled ft the dimensionto mo I y.2. In the Modifi! window, the current length of the line isdisplayed. Enter 50 to reset the length of the line.3. Click on the OK icon to accept the entered value.Repositioning DimensionsI. Move the cursor near the vertical dimension; note that thedimension is highlighted. Move the cursor slowly until asmall marker appears next to the cursor, as shown in thefigure.2. Drag with the left-mouse-button to reposition the selecteddimension.3. Repeat the above steps to reposition the horizontaldimension.4. Click once with the left-mouse-button on the Exit Sketch iconon the Sketch toolbar to end the Sketch option.

Constructive Solid Geometry Concepts3-11Completing the Base Solid Feature 0.1 Sketch I. Select the Features icon in the control area by clickingonce with the left-mouse-button; this will display theFeatures tool bar in the CommandManager.2. In the Features toolbar, select the Extruded Boss/Base command byclicking once with the left-mouse-button on the icon. The ExtrudeProper vManager is displayed in the left panel.3. In the Extrude PropertyManager panel, enter 15 as the extrusion distance. Noticethat the sketch region is automatically selected as the extrusion profile.4. Click on the OK button to proceed with creating the 3D part.5. Use the Viewing options to view the created part. Select the Isometric icon in theStandard Views pull-down menu to reset the display to the isometric view beforegoing to the next section.1i

3-12Parametric Modeling with Solid WorksCreating the Next Solid Feature Eile l;dit ILiew Insert I1. Select the Sketch icon in the control area by clicking oncewith the left-mouse-button to display the Sketch tool bar inthe CommandManager.E':2. Select the Sketch button on the Sketch tool bar to create a newsketch.( 5kekh"5mattt·.:t Dimension3. In the Edit Sketch Proper vManager panel, trye message "Select a plane on whichto create a sketch for the enWv" is displayed. SolidWorks expects us to identify aplanar surface where the 20 sketch of the next feature is to be created. Move thegraphics cursor on the 3D part and notice that So lidWorks will automaticallyhighlight feasible planes and surfaces as the cursor is on top of the differentsurfaces.4. Rotate the view using the up arrow key to display the bottom face of the solidmodel as shown below.5. Pick the bottom faceof the solid model.5. Pick the bottom face of the 3D model as the sketching plane.)roRedar,gleNote that the sketching plane is aligned to the selected face .oCircle. '1'-. Centerpoint,,{Arc6. Select the Circle command by clicking once with theleft-mouse-button on the icon in the Sketch tooIbar.