Tutor For Mechanical Softwares

Creating Lines in Catiav5

noreply@blogger.com (Navin) — Mon, 14 Apr 2008 11:35:00 +0000

Creating Lines

Path:
Insert | Profile | Line | Line
Insert | Profile | Line | Infinite Line
Insert | Profile | Line | Bi-Tangent Line
Insert | Profile | Line | Bisecting Line
Insert | Profile | Line | Line Normal to Curve
Located in a fly-out on the Profile toolbar.

Use this to ...
• Create lines in a sketch.

Prerequisites
• The Sketcher workbench must be active.
• The Sketch tools toolbar must be visible, and Dimensional and Geometrical Constraints active.
• All SmartPick options must be active.

Process: Creating a Line Using Coordinates

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, pick the start point.
Or
On the Sketch tools toolbar, enter the H and V values for the start point and press TAB.
The text boxes change, allowing you to define the endpoint of the line.
3. In the Graphics window, pick the endpoint.
Or
On the Sketch tools toolbar, enter the H and V values for the endpoint and press TAB.
CATIA creates the line and adds dimensions from the sketch origin if you specify an H and V value.

Process: Creating a Line from Endpoints

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, pick the start location of the line by picking an existing endpoint. CATIA displays a preview of the line as you move the mouse.
3. Pick the end location of the line by picking an existing endpoint. CATIA creates the line.

Process: Creating a Line from the Midpoint of a Line

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, move the cursor over the line that contains the midpoint.

3. Right-click and select Midpoint from the pop-up menu. CATIA creates the first endpoint of the line and displays a preview.
4. Pick the endpoint of the line to create it.

Process: Creating a Parallel Line

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, pick the start point of the line.
3. Move the cursor over the line that you want to be parallel. CATIA highlights the line.
4. Right-click and select Parallel from the pop-up menu. CATIA locks the previewed line parallel to the line you select.
5. Pick the endpoint of the line.

Process: Creating a Perpendicular Line

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, pick the start point of the line. CATIA displays a preview of the line as you move the mouse.
3. Move the cursor over the line that you want to be perpendicular. CATIA highlights the line.
4. Right-click and select Perpendicular from the pop-up menu. CATIA locks the previewed line perpendicular to the line you select.
5. Pick the endpoint of the line.

Process: Creating Infinite Lines

1. Select Insert | Profile | Line | Infinite Line.
2. On the Sketch Tools toolbar, click either Horizontal Line or Vertical Line.
3. In the Graphics window, pick the point that the line passes through.
Or
On the Sketch tools toolbar, enter the H and V values for the point that the line passes through and press TAB.

CATIA creates the infinite line.

Process: Creating a Bi-Tangent Line

1. Select Insert | Profile | Line | Bi-Tangent Line.
2. In the Graphics window, pick the geometry that contains the first tangent point.
3. Pick the geometry that contains the second tangent point to create the line.

Process: Creating a Bisecting Line
1. Select Insert | Profile | Line | Bisecting Line.
2. In the Graphics window, pick the first line that you want to bisect.
3. Pick the second line that you want to bisect. CATIA creates an infinite line.

Process: Creating a Line Normal to a Curve

1. Select Insert | Profile | Line | Line Normal to Curve.
2. In the Graphics window, pick a point in space to define the first endpoint of the line.

3. Pick the curve that the new line will be normal to.

4. CATIA creates the line and a Perpendicular constraint.

Options
Infinite Line
Creates an infinite line in space. The three options available on the Sketch tools toolbar are Horizontal, Vertical, and Line through Two Points.

Horizontal Line
Creates an infinite horizontal line.
Vertical Line
Creates an infinite vertical line.
Infinite Line Through Two Points
Creates an infinite line through two points. This command is similar to the standard line creation.
Line Normal to Curve
Creates a line perpendicular to a selected curve.

Select a Curve Before
Reverses the selection order. This is located on the Sketch tools toolbar. Pick the curve first, then the opposite endpoint.

Tips
• Use SmartPicks to increase productivity.
• Look at the geometric symbols that appear when constructing geometry. By reviewing these symbols, you will know if you are creating unwanted geometric constraints.
• Hold SHIFT to deactivate SmartPick when creating geometry.
• Double-click the icon to use the same command continuously.

Creating Points

noreply@blogger.com (Navin) — Wed, 19 Mar 2008 10:25:00 +0000

Creating Points

Path:
Insert | Profile | Point | Point
Insert | Profile | Point | Point...
Insert | Profile | Point | Equidistant Points
Insert | Profile | Point | Intersection Point
Insert | Profile | Point | Projection Point

Located in a fly-out on the Profile toolbar.

