CATIA V5 Sketcher: Corners, Rotate Patterns and a Spanner

Next, let's create triangular cutouts as shown in the picture. In this step, we shall use commands like Line, Mirror, Corner, Constraint and Rotate. I will use the D90 and D40 circles as references to create this triangular cutout shape and create a circular pattern of the same. To begin with, I will click on the Axis option in the Profile toolbar and draw a line on the vertical axis as shown. Next, I will click on the Line option in the Profile toolbar and draw a line from the point at which the D40 circle and vertical axis are coinciding.

This start point can be identified when both the circle and construction lines turn orange in color. Now, let's place the end point of the line on the D90 circle. Note that this line is not fully constrained and is moving along the center. So, an angular dimension is required to arrest this movement. Before that, let's use the Mirror command from the Operation toolbar and create a duplicate of this line on the other side of the vertical axis. Now, I will click on the top end of the first line, then press and hold the Ctrl key, and then click on the top end of the other line and constrain the distance between them to 25 mm.

Now, these two lines are fully constrained. Now, I will double-click on the Corner command from the Operation toolbar and then select the left side line and the circle as shown to create a rounded edge. Based on the preview, we can release the mouse when the fillet is in the correct position. Let's do the same operation on the right side and also at the bottom of this triangular shape. It is sufficient to pick on the point at the bottom as both the connecting objects are straight lines, unlike the other two corners which are connecting a straight line and a curve.

Now, I will modify the radius of one corner to 4 mm. I will double-click on the Corner Radius value on the other side. Type equal to sign and then click on the 4 mm radius from the first corner. This creates a formula as discussed earlier. Now, let's modify the Bottom Corner Radius value to 2 mm. The triangular cutout is now fully constrained. Let us now use this triangular shape to create instances along the circumference of the circle. I will press and hold the Ctrl key and select all the edges of the triangular cutout.

Next, I will click on the Operation toolbar. Then click on the Rotate option. This option allows us to rotate one or more selected objects along a point, an axis or a plane. Then, in the Rotation Definition window, with the Duplicate mode checked, I will change the instance's value to 5. Then, I will click on the center of the circle. Then click on the top of the triangular shape. Now, I will change the angle value to 60. And then click on the left side of the original shape, making sure the angle shows 60 degrees.

This means that the Rotate command created the first instance at an angle of 60 degrees from the vertical axis, anticlockwise, and so on. As we can see, the instances are not fully constrained. There is a limitation in the software. However, it is recommended to create duplicates of such cutouts in the part model rather than while sketching. Now, let's move on to creating hole cutouts on the inner construction circle as shown in this picture. We shall use Polygon and Rotate commands for this step. First, let's click on the Polygon option in the Profile toolbar.

And then click on the point at which the D25 circle is coinciding with the vertical axis. You can zoom in or out of the sketch as required. Let's constrain the hexagon by giving a dimension to a side as 2 mm. Now, I will use the Rotate option from the Operation toolbar to make 5 more instances of this shape along the D25 circle. To do this, I will select all 6 sides of the hexagon, the 2 construction circles around the hexagon, and the 2 mm dimension constraint.

Then, I will click on the Rotate option, change the instances to 5, with duplicates option checked. I will now select the center of the main circle, then select the center of the hexagon. Then, I will click on the D25 circle towards the left of the hexagon as shown. Making sure the angle is set to 60 degrees. Note that, when I move the mouse to indicate the direction of rotation, the angle value changes by 5 degrees each time. Rotate command is now complete. Again, the rotated instances are not fully constrained because of the limitation in the software.

I am clicking on the Dimensional and Geometrical Constraints options on the Visualization toolbar to hide all the constraints. Now, we shall create a slot in the sketch as shown in the picture. I will use Elongated Hole and Constraint commands for this step. From the Profile toolbar, I will click on the Elongated Hole command. The inputs for an elongated hole are Start Point, End Point, and Radius of the Curved Edge. So, let's create the slot as shown in the picture here. I will use the Constraint command to give dimensions and fully define the slot position as shown.

I can click on the Dimensional Constraints icon from the Visualization toolbar to view the dimensions. As you can see, the distance from the central vertical axis to the start point of the slot is 28 mm. Distance between the start and end points of the slot is 12 mm, and the radius of the slot's curved edge is 3.5 mm. Now, the entire wheel cover sketch is complete. I can click on the Exit Workbench icon to come out of the sketch. I can double-click on Sketch 1 under Geometrical Set 1 in the Specification Tree to activate the sketch and make changes.

If I click on the Sketch Solving Analysis icon from the Tools toolbar at the bottom of the CATIA window, the Diagnostic tab shows that the sketch is under-constrained, which is expected as the rotated feature constraints are not fully defined. However, if you look at the Geometry tab, it is shown that all the curves are closed, and this sketch can be used to create a solid model. Now, we shall work on another sketch exercise to learn a few more commands used in the Sketcher Workbench. In the picture is the sketch of a spanner.

To begin with, we shall draw the circular ends of the spanner as seen in this slide. For this step, I shall use the commands like Axis, Circle, Offset, and Constraint. I will click on Start under Menu Bars on the top left corner of the screen. Then click on Mechanical Design. And then click on Sketcher Workbench. I shall name this part as Spanner. Let's keep the Create a Geometrical Set box checked. I will click on OK. And then click on File and save the cat part in a preferred location.

