Introduction to Circular Pattern Flower Pot

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Shon Nelson
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Prerequisite Knowledge Previous knowledge of the sketching commands Line, Circle, Add Relations, Smart Dimension is required to complete this lesson.

1 Prerequisite Knowledge Previous knowledge of the sketching commands Line, Circle, Add Relations, Smart Dimension is required to complete this lesson. Previous examples of Revolved Boss/Base, Cut Extrude, Chamfer, Fillet, Shell and Editing Appearance should also have been completed. Focus of the Lesson On completion of this lesson you will have used: The Line, Centerline, Circle, 3 Point Circle, Add Relation, Convert Entities and Smart Dimension commands form the Sketch Toolbar. The Revolved Boss/Base, Cut Extrude, Chamfer, Fillet, Shell and Circular Pattern commands from the Features Toolbar. Circular Pattern is used when circularly spacing multiple instances of one or more features around an axis. The pattern will be created on the same face of the model as the initial feature to be patterned. This is called the Seed Feature. The Property Manager of the Circular Pattern controls the layout of the pattern. To create the pattern an axis must be chosen to revolve around. Other parameters to be set include the degrees of revolution, the number of instances and whether these will be equally spaced. The pattern can be modified to allow certain instances of the patterned feature to be skipped. RD5 DCG/Ex1 Design & Communication Graphics - 1 -

Commands Used This lesson includes Sketching (Line, Circle, Centerline, Add Relations, Convert Entities and Smart Dimension), Revolved Boss/Base, Cut Extrude, Chamfer, Fillet, Shell, Circular Pattern

2 Commands Used This lesson includes Sketching (Line, Circle, Centerline, Add Relations, Convert Entities and Smart Dimension), Revolved Boss/Base, Cut Extrude, Chamfer, Fillet, Shell, Circular Pattern and Edit Materials. Where to start? It is important to analyse the design of a flower pot prior to starting the model. The model is created by revolving a sketch so that the axis for this feature will provide the axis for the circular patterns on the base. Sketch to generate feature Revolved feature Getting started Open a new part and save as Flower pot. Choosing a plane Select Sketch on the sketch toolbar. Choose the Front plane. The view will automatically change to a front view. Creating a sketch Select the Line command, and starting from the origin create a sketch similar to the one shown above. It is good practice when creating a sketch to follow the sequence sketch, add relations and dimension. RD5 DCG/Ex1 Design & Communication Graphics - 2 -

Note: The little blue symbols at the sketching stage.

3 Select the Add Relation command from the sketch toolbar. Select the two lines indicated and choose Parallel in the add relation property manager. Note: The little blue symbols at the sketching stage. indicate the relationship a line may have gained Dimensioning the Select Smart Dimension from the sketch toolbar and dimension the Sketch sketch as shown below. To set the angle, select the two lines indicated, enter 85 in the Modify Box and confirm. RD5 DCG/Ex1 Design & Communication Graphics - 3 -

Note The sketch will change from blue to black when it is fully defined.

Creating the feature Select Features from the Command Manager.

screen. Select Revolved Boss/Base, the sketch rotates to a trimetric view.

edge of the sketch as the axis for the revolution.

4 Note The sketch will change from blue to black when it is fully defined. To Confirm the sketch. Creating the feature Select Features from the Command Manager. The Features toolbar has now replaced the Sketch toolbar along the top of the screen. Select Revolved Boss/Base, the sketch rotates to a trimetric view. In the Revolved Boss/Base feature property manager select the 150mm vertical edge of the sketch as the axis for the revolution. At this point a preview of the feature will appear. Click OK button to create the feature. Alternatively select the confirmation corner. from the RD5 DCG/Ex1 Design & Communication Graphics - 4 -

Completed feature: This is the first completed feature of the part. The sketch has been absorbed into the Revolve 1 feature in the Feature Manager.

Creating the indents on the base Creating the sketch Select the Sketch toolbar from the Command Manager.

The model will rotate to a view looking perpendicular to the bottom surface. Note: Select the Rotate View icon in the View Toolbar.

Select the Centerline Sketch command. Draw a vertical line on the chosen surface from the centre.