Use this to ...
• Create points.
• Create equidistant points.
• Create intersection points.
• Create projection points.

Prerequisites
• You should be in the Sketcher workbench.
• The Sketch tools toolbar must be visible, and Dimensional and Geometrical constraints active.
• All SmartPick options must be active.

Process: Creating a Point by Clicking
1. Select Insert | Profile | Point | Point.
2. In the Graphics window, pick the point.
Or
On the Sketch tools toolbar, enter the H and V values for the point and press TAB. CATIA creates the point and its associated dimensions if specified using the toolbar.

Process: Creating Points Using Coordinates
1. Select Insert | Profile | Point | Point… The Point Definition dialog displays.

2. Click Cartesian or Polar.
3. Enter the coordinates of the point.
4. Click OK to create the point and its associated dimensions.

Process: Creating Equidistant Points – Points and Length

1. Select Insert | Profile | Point | Equidistant Points.

2. In the Graphics window, pick the geometry on which you want to create equidistant points. The Equidistant Point Definition dialog displays.
3. In the New Points text box, enter the number of points.

4. Click OK to create the points.

Process: Creating Equidistant Points – Points and Spacing

1. Select Insert | Profile | Point | Equidistant Points.

2. In the Graphics window, pick the geometry on which you want to create equidistant points. The Equidistant Point Definition dialog displays.

3. Pick the origin point. The Equidistant Points Definition dialog text boxes become selectable.
4. In the New Points text box, enter the number of points.

5. In the Spacing text box, enter the spacing.
6. Click OK to create the points.

Process: Creating Equidistant Points – Spacing and Length

1. Select Insert | Profile | Point | Equidistant Points.

2. In the Graphics window, pick the geometry on which you want to create equidistant points. The Equidistant Points Definition dialog displays.
3. Pick the origin point. The Equidistant Points Definition dialog text boxes become active.

4. In the Parameter list, select Spacing and Length.

5. In the Spacing text box, enter the spacing.

6. In the Length text box, enter the length.
7. Click OK to create the points and dimensions.

Process: Creating Intersection Points

1. Select Insert | Profile | Point | Intersection Point.
2. In the Graphics window, pick the first element to intersect.
3. Pick the second element to intersect. CATIA creates the intersection point and geometric constraints.

Process: Creating Projection Points

1. In the Graphics window, pick the points for projection.
2. Select Insert | Profile | Point | Projection Point.
3. Pick the element for the points to project onto. CATIA creates the points and geometric constraints.

Options

Point Definition Using Cartesian Coordinates

Allows you to specify the point location using Cartesian coordinates. Cartesian coordinates define a point by specifying the horizontal and vertical position relative to a datum.

Point Definition Using Polar Coordinates

Allows you to specify the point location using Polar coordinates. Polar coordinates define a point by specifying a radius and an angle that the point lies on relative to a datum.

Equidistant Points – Parameters
Specifies how to create the specified points.

Points and Length
Creates a number of equidistant points along a specified length. This option is the default when the Equidistant Points Definition dialog displays.

Points and Spacing
Creates a number of points along a specified spacing. This option is only available after you pick a start point.

Spacing and Length
Creates a number of points along a specified spacing and length. This option is only available after you pick a start point.
Projection Point
When this option is active, two projection methods are available on the Sketch tools toolbar.

Orthogonal Projection
Projects the point in a direction that is perpendicular to the target curve object.
Along a Direction
Projects the point in a direction that you specify by entering H, V, and Angle data.

Frequently Asked Questions

noreply@blogger.com (Navin) — Wed, 19 Mar 2008 06:05:00 +0000

1. Can I modify the sketch directions and origin?
A: Yes, you can modify all the sketch definitions by picking the sketch in the Specification Tree and selecting Edit Change Sketch Support, or right-click to display the pop-up menu.