Next, I will click on the Point option in the Reference Elements toolbar. I will let the X, Y, Z components be 0. And then click on OK. Now, I can click on the Sketch toolbar downward arrow and select the Position Sketch option. And then, I will click on Y, Z plane from the specification tree for planar support reference. Let's change the origin type to Projection Point and select 0.1 from the specification tree. To ensure the central, vertical, and horizontal axes are aligned as shown, you can use the Reverse V, Reverse H, and Swap checkboxes to modify the alignment.

And then click on OK. From the Profile toolbar, I can select the Axis command and draw a horizontal line starting from the coordinate axis and place the other end at a distance of 250 mm. Now, I can click on the Circle option from the Profile toolbar and draw two circles on either end of the axis. I will apply dimensions of 40 mm radius to the circle on the left end and 30 mm radius on the circle on the right end. I will double-click on the Offset command from the Operation toolbar.

Then click on the R40 circle and modify the offset value to 15 mm and place the mouse pointer inside the R40 circle and then hit the Enter key. Next, I will click on the R30 circle, change the offset value to 5 mm and move the mouse cursor to the outside of the R30 circle and then hit the Enter key. I can press on the Escape key to exit the Offset command. Let's look at the picture to understand the connector. Let's look at the picture to understand the connector.

The connector is straight in the middle and has curved ends where it joins the circles. There is an elongated hole at the center of the sketch as well. I will use Profile, Mirror, Elongated Hole and Constraint commands for this step. For this part of the sketch, we shall use the Profile option in the Profile toolbar. I will click on the R40 circle above the horizontal axis. Now, I will move the mouse pointer towards the right and then click on the Tangent Arc icon in the Sketch Tools toolbar to convert the straight line to a curve in the same Profile.

Now, I will click on the R35 circle to end the Profile and then I will hit the Escape key. I will now update the Arc Radius to 30mm and the vertical distance of the straight line from the horizontal axis to 10mm. If the Tangent Arc is still not fully constrained, I can select the Arc and the R35 circle and click on Constraints defined in Dialog Box command. Then, I can check the Tangency box and click on OK. On the left end of the connector, I will apply the Corner command from the Operation toolbar to create a smooth curve.

Now, I am applying a corner radius of 30mm. Next, I shall use the Mirror command from the Operation toolbar to replicate the connector line onto the other side of the horizontal axis. First, I will select the straight line, then press and hold the Ctrl key and then select both curves at the ends. Now, I will select the Mirror command. Once I click on the horizontal axis for reference, the Mirror command is completed. Next, let's use the Quick Trim command from the Operation toolbar to remove unnecessary curves as shown in the picture.

This action creates completely closed curves. Let's check the Sketch Solving Analysis to ensure all the curves are closed. I can go to Tools, Sketch Solving Status, Geometry tab and see that all the curves are closed. I can click on Close to come out of this window. Next, I will click on the elongated hole from the profile toolbar and place the start point on the horizontal axis. Let's place the end point on the same axis at a distance of 120mm and apply radius 6mm to the end curves.

Now, let's define the distance between the start point of the slot and the vertical axis as 65mm using the Constraint command. Now, can you see the sketch is fully constrained? In the next step, we will create grooves on either end of the spanner as shown in this picture. Let's draw a vertical axis passing through the center of the R30 circle. I will make sure the axis is coincident with the center of the circle. If not, you can add the constraints separately. Now, I will select the Circle option from the Profile Toolbar and draw a circle on the R30 circle coinciding with the vertical axis with a radius of 1.5mm.

Using the Quick Trim option from the Operation Toolbar, I will erase the upper part of the circle that we just created. Next, I will select the semicircle. Then click on the Rotate option in the Operation Toolbar. In the Rotation Definition window, I will change the instances to 24. Click on the center of the R30 circle. Then click on the center of the semicircle. Now, I will move the mouse cursor anti-clockwise. Update the angle value to 15 degrees. And click on the R30 circle. This completes the Rotate operation.

Let me hide a few dimensions to keep the sketch clean. I will click on the Line command from the Profile Toolbar and draw as shown. I will make the line coincide with outer and inner circles as shown. I will use the Constraint command to give the height of the start point of this line from the center axis as 10mm. Also, I will constrain the angle between this line and horizontal axis to 20 degrees. Next, I will draw another line parallel to the line we just drew with a length of 43mm.

I will apply constraints to make sure the start and end points of the line are coincident with the circles as shown. I will use the Quick Trim option to remove the four curves as shown. The Spanner sketch is now complete. Let's click on the Sketch Solving Analysis command from the Tools Venue Bar at the top of the CATIA window. The Diagnostic tab shows that the sketch is under-constrained, which is expected as the rotated constraints are not fully defined. In the Geometry tab, it is shown that some of the curves are open as the rotated elements are missing constraints.

This sketch can still be used to create a solid model. I can click on the Exit Sketcher command to come out of this sketch. I hope you got a good understanding of the Sketcher workbench from the exercises that we did. In the next session, we will be taking a look at part design. Goodbye and thank you for watching.