CATIA V5 Interface, Workbenches and Your First Sketch

Welcome to this course. Hope you are doing well. In the following sessions, you will be learning how to use CATIA V5 software for mechanical design. As part of CATIA V5 basics, we are going to cover sketching, Part Design, advanced Part Design and drafting, assembly design and surface design. In this session, we are going to cover the definition of CATIA. I will introduce you to CATIA V5 user interface and then we shall learn about CATIA workbenches. Next, we shall see how to start a new part in CATIA and understand the mouse controls.

I will walk you through the sketcher workbench toolbars and then we shall do some exercises to sketch, a handset, a wheel cover and a spanner. Moving on, let's look at the next slide. CATIA stands for Computer Aided Three-Dimensional Interactive Application. CATIA is a solid modeling tool used for design, manufacturing, simulation and analysis. It was developed by a company called Dassault Systèmes from France. The software is used in industries like aerospace, automobile, consumer products, industrial machinery, etc. CATIA unites 3D parametric features with 2D views, which means that the two-dimensional designs can be built into three-dimensional bodies using the tools from the CATIA software.

Let us now learn the terminology of what we see on a CATIA window. User interface is the face of the software that the user sees and works in. On the top left are the menu bars, which list various menu options. Under the menu bars, on the right side and at the bottom of the CATIA window are the toolbars, which contain direct commands to create the designs. On the left side of the window is the specification tree. While creating a design, a number of elements like sketch, line, circle are created.

All these elements are included under this tree structure in a chronological order. Compass and coordinate system help the user orient and position the design in the graphics area. Let's now move on to the next slide. Let's learn how to create a new part in CATIA V5. We will see how to start a new sketch and also learn about mouse manipulation to be able to navigate in the CATIA window. So, once CATIA V5 software is installed on your computer, you may open it by clicking on this icon.

When you open CATIA V5 for the first time after installation, a new product window pops up. To design an object using computer-aided design softwares, it is general practice to create a 2D sketch of the object and then apply features like extrude or pocket to the sketch step by step. So, to start a new part, I can click on the Start menu, which is seen on the top left corner of the CATIA window. Then, I click on Mechanical Design and then Part Design. I can type in a part name.

Traditionally, solid bodies and surface-based parts are not designed in the same environment. Enable Hybrid Design option is checked if you are designing parts with multiple environments, like surfacing and solid modeling in the same window. This means that you will have access to surfacing or wireframe tools even from the part design environment. So, users with professional experience generally use this option. I shall uncheck this box for our sessions, as this course is for beginners. Create a Geometrical Set option helps organize different geometrical elements, like points, planes, axes, etc., to be grouped in one place under the tree structure.

This feature avoids confusion when the part or assembly is complex and has too many geometrical elements. I will check this box and then click on OK. Before starting your work, it is recommended to save the file in a preferred location. You can do this by going to the File menu on the top and clicking on Save. And then browsing to a preferred location and clicking on Save again. The coordinate system in a CAT software is assumed to be in an infinite space. So, if we define a reference point and have the coordinate axis from that point, the design would be easier to modify.

From the Reference Elements toolbar, I can click on the Point command to create a reference point at the center of the coordinate system. The X, Y, Z coordinates are editable and the point is placed accordingly. Now, I can click on OK to exit this window. On the left side of the CATIA window, notice that point 1 is added to the specification tree under the geometrical set 1. Now, when I click on the downward pointing arrow on the Sketch toolbar, you will see two options, Sketch and Position Sketch.

Once I click on Position Sketch, you can see two options under Type drop-down list. Sliding Sketch is constrained to a plane or a surface only. A sliding sketch can move around when its location element is moved. Location element is the origin of the sliding sketch that the user places on the sketch plane. The user would not have control over the origin and orientation of the sketch. If any changes are made to the initial steps of the sketch, the changes could impact the rest of the sketches.

Position Sketch, on the other hand, helps us define the sketch origin, plane and orientation, all of which can be modified at any point of the design. This way, the shape of the sketch profile remains the same even if the associated position of the sketch changes as the geometry of the part evolves. I will be using Position Sketches throughout this course. So, in the Sketch Positioning Definition window, I will keep the Positioned option selected for Planar Support Type from the drop-down list. From the Specification Tree, I will select XY Plane for reference.

I will then pick Projection Point as Origin Type from the drop-down list and then select Point 1 as Reference from the Specification Tree. I will leave Orientation Type as Implicit. This option allows the sketch orientation to be positioned according to the geometry of the sketch plane. Other options in the drop-down lists are applicable when there are other reference geometrical elements. We can use the Reverse H, Reverse V and Swap buttons to orient the vertical and horizontal axis seen at the center of the CATIA window graphics area.

Now, I can click on OK to complete this command. Let us now understand some basic mouse controls in CATIA V5. I will draw a line here to explain the mouse movements. I will explain how to draw these lines more in detail as we progress further. To rotate an object in the graphics area, I can press and hold the middle mouse button and left or right mouse button simultaneously and then move the mouse. To zoom in or out of an object, I can press and hold down the control key and the middle mouse button and then move the mouse.