Sketch Tools Toolbar The Sketch tools toolbar (select View | Toolbars | Sketch tools) is invaluable when creating sketch geometry.
Click Here to Download Sketch Tools Movie

The toolbar enables you to automatically create constraints, and it changes to display the coordinates, lengths, and other information in the context of command you are using. The Sketch tools toolbar also provides feedback as you dynamically move the cursor in the Graphics window, showing you the current length of a line or the diameter of the circle. This information is helpful because sketches are much easier to constrain when the initial geometry is drawn close to the desired size. Additionally, toolbar functions allow you to snap the curves to a grid and create construction geometry. The Sketch tools toolbar has several distinct areas. The first section contains: Grid, Snap to Point, Construction/Standard Element, and Geometrical and Dimensional Constraints. These first five commands are always present and are the same, regardless of the active sketch command. The next section contains options that vary, depending on what geometry you are creating or what command you are using to modify your existing geometry. For example, when creating a line, the Sketch tools toolbar displays several different text boxes. Initially, the toolbar allows you to specify the H (horizontal) and V (vertical) start coordinates. Then the toolbar changes to display the end coordinates. The length of the line and the angle text boxes display at all times while the line command is active. The Sketch tools toolbar for creating a sketch chamfer has options for how to trim the selections. After you select the geometry, the toolbar displays text boxes for the offset(s) and/or the angle. You can simply click in the text boxes and enter the values or press TAB to cycle to the next text box. When you finish an entry, press TAB to accept the value. After specifying all the values for a particular geometric parameter, like an endpoint, CATIA modifies the text boxes in the toolbar, allowing you to enter the next piece of geometric information. The advantage in using the Sketch tools toolbar, instead of picking in the Graphics window, is that dimensional constraints are applied automatically to the geometry. Grid This option creates a visual grid on which you create sketches. Turn this option on by clicking Grid on the Sketch tools toolbar. Other grid options are set under Tools | Options. Snap to Point Locates curve endpoints onto the grid points.
Click Here to Download Grid Option Movie

Construction/Standard Element Creates sketch geometry using any of the creation modes described below. This geometry is used to create solids and surfaces. When the icon is active (highlighted), any new geometry is created as construction geometry. Construction geometry is gray by default, has a dashed line type, and does not display outside the Sketcher workbench. You can convert from standard to construction elements and vice versa by selecting existing curves and then changing the status of the Construction/Standard Element icon. Geometrical Constraints Creates automatic geometric constraints in conjunction with SmartPick when creating geometry. When deactivated, geometric constraints are only applied at the time of creation. After you draw curves, CATIA does not save the constraints. It is very likely that that this will be active all of the time. Dimensional Constraints Creates automatic dimensional constraints when entering values in the Sketch tools toolbar to create exact geometry. It is very likely that that this will be active all the time. Tips • Roughly create the profile you need. Then use dimensional and geometrical constraints to finalize the profile. • When creating a continuous profile, you can activate the Tangent Arc command by clicking and dragging the cursor away from the endpoint of the line. Release to activate the Tangent Arc command.

Creating Sketches

noreply@blogger.com (Navin) — Mon, 17 Mar 2008 08:49:00 +0000

Creating Sketches
Path: Insert Sketcher SketchInsert Sketcher Positioned Sketch
Located on the Sketcher toolbar.

Use this to ...
Create a new sketch.

Key Points
In CATIA, there are two ways to create a sketch: Sliding (also known as a Non-positioned sketch) and Positioned. In a sliding sketch, you do not have control over the origin or orientation. This can lead to potential errors in your model, such as, if base sketches update, later sketches can become out of place. It is good modeling practice that all the sketches you create are positioned sketches. However, you can update a non-positioned sketch to a positioned sketch.

Process: Creating a Sliding Sketch (Non-positioned Sketch)

1. Select Insert Sketcher Sketch. CATIA prompts you to pick a face or plane.
2. In the Graphics window, pick the sketch placement face to activate the Sketcher workbench.
3. On the Workbench toolbar, click Exit Workbench to return to the modeling application.

Process: Creating a Positioned Sketch
Click Here to Download Positioned Sketch Movie

1. Select Insert Sketcher Positioned Sketch. The Sketch Positioning dialog displays.
2. In the Graphics window, pick a placement face. CATIA projects the sketch origin onto the selected plane or face origin.
3. In the Origin Type list, select the origin definition method.
In the Graphics window, pick the geometry to define the origin.
4. In the Orientation Type list, select the orientation method options. In the Graphics window, pick the geometry to define the orientation.
5. Click OK to create the sketch.
6. On the Workbench toolbar, click Exit Workbench to return to the modeling application.

Options
Sketch Positioning
Defines the two options for creating a sketch.
Positioned Defines the sketch by selecting a planar face or plane, or by defining two axes. A positioned sketch allows you to define the origin and the reference direction. Using existing edges as references for the sketch direction means the directions update if you modify the underlying edges. Using a positioned sketch is the recommended method of creating a sketch.
Sliding Creates a non-positioned sketch. The default origin and directions of the selected plane or face define the origin and direction of the sketch. Sliding sketches can be updated to positioned sketches by selecting new reference directions.

