CATIA V5 Sketcher: Circles, Translate, Mirror and Constraints

Now, let's draw the next part of the sketch, i.e., the keypad circular cutouts. For this part of the sketch, we shall use commands like Axis, Circle, Translate, Mirror, and Constrained. I will first draw a circle at the center of the smallest rectangle, and then use the Translate command to create duplicates of the circle above and below the original circle. You will see how useful the mirror command is for reducing rework. To draw a circle, I can click on the circle command on the Profiles toolbar. Then, I can click on the point that I want to be the center of the circle, and move the mouse pointer.

You can see the circle growing bigger and smaller as I move the mouse. Once I click elsewhere on the sketch, a circle is formed. If the geometric constraints are blocking the view, we can deactivate the geometric constraints icon in the visualization toolbar. The radius value can be entered in the point on circle H window on the top or after creating the circle. If the circle is not fully constrained, I can select the center of the circle, then the center of the third rectangle, and then click on the constraints defined in Dialog Box command.

Now, I can select the Coincidence checkbox to create a geometrical constraint. Notice how the circle is fully constrained. Next, I will select this circle by clicking on its edge. Then, I will click on the Translate option from the Operations toolbar. Translate option allows moving a selected object from one position to another in a linear fashion. If the Duplicate Mode checkbox is on, it will create the number of duplicates mentioned in the Instances field. The numerical value at the bottom determines how far the object is to be moved.

The direction in which the object is to be translated is determined by selecting the axis in the graphics area. Please note that while duplicating, the original instance will still be present. Now, I will click on the center of the original circle. Then, click along the vertical axis above the original circle. This places the duplicate circle in position. Let's apply a constraint between the center point of the new circle and the yellow horizontal axis to 11 mm. I will also apply a coincidence geometrical constraint between the center point of the circle and yellow vertical axis.

Let's do one more translation operation. For this, I will select the new circle. Click on the Translate option from the Operations toolbar. Next, I can click on the center point of the selected circle. And then, click along the vertical axis to provide the direction. I will update the dimensional and geometrical constraints to make the circle fully constrained. Next, let's draw two construction lines parallel to the vertical axis as shown in the picture. To do this, I can click on the Offset command from the Operations toolbar.

Then, I will select the yellow vertical axis and then click on Construction or Standard Element from the Sketch Tools toolbar. I activate the both sides offset icon on the same toolbar. You can see that two vertical lines are being added on either side of the yellow vertical axis and they are seen as construction lines. Now, if I move the cursor to the new position window at the top, I can update the offset numerical value to 5 mm and hit Enter to complete the offset command. Next, I will select these three circles.

I can do this by selecting the first circle in the usual manner. And then, if I press and hold the Ctrl key, I can add more entities to my current selection. Now, I can directly click on the Mirror option from the Operations toolbar. Then, click on the left vertical axis or construction line created using the Offset command. You can see that the new set of circles are copied from the center at a distance of 5 mm from the construction line. The position at which the circles are mirrored is determined by the axis along which the mirror happened.

Let's repeat the Mirror command. I will click on the Mirror option. Then, I press and hold the Ctrl key and select all three circles which are on the yellow vertical axis. The software allows you to select one circle and not the rest. Let me hit Escape on the keyboard to exit this command. We shall first press and hold the Ctrl key and multi-select all three circles and then click on the Mirror option. Now, I can left-click on the right vertical construction line to complete this Mirror operation.

Moving on to the next part of this sketch, we shall draw the antenna as shown in this picture. We shall use commands like Line, Circle, Trim and Constraint for this step. First, I will click on the Line command in the Profile toolbar. Now, I will click above the outer frame like this and then click on the top of the frame to draw a vertical line. While placing the endpoint of the line, you can see that the top line of the frame is highlighted in orange, which means that Katia is assuming a coincidence geometrical constraint between the two lines.

Next, I will select the Line option again and draw another line approximately equal and parallel to the first one. I will constrain the height of the first line as 8 mm and constrain the horizontal distance from the center to this same line as 25 mm. Next, I will constrain the distance between the two parallel lines to be 7 mm. If I pick on this point on top of the left line, you can notice that it is movable in up and down directions, which means this line is not fully constrained.

If we define the height of this line, the movement will be arrested. To do this, I can select this line and constrain command. Then, I can double-click on the numerical value in the graphics area to modify the value. Now, let's learn something new. In the value field, I will type equal to sign from the keyboard and then click on the dimension of the right side line. You can see that the value field updated to 8 mm and is now not editable. Once I click on OK, you can see that the dimension value that is newly added has f of x as suffix, which indicates that a formula has been applied to this dimension.

It also implies that if you change the parent dimensional value, this dimension updates as well. Let's test this out. I will double-click on the right side line dimension and change the value to 10 mm and hit OK. Observe that the dimensional value of the left side line has also updated to 10 mm. Now, let's change the value back to 8 mm. Next, we need to create a curved edge on top of these two lines. To do this, I will select the circle option in the profile toolbar.

Now, I will left-click to place the center point in an approximate position as shown and draw the circle. Let's constrain the circle radius to 3.5 mm. Now, I will press and hold the CTRL key and select the left side line and the circle and then select the constraints defined in the dialog box option. I will check the tangency box and click on OK. This step applied a tangency constraint between the line and the curve. Let's do the same for the other line as well. If you selected the regular constraint command by mistake, you can hit the escape button on the keyboard once and you will be able to select the correct option this time around.

Both lines and the circle turned pink in color. This means that there are more than enough constraints defined for these elements. You may hit CTRL plus Z from the keyboard to go one step back and eliminate this constraint or you may carefully select the constraint symbol from the graphics area and hit the delete button from the keyboard. We can see that the element that is under-constrained is the circle. If I select and move the circle, I can understand in which direction this element needs to be constrained.