Or, I can press and hold down the middle mouse button, then click and release the left or right mouse buttons once and then move the mouse up and down. The mouse movements will take some practice to get used to. Let's move on to the next slide. What is a workbench? CATIA has thousands of commands in order to make designing easy. CATIA grouped the commands for us into different categories and called them workbenches. If you are creating a 3D model, most of the tools you need are available in sketcher or Part Design or assembly design and generative shape design workbenches.

Workbenches are customizable, meaning you can add the frequently used workbenches to shortcuts menu. From the top of the CATIA window, in the menu bars, if I click on Tools and then click on Customize, I can select and add workbenches to the Favorites column. These workbenches will now show up on the top of the list under the Start menu like this and also show up when I click on the shortcut icon on the top right corner of the CATIA window. You can also create user-defined workbenches with frequently used commands.

You will get a better idea about workbenches as we go through the course further. In this course, I will predominantly use sketcher, Part Design, assembly design, wireframe and surface design and drafting workbenches under Mechanical Design category and Generative Shape Design workbench under Shape category. Now, let's take a quick look at some of the toolbars we will be using this week in the sketcher workbench. Reference Elements Toolbar As the name suggests, at any point in the design creation, if there is a need for a reference point, line or a plane, commands from this toolbar are applicable.

Next, let me take you to the Profile Toolbar. Profile Toolbar Profile Toolbar provides different shapes that can be used to draw a 2D sketch, like undefined profile, predefined profiles, which include rectangle, where covered glam accessible. Parallelogram, Elongated Hole, Polygon, etc. Next, the sketch tools help hide or unhide dimensions, constraints, grid, etc. This toolbar also helps with converting a solid line or arc to a construction element. Let's look at the Constraints toolbar. Once we draw a profile, it needs to be fully defined to refrain from moving in any direction. All degrees of freedom need to be arrested.

Constraints help in achieving this by assigning dimensions, limitations, etc. Down here at the bottom of the CATIA window is the View toolbar that helps the designer interact with the design by zooming in or out, Pan, shading the model, viewing in different orthogonal and isometric views, etc. Next is the Operation toolbar. It provides various options to modify the sketch profile to fit the design requirements, like making sharp edges round, erasing unnecessary lines, making duplicate profiles, etc. We will touch upon as many commands as possible from these toolbars in the exercises that follow.

The first exercise is to make a sketch of a handset as seen in this picture. For a design engineer, it is recommended that they observe and understand the model for some time and then jump into the software. It is essential to perceive how a product is going to be manufactured and then plan the design. The main end goal of CAD is manufacturability. Having this in mind, let's take a moment to understand the sketch. For a sketch, it has four parts. Outer frame, keypad holes, display screen cutout, and antenna.

So let's approach the sketch design with these steps. As seen in the slide, the outer frame consists of three rectangles. You may watch as I go through the exercise until the end and then practice or you may do it along with me. First, let me close this part and start afresh. From the start menu, I will click on the mechanical design option and then click on sketcher option. Let's name this part as handset. I am first going to save this file in a preferred location. You can see that the part type of this CATIA file is CATPART.

As discussed earlier, let's create a point from the reference elements toolbar with X, Y, Z coordinates as 0. Then, I can click on OK on the point definition window to complete this command. Now, I will click on the position sketch command from the sketcher toolbar. In the sketch positioning definition window, I will select positioned for planar support type from the drop-down list. From the specification tree, I will select X, Y plane for reference. I will pick projection point as origin type from the drop-down list and then select point 1 as reference from the specification tree.

I shall leave orientation type as implicit. Once I align V and H direction axis correctly by using these checkboxes, I can click on OK to exit the position sketch definition window. Now, from the profiles toolbar, second icon drop-down list, I will select the centered rectangle command. With the left mouse button, I can click on the center point of the coordinate system. Now, if I move the mouse pointer away from the center point and then left-click anywhere again, a rectangle is formed. The green H, V and perpendicular symbols say that the lines are horizontal or vertical with respect to the coordinate axis and perpendicular to each other respectively.

A centered rectangle also makes sure that both horizontal lines are of the same dimension and same goes with the vertical lines. The same definition does not apply to other predefined profiles in this toolbar list. Now, let's define the dimensions for this rectangle. In the constraint toolbar, I will select the constraint option, then select the bottom horizontal line of the rectangle and then click on the yellow horizontal axis that's named H. As you can see, a number pops up with arrows. Katia gives a dimension based on its spatial references.

We can adjust this reference value by double-clicking on the numerical value and editing it in the constraint definition window. Let's update the value to 40 mm. If I click on the reference option, the value box is grayed out and it suggests that this value is not editable as we proceed with the sketch design. Here, I will uncheck the reference option in the constraint definition window. Note that we can always go back to modify constraint definition by double-clicking on the dimension value in the graphics area. I will click on cancel to exit this window.