Origin

Click Here to Download Sketch Origin Movie

These options define the methods to position the origin of the sketch.
Implicit Defines the origin as the default origin of the face or plane. Selecting two lines places the origin at the intersection of the two lines. The H direction is collinear with the first line; the second line only defines the side on which the V direction is created, not the orientation.
Part Origin Defines the sketch origin as the absolute origin of the part.
Projection Point Defines an origin by projecting a point onto the sketch positioning face or plane.
Intersection 2 Lines Defines the origin at the intersection of two lines.
Curve Intersection Defines the origin at the intersection of two curves.
Middle Point Defines the origin at the mid-point of a line or edge.
Barycenter Defines the origin at the center of a face.

Orientation

Click Here to Download Sketch Orientation Movie

Defines the H and V directions of the sketch. When defining the direction, you can control either the H or V direction. You also have the ability to reverse the direction.
Implicit Defines the sketch directions as the default directions of the sketch support.
X Axis Defines the active direction along the X-axis.
Y Axis Defines the active direction along the Y-axis.
Z Axis Defines the active direction along the Z-axis.
Components Defines the active direction by entering vector components.
Through Point Defines the active direction as the vector through a point.
Parallel to Line Defines the active direction as parallel to a selected line.
Intersection Plane Defines the active direction as the line created by the intersection of two planes.
H Direction Lets you define the H direction of the sketch.
V Direction Lets you define the V direction of the sketch.
Reverse H Reverses the H vector.
Reverse V Reverses the V vector.
Swap Swaps the H and V directions.

Sketch Design

noreply@blogger.com (Navin) — Mon, 17 Mar 2008 05:06:00 +0000

Sketcher Overview

Click here to download Sketcher Introduction Movie
Overview: Sketcher enables you to create parametric, planar geometry on faces and planes. After you draw the geometry, you use the sketch to create pads, pockets, shafts, and surface geometry.

Sketches
Sketches are sets of 2D, fully-parametric curves. In a typical sketch, you first create base curves, and then add geometric and dimensional constraints to control the size and shape of the curves. By adding these constraints to the sketch curves, you can capture and define your design intent. This approach makes it much easier to modify the sketch shape later.

Sketch Usage
Sketches are commonly used to define section curves for pads, pockets, shafts, grooves, or surface geometry. Sketches maintain associativity to their parent and child features. If you change the geometry in a sketch, the solid model changes accordingly. Similarly, if a plane or face changes orientation or moves, any sketches attached to that plane or face move with it. You can also add dimensional and geometric constraints to the sketch. Using dimensional constraints, you can create system-defined expressions and link them to other sketch dimensions or to other features of the solid.Using Sketcher intelligently allows you to quickly modify the model to reflect changes during the product life cycle.

Sketch Placement
You create sketches on a plane or solid planar face. A sketch remains associative to its placement face. If the face changes orientation or location, the sketch changes with it.When you pick a plane or face as the sketch plane, CATIA sets the horizontal and vertical directions as the main axis of the selected plane. You can manually control the horizontal and vertical directions by selecting the horizontal and vertical reference edges, and the placement face, before creating the sketch.

Sketch Management
Organizing the data within a CAD file is always important when different people are potentially going to use the data. Data organization is especially important when using sketches because you can define sketch information in many geometrical sets, with different sketch names. Depending on the complexity of a design, even a simple, single solid model can contain over 20 sketches. With this amount of data, it is prudent to use good techniques to manage your sketches.CATIA automatically makes a sketch invisible once you use it to create a feature, such as a pad or pocket. However, it is a good practice to place each sketch into a geometric set. This makes it easier to find the information required in the Graphics window. It is also advantageous to give each sketch a descriptive name by editing the properties of the sketch.

Tips
· Always assign the In Work object to the appropriate geometrical set before creating a sketch. Although you can move objects, it may be easier to initially create objects in the correct location.

Method For Extending A Sketch Profile Into A solid In CatiaV5

noreply@blogger.com (Navin) — Sat, 15 Mar 2008 08:37:00 +0000

Options
Type
Defines the method for extending the sketch profile into a solid.

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Dimension
Creates a pad at a set length.

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If the model updates, the pad always remains at the specified dimension value.
Up to Next
Creates a pad to the next face that encloses the pad profile. With this option, if the limiting face moves, the pad height updates to the new

limiting face location.

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Up to Last
Creates a pad to the last face that encloses the pad profile in the model. The pad height is parametric, which means if the position of the

limiting face moves, then the pad updates to reflect the change.

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Up to Plane
Creates a pad to a selected plane.

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You can pick both reference planes and existing faces. The advantage of this option is that the selected face does not have to enclose the

pad profile for the pad to stop.

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By moving the selected plane or selecting a new plane, the pad updates to reflect the change.

SmartPick for sketch in CATIAV5

noreply@blogger.com (Navin) — Fri, 14 Mar 2008 08:15:00 +0000

Overview: As you work with the sketcher there are several onscreen hints that you will want to look for as you define your profile. This feedback will come from a tool called SmartPick. SmartPick will help you to reduce the design time involved in creating sketches.

SmartPick Coincidents
SmartPick allows you to pick endpoints, arc centers, midpoints, intersections, and other control points. Catia will display different symbols next to your cursor as you create sketch geometry. The symbol displayed will help you determine if you have the proper coincident constraint, (profile connections).

The symbols displayed in the Graphics window show what coincident constraints will be created on the geometry. In the following graphic, figure 1 shows a coincident endpoint connection. Figure 4 shows a coincident connection to the arc center of the circle. Figure 3 shows a coincident connection to the midpoint of the highlighted element. Point connections have a filled symbol. Figures 2 and 5 show a coincident connection to the element highlighted. Element connections show an open symbol.

SmartPick Alignments

SmartPick can also help you to identify when you are in an alignment with other elements near your cursor. Catia displays alignments using a thin dashed line. Sometimes the line may appear to be continuous because of the way the workstation renders the image.

SmartPick Geometric Relationships/Constraints
SmartPick can also help you to define geometric relationships between elements. These include parallelism, perpendicularity, and tangency.

In the following graphic, the first figure shows only an alignment. Figure 2 shows that the line is also horizontal, (parallel to the horizontal axis of the sketch). The horizontal orientation is indicated by SmartPick with the change in color, (the default is blue). Both horizontal and vertical use a change in color to indicate the proper orientation.

The next graphic shows the parallel and perpendicular relationships. Notice that the relationship is defined relative to the highlighted element. The relationship symbols displayed in the Graphics window correspond to the constraint symbol.

The creation of constraints is dependant on Geometrical Constraints being active on the Sketch Tools toolbar; however, the relationship with other geometry will still be recognized by SmartPick even if Geometrical Constraints is not active, but no constraint will be created.

The following symbols display on the geometry after creation to show what geometric constraints exist.

The following graphic shows the completed profile with the geometric constraint symbols displayed.

SmartPick Options

SmartPick recognition settings are available from Tools | Options, Mechanical Design, Sketcher, SmartPick.

Tips
• To temporarily deactivate SmartPick, hold SHIFT.
• To lock a displayed relationship or alignment, hold CTRL after the symbol displays. You can now move your mouse and maintain the relationship.

Options - Sketcher In CATIAV5

noreply@blogger.com (Navin) — Thu, 13 Mar 2008 07:44:00 +0000

Overview: The Options dialog is where you set various sketch options, such as, Grid, Sketch Plane, Geometry, Constraint, and Colors. All these options are available by selecting Tools | Options, Mechanical Design, Sketcher.

Grid

Controls the virtual grid that displays on the sketch plane. You can use the grid as a reference when creating geometry.

Activate Snap to point to restrict the cursor movement to the grid intersections. Specify the horizontal distance between grid lines by entering values in the Primary spacing text box and specify the spacing between each grid line in the Graduations text box. To specify different vertical grid lines activate Allow Distortions.

Sketch Plane

Allows you to shade the plane that the sketch lies on and to orientate the sketch plane parallel to the screen. Both of these options help you see where the sketch lies in space and aids in the construction of the geometry.
The Visualization of the cursor coordinates option displays the cursor coordinates during element creation.

Geometry

Lets you control whether or not arc centers are created when sketching circles, arcs, and ellipses or whether or not to dynamically drag elements. Deactivate Create circle and ellipse centers to disable center point creation. Activate Allow direct manipulation to dynamically drag elements.

Click Solving Mode to display manipulation options when dragging elements.

Standard mode drags as many elements that are connected as possible while keeping the constraints. Minimum move drags as few elements that are connected as possible. Relaxation looks for the minimal way an element can be modified and carries out that change. Drag Elements end points included allows you to drag the end points of lines and arcs.

Constraint

Enables you set automatic geometric and dimensional constraints. Activating