Since it is moving in up and down directions, we need to give a vertical dimension. If I select the center of the circle and the line on the upper frame and hit Enter key, I can modify the dimension to 8mm. The antenna is almost done, except that the bottom curve of the circle is not needed. This half of the circle needs to be eliminated. This can be achieved by using the trim option from the operation tool. To do this, I will select the top part of the circle and then the left side line of the antenna.

A warning message pops up. Please read through the message and then click on Yes. The sketch seems to be fully constrained, so we shall proceed further. Next, we will draw the screen cutout sketch as seen in this picture. In this step, we will use rectangle, constrained and corner commands. From the Views toolbar, I can click on the Normal View icon to bring the sketch to a normal view in case the sketch was rotated. I can also click on the Fit All In icon from the Views toolbar to make the entire sketch visible.

Now, I will select the Centered Rectangle command from the Profile toolbar and place the center of the rectangle along the yellow vertical axis. You can zoom in or out of the sketch to have a more clear view. Let's constrain the distance between the center point of the rectangle to the yellow horizontal axis to 17 mm. Next, I shall constrain the distance between the center point of the rectangle and the bottom line of the rectangle to 18 mm. I will also constrain the center point of the rectangle with the right side of the rectangle to 24 mm.

Since this is a centered rectangle, defining one half of the rectangle is enough. The other half is assumed to be symmetrical. This is not the case when we use a normal rectangle in our sketch. We will have to define more constraints than we did here to make the rectangle fully defined. Let us now learn a new command called Corner. This command helps make sharp edges into smooth curves. From the Operation toolbar, I will select the Corner option and then pick and place the curve as shown.

To smoothen the other corners, we need to select the Corner option each time. Instead, if you double-click on the Corner command, it will stay selected until we hit the Escape button. Let us modify the Corner Radius value to 5 mm on one corner. Now, I can double-click on the second corner to modify the radius. In the Value field, I will type equal to sign and then select the R5 value from the Graphics area. And then click on OK. Let us repeat the same process for the other two corners as well.

This way, if the parent Corner Radius value is changed, other three corners will also be updated with the same radius. The screen cutout is now fully defined. If I click the Fit All In icon from the Views toolbar, you can see the entire sketch. I will click on the Dimensional Constraints and Geometrical Constraints icon on the Visualization toolbar to make the constraints invisible. Next, I will click on the Vertical Construction line and then click on the Hide or Show icon in the Views toolbar. This command helps you hide or show one or more selected objects in the Graphics area.

If you want to know what objects have been hidden using this Hide or Show option, you may click on the Swap Visible Space option in the same toolbar. You can click the Swap Visible Space option again to come back to your original space. If I click on Tools from the Menu Bars, I can select Customize. In the Customize window, I will select View in the Categories list, then select Hide or Show under Commands list. Now, I will click on the Show Properties button. Under Command Properties, you can see that I have given space as an accelerator.

Meaning, I can use the space bar on the keyboard as a shortcut for this action. I can click on Close to exit this window. Now, I will select the other construction line and hit the space bar and it hides itself. In order to come out of the Sketcher Workbench and make a solid model out of the sketch, you can click on the Exit Workbench icon on the top right corner of the CATIA window. In the Specification Tree, you can see Point 1 and Sketch 1 elements under the Geometrical Set 1, indicating that the sketch is considered as geometry in CATIA.

Hide or Show Shortcut option is applicable for items in the Specification Tree as well. The Handset Sketch exercise is now complete. This next exercise that we are going to work on is a Wheel Cover Sketch as shown in this picture. This sketch is circular on the hole. It consists of triangular cutouts, hole cutouts and an elongated hole. Let's start making this sketch. First, I will click on Start from the menu bars on the top left corner of the screen. Then, I will click on Mechanical Design and then click on Sketcher Workbench.

Let's name this part as Wheel Cover. I will keep the Create a Geometrical Set box checked and click on OK. Now, I can go to File and save the CAT part in a preferred location. I will click on the Point option in the Reference Elements toolbar. Let the XYZ components be 0 and then click on OK. In case you want to change the name of the part, you can right-click on the part name in the Specification Tree. Click on Properties. Then click on the Product tab.

In the Part Number field, the part name can be edited. Other fields like Revision, Description, etc. can also be filled up as required. You can click on OK to come out of this window. Observe the Specification Tree. Geometrical Set 1 is underlined, meaning the following actions are going to update under this part of the tree. If you click on the plus sign beside the Geometrical Set 1, you will see the point 1 that we just created and further down there are the X, Y and Z components.

By double-clicking on any of these components, we should be able to edit the numerical value of the coordinate. You can hit Cancel to come out of this window. Now, let's start the sketch by clicking on the Sketch toolbar downward arrow and selecting the Position Sketch option. I will click on YZ plane from the Specification Tree for Planar Support Reference. I will change the Origin Type to Projection Point and select Point 1 from the Specification Tree. This point can also be selected from the Graphics Area at the center of the coordinate system.

You can make sure that 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 as needed. Let's click on OK to exit this window. Notice how Katia has brought the Normal View by default after creating a Position Sketch. Let's look at the sketch for a second to see the dimension. As part of the first step, we shall use commands like Circle and Constraint. We shall use the Circle command from the Profile Toolbar and draw 5 concentric circles.

I will use the Constraint command to dimension all the circles as shown. Double-click the Constraint command to keep it active until we finish giving all the dimensions. I will press and hold the Control key and select the D25 and D40 circles and click on the Construction or Standard element to make these construction circles.