IT, Sligo. Equations Tutorial

Transcription

1 Equations Tutorial Parametric Modelling: SolidWorks is a parametric modelling system where parameters, such as dimensions and relations, are used to create and control the geometry of the modelled part. When modelling in SolidWorks it is possible to create mathematical relations between model dimensions or other model properties using SolidWorks equations When using equations, dimension names and other property names are used as variables and other global variables can be created. Mathematical functions can be used to create mathematical relationships variables and between two or more dimension in sketches, parts and assemblies. Tutorial Exercise In the following exercise you will create an equationsdriven design for the component shown opposite. The purpose of this assignment is to create a component which will have adjustable overall thicknesses, in order to produce different variants of the component, such as for light, medium and heavy duty applications. You are going to create (and submit drawings for) two variants of this component, both a Light Duty and Heavy Duty version. Note that the bore diameter, overall height and length, along with the hole size and position will not change; it is the wall and base plate thicknesses which will update. Variants Light Duty (t = 10mm) Heavy Duty (t = 20mm) Create a New Part: Create a folder for the equations assignments and then create a new Part. Save the part using a suitable name (e.g. Flange) Modelling the base Using the Top reference plane, model the base using three circles as shown and 4 lines tangential to each of the circles. 1

2 Next trim out the inner portions of the each of the circles. Ensure that the circle centres are horizontally aligned and apply an Equal relationship between the left and right hand arcs N.B Trimming the middle circle automatically maintains this relationship between the top and bottom arcs. Finally, add dimensions to the geometry as shown, to fully define your sketch. N.B. Disregard the actual values accept whatever sizes have been used. Correct values will be specified later. Variable Name: Each dimension has an identity or variable name. Hovering over the dimension for a moment will reveal this name. Selecting a dimension will show its name in Feature Manager in the Primary Value section. These will be used to create mathematical relationships between dimensions. Modelling the base Where features are required to be the same size (and to remain the same size in the event of modifications) the equal relationship should be used (as in the case of the left and right hand arcs). However where relationships other than this are needed Equations are required. For this assignment to maintain symmetry, the dimension defining half the width (HalfSpan) must be half of the dimension defining the full width (FullSpan). This relationship will be applied using an equation. Renaming Dimensions Select the dimension which defines the full width (e.g D1@Sketch1 ) and then rename the variable as FullSpan. (FeatureManager pane on the left). On entering Return portion reappears. This identifies the sketch to which the variable belongs. Rename the remaining dimensions as shown in the diagram above (i.e HalfSpan, SideRad, etc. 2

3 The Equations tool may be accessed from the pull-down menu by selecting Tools- Equations. From the Tools drop-down menu, select Equations. This will bring up the equations dialog box, where equation subsequently created will be listed. To add a new equation pick in the Add equation cell. Applying Equation1: To specify that dimension A (the half width dimension) is half dimension B (the full width dimension: Pick in the Add equation cell. Select the HalfSpan dimension in the sketch its name will be displayed in the cell and an = sign will appear in the Value/Equation cell (see below). Select the FullSpan dimension (its name will appear in the cell) and then type / and 2 (= FullSpan@Sketch1 /2 will be entered see below). 3

4 This creates a mathematical relationship whereby Dimension A will always be half the value of dimension B. Select OK to close the Equation dialog box. Note that the symbol the HalfSpan dimension, indicating that it is driven by an equation. will be attached to To see the effect of this relationship double click on the FullSpan dimension and change it values to 150mm. Note that the HalfSpan dimension changes to 75. In this relationship the 150mm dimension is the driving dimension while the 75mm dimension is the driven dimension. Driven dimensions are represented by the symbol and cannot be modified directly by the user. This equation has been applied within this specific sketch. However equations are not limited to operating to within a sketch. Dimension can also be applied between any dimensions within a model (or between models in an assembly). Before finishing the sketch change the larger radius (BaseRad) to 50mm and the smaller radius (SideRad) to 25mm. Continue modelling Continue modelling by extruding the base by 10mm. Working on the top surface draw a circular sketch concentric with the central arcs. However rather than snapping to the arc end points; dimension independently of the base and specify a dimension of 100mm. Create an extrusion 80mm high. Continue by creating another sketch and cutting a 70mm diameter hole Through All (you can create the sketch on the Top plane or on either the base or upper surface of the model). Finally cut through holes of diameter 15mm at the centres of the 25mm arcs. Define the hole diameters using an Equals relationship and one dimension only. 4