Next, from the constraints toolbar, I can select constraint, then select the vertical line on the right-hand side of the rectangle, and then the yellow vertical axis and update the numerical value to 30 mm. Please note that all dimensions are in mm. The units of the design can be changed in the options if required. Moving forward from the visualization toolbar at the bottom of the Katia window, we can see that a grid icon is orange in color, which means that grid option is active. If I click on this icon, the option is deactivated, and the grid vanishes from the graphics area.

Grid helps with positioning points on the sketch, so I will keep it active. The sixth icon in this toolbar shows dimensional constraints when it is activated. If I deactivate this option, we cannot see the dimensions on the sketch. The seventh icon shows geometrical constraints like parallel, perpendicular, etc. when activated. Let's test it out. Now, the fifth icon is called Diagnosis, which when activated, shows the sketch in green color, if it is fully constrained. Meaning, the sketch is well defined and it cannot move. If we deactivate this icon, the sketch turns white, and we don't know if it is fully constrained.

I will go ahead and activate this icon back on. While we are here, let's click on the icon that looks like a traffic signal on the tools toolbar. This option is very important in determining if the current sketch is fully defined, also known as ISO constrained. I can click on the magnifying glass on the sketch solving window to open the sketch analysis window. The diagnostic window lists all the constraints that are applied on the current sketch. If I click on the geometry window, it shows that the status of the profile is closed, which is an ideal situation.

Now, let's close this analysis window and do a small change to the sketch. I will click on the 30mm dimension value and press delete on the keyboard. The sketch color has now changed to partly white and partly green. Now, if we look at the sketch analysis, it shows that the sketch is under constrained, highlighting all the elements that need to be constrained. However, the geometry tab still shows that the profile is closed as all the corners are connected. This tells us that CATIA treats all the sketch elements as curves and points.

I will add the 30mm dimension back on to make the sketch fully constrained. Another thing to note here is, since this is a centered rectangle, it is sufficient to define only half of the length and breadth of the rectangle. The other half is assumed to be symmetrical to the first half. Drawing the inner rectangle can be done in a couple of ways. One is using the same rectangle option and another is to use a command called offset. The object we want to offset is the rectangle.

So, we need to select the rectangle. Since this is the only sketch element so far, if I click on the sketch 1 under geometrical set 1 from the specification tree on the left, the whole rectangle will highlight in orange color. Another way to do this is to select the lines from under the geometrical set 1. I will expand sketch 1, expand geometry, and then I can select lines 1, 2, 3, 4. Note that, if line 2 is clicked on the specification tree, it highlights in the graphics area, and vice versa.

When we are working on complex designs, there would be numerous geometries, and it is hard to locate a specific element in the specification tree. To easily locate the associated geometry in the graphics area, with that of the feature in the specification tree, we can use commands like reframe on and center graph. If I right-click on a line and then select reframe on, this will automatically highlight the sketch in which this line belongs to in the specification tree. If I right-click on a specific geometry feature in the graphics area, and click on the center graph command, the corresponding sketch element will be displayed in the center of specification tree.

Moving forward, I can select all four lines of the rectangle by using the left mouse button and holding the control key. Then, on the operation toolbar, in the transformation tree, I will click on the Offset icon. A blue-colored dotted rectangle is created whose size varies as I move the mouse in and out of the existing rectangle. I will move the mouse pointer towards the inside of the existing rectangle. Since we want a smaller rectangle, there is a new position window on the top in which we can define the offset distance. We could write the offset value in the offset box and hit the Enter button on the keyboard.

Or we could click inside the first rectangle to exit the offset command. The dimension can be moved by picking the numerical value with the mouse left click. And the dimensional arrow line can be moved by picking the dimensional line. Next, I will click on the Automatic Dimensional Constraints icon on the Sketch Tools toolbar. I will explain why I did this shortly. To draw the third rectangle, I click on the Profiles toolbar, Pre-Define Profiles drop-down list. Then, the Centered Rectangle command. I will now draw the rectangle at an approximate position inside the outer frame and below the coordinate axis as shown in the picture.

Now, I constrain this rectangle by applying the dimensions. Note that, unlike earlier, the dimensions appeared automatically this time. This is because the Automatic Dimensional Constraints option is active. I can now double-click on the horizontal dimension of the rectangle and modify the numerical value to 40 mm and then modify the vertical dimension to show 30 mm. Did you observe that the sketch is not fully constrained? If I click anywhere on the rectangle and move the mouse, the only possible movement of the sketch is up and down.

This movement needs to be arrested to make this rectangle fully constrained. To do this, I can click on the Constraint command, then click on the center point of the rectangle, and then click on the yellow horizontal central axis to define the distance from the center. Let's update the numerical value to 20 mm. Now, the sketch is fully constrained. If part of the sketch is not visible, how do we see the entire sketch? From the View toolbar, I can click on the Fit All in command to see the entire sketch.

If you are actually sp wyposaure, you have to try the left and take the same route... If I made it so, let's at you.