5 Completed feature: This is the first completed feature of the part. The sketch has been absorbed into the Revolve 1 feature in the Feature Manager. Renaming a feature: Select in the Feature Manager Tree, press the F2 key and type the new name Main Body to replace Revolve1. Creating the indents on the base Creating the sketch Select the Sketch toolbar from the Command Manager. Enter the sketch mode by selecting at the start of the Sketch toolbar. When prompted select the bottom face and select Normal To from the View Command. The model will rotate to a view looking perpendicular to the bottom surface. Note: Select the Rotate View icon in the View Toolbar. Alternatively by pressing and holding down the wheel on the mouse the rotate view mode is activated. Also the arrows keys on the keyboard can be used. Select the Centerline Sketch command. Draw a vertical line on the chosen surface from the centre. Select the Line sketch command and draw the vertical line shown. Click to end the vertical line, remain in the Line command. By moving the pointer as if to start a second line and then doubling back to the start point and starting again, the software will automatically change into circle/arc mode. Draw a semi-circle. Click RD5 DCG/Ex1 Design & Communication Graphics - 5 -

to complete the semi-circle and the software changes back to the Line command.

Select the Convert entities command to convert this circle to a circle within the sketch.

Select the centerline and the centre point of the semi-circle and in the Add Relation Property Manager make

Confirm the dimensions and exit the sketch. Creating the feature Select Features from the Command Manager.

6 to complete the semi-circle and the software changes back to the Line command. Draw a second line parallel to the first. Select the circular edge of the base. Select the Convert entities command to convert this circle to a circle within the sketch. Use the Trim Entities command to trim the circle to the required size. Select the Add Relation command. Select the centerline and the centre point of the semi-circle and in the Add Relation Property Manager make them coincident. Using Smart Dimension apply the above dimensions to the circle. Confirm the dimensions and exit the sketch. Creating the feature Select Features from the Command Manager. The Features toolbar has now replaced the Sketch toolbar along the top of the screen. Choose Extruded Cut. Select Isometric View form the Command View. The feature previews in isometric. RD5 DCG/Ex1 Design & Communication Graphics - 6 -

Use the Extrude Feature Manager on the left of the screen set up the feature.

Adding a Chamfer A 4mm chamfer is now added to the top edge of the Base Cut. Rotate the model to view the base cut.

In the Chamfer Feature Manager set the parameters as shown and select the top edge of the extruded cut in the graphics area.

7 Use the Extrude Feature Manager on the left of the screen set up the feature. to Extrude Feature Settings End Condition = Blind Depth = 4mm Click OK button to create the feature. Rename the feature Base Cut. Adding a Chamfer A 4mm chamfer is now added to the top edge of the Base Cut. Rotate the model to view the base cut. Select Chamfer from the Features toolbar. In the Chamfer Feature Manager set the parameters as shown and select the top edge of the extruded cut in the graphics area. Note: The flip direction check box will angle the chamfer inwards. Confirm the feature. Adding a Fillet A fillet is now added to the top and bottom edges of the chamfer. Select Fillet Toolbar. in the Features In the Fillet Feature Tree Manager set the Fillet radius to 2mm and the select the top and bottom edges of the chamfered cut in the graphics area. Confirm the feature. RD5 DCG/Ex1 Design & Communication Graphics - 7 -

The completed feature should now look like this.

In the View menu activate the Temporary Axes.

Choose the Circular Pattern Command from the features toolbar.

Expand the Feature Tree of the Flower Pot (left click on the + sign) in the graphics area and

8 The completed feature should now look like this. Pattern the Feature The Base Cut can now be patterned on the bottom surface of the model. In the View menu activate the Temporary Axes. The axis from the original Revolved Boss/Base will become visible. Choose the Circular Pattern Command from the features toolbar. In the Circular Pattern Feature Manager select the visible axis, instances = 4 with equal spacing. Expand the Feature Tree of the Flower Pot (left click on the + sign) in the graphics area and select Base Cut, Chamfer1 and Fillet1 as the Seed Features to pattern. Alternatively click the Features to Pattern box and select them on the actual model. Click OK to create the pattern. Rename Feature Rename the feature Base Pattern RD5 DCG/Ex1 Design & Communication Graphics - 8 -

Shell Command It is also important to shell after the cut feature on the base has been patterned.

In the Shell Feature Manager Distance = 1mm Select the top surface of the model. Tick Show Preview Click OK button to create the pattern.

Creating the holes Creating the Sketch A circular hole is created first on the base and then patterned. Select the Sketch toolbar. Select Sketch on the Sketch toolbar.

9 Shell Command It is also important to shell after the cut feature on the base has been patterned. If the shell was created first the 4mm deep indents could not have been created in a shelled feature 1mm thick. Select the Shell command on the Features toolbar. In the Shell Feature Manager Distance = 1mm Select the top surface of the model. Tick Show Preview Click OK button to create the pattern. Rename the Feature Select the Feature in the Feature Manager Tree, press F2 key and rename Base Cut Pattern. This is how the completed shell feature should look when complete. Creating the holes Creating the Sketch A circular hole is created first on the base and then patterned. Select the Sketch toolbar. Select Sketch on the Sketch toolbar. When prompted, select the bottom surface as the plane to sketch on. This will require the model to be rotated. Select Normal To from the View Command Menu. Select the Centerline Sketch command. Sketch two centerlines from the centre of the circle to the circumference of the base circle. Add Relations to make one RD5 DCG/Ex1 Design & Communication Graphics - 9 -

horizontal and Smart Dimension the angle to 45 0. Select the Circle Command.

Finish the sketch by clicking on the Exit Sketch icon or Exit Sketch in the Confirmation Corner.

In the Cut Extrude Feature Manager set the direction to Through All. Click OK to complete the feature.

10 horizontal and Smart Dimension the angle to Select the Circle Command. Sketch a circle centred on the centerline and Smart Dimension as shown. Click OK to complete the sketch. Finish the sketch by clicking on the Exit Sketch icon or Exit Sketch in the Confirmation Corner. Creating the Feature Select the Features Toolbar in the Command Manager. Select Extrude Cut. Change the view to Isometric in the View Command. In the Cut Extrude Feature Manager set the direction to Through All. Click OK to complete the feature. Select this feature in the Feature Tree Manager, press the F2 key and rename the feature Circular Hole. Pattern the Feature The Circular Hole feature can now be patterned with similar settings as the previous Circular Pattern. Select the same axis as previously, instances = 8 with equal spacing. RD5 DCG/Ex1 Design & Communication Graphics

Circles Pattern. The model should now look like this.

This can done using the Quicksave button.

Select the Line command and sketch as shown in the diagram opposite.

11 Click OK to complete the feature. Rename the Feature In the Feature Manager Tree rename the pattern Base Circles Pattern. The model should now look like this. Note: It is advisable to save the part at regular intervals. This can done using the Quicksave button. Adding an edge A protruding edge is added to top of the Flower Pot. Sketch the profile below on the Right plane. Zoom to the top corner. The graphics area will enlarge the selected area. Select the Line command and sketch as shown in the diagram opposite. Ensure the outer line is parallel to the side of the Flower Pot. Dimension as shown. Creating the Feature Select Features in the command Manager and select Revolved Boss/Base. Select the same axis as before. Click OK to confirm the feature. One last Fillet Add a 1mm fillet feature to the underside surface of the external rim. RD5 DCG/Ex1 Design & Communication Graphics

Adding color To add colour to the model, right click

In the menu select Appearance and Color.

colour for the Flower Pot. Click OK to complete.

12 Adding color To add colour to the model, right click on the Flower Pot feature in the Feature Manager Tree. In the menu select Appearance and Color. In the Color and Optics Property Manager select a colour for the Flower Pot. Click OK to complete. Save the completed model. RD5 DCG/Ex1 Design & Communication Graphics

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Digital Camera Exercise

Digital Camera Exercise Commands Used New Part This lesson includes Sketching, Extruded Boss/Base, Extruded Cut, Fillet, Chamfer and Text. Click File, New on the standard toolbar. Select Part from the New SolidWorks Document