5 To display all dimension for the current model, Right click on Annotations in the Feature Manager and select Show Feature Dimensions. The model should now look as shown opposite. Select the dimension shown and rename them as OD, ID and T respectively. If you want to display the dimension names in the graphics window, this can be done by selecting the View pull-down menu and activating the Dimension Names menu item. The names will be displayed in brackets, under the dimension value. Building design intent into the model In the following steps the model will be adjusted to enable the design to cater for a pipe size of 75mm and to enable the model thickness to be uniformly adjusted to produce models of varying strengths. Manually adjust the 70mm bore diameter dimension to 75mm. 5

6 Definition of the upper section. Now other dimensions will be adjusted in a manner that will achieve a uniform wall thickness, where that wall thickness is dictated by the base thickness dimension. Once an equation has been added, an Equations feature menu item is added in the Feature Manager pane. To add further equations, or to modify existing ones, pick Equations from the Tools drop-down menu or alternatively right-click Equations in Feature Manager and pick Manage Equations... from its pop-down menu. Pick in the Add equation cell. Select the OD dimension its name will be displayed in the cell and an = sign will appear in the Value/Equation cell (see below). Pick the 75mm ID dimension Type + Pick the 10mm T dimension Type *2 Pick OK and adjust the height or thickness (T) of the base to 10mm, 15mm and 20mm and observe the model updating. Note that the larger radii on the base flange remains at R50, whereas the cylindrical feature changes to reflect the varying wall thicknesses. To keep the base flange tangential to the Cylindrical upright, activate the Equations Editor again and add an appropriate equation. Select the R50 BaseRad dimension and make it equal to the outside diameter OD divided in half. Finally, to establish and maintain a 2:1 relationship between the two radii in Sketch1 (BaseRad & SideRad) add another equation: Pick OK to exit Equations and add 5mm fillets to complete the model. 6

7 Test the Equations: To test the equations, modify the T dimension ( base flange thickness) and observe the model updating. Try different sizes and note the model changing. NOTE: You may need to rebuild the model to see the effect of the equations entered. Assignment Instructions/Requirements Two variants are required one Light Duty version with a flange base and wall thickness of 10mm and a Heavy Duty version with a T thickness of 20mm. Modify the thickness dimension and observe these two variants. Save two copies of this part, one called Light Duty and the other part called Heavy Duty Drawings Required: On a single drawing sheet, create a drawing of both of these variants. (Suggestion: sketch a vertical line to divide the sheet in half and place a drawing on either side of the sheet). Both drawings should contain a Plan, Elevation, Side View and Isometric View. Fully dimensions both drawing (only 8 dimensions {approx.} required per drawing). Ensure that the drawing contains a Title, Drawing Number, Your Name and the date. Consider scale, layout, and the use of tangent edges, hidden detail lines, centre lines, etc. Submission Submit the drawing detailed above on an A4 sheet. 7

8 Equations Assignment Introduction: A company manufactures the component shown opposite in a variety of strengths/sizes, depending on customer requirements Standard Features: Large Boss: Bore Diameter is 50mm Height (H1) is 20mm greater than the Rib height. Small Boss: Bore Diameter is 30mm Height (H2) is 10mm greater than the Rib height. Rib: Height (H3) is three times the thickness Rib width is equal to the thickness Overall centre-to centre distance is 140mm Apply fillets to all internal corners with a radius of one fifth of the thickness. The product is made in a variety of thicknesses, i.e. 10, 15 and 20mm. For any variant all sections must be of equal thickness Model the component so that each variant can be achieved by simply changing a single thickness dimension. Assignment Instructions/Deliverables: Model the component to meet the requirements specified. Apply appropriate equations so that all component wall thicknesses and other dimensions can be adjusted using a single thickness variable. Create 3 variants (configurations) of the part. Create draft views of the 3 variants, providing dimensional evidence of adherence to the thickness requirements. (NOTE: the drawings for all 3 variants may be made on a single A3 sheet). Submission Submit the drawings detailed above on an individual A3 sheets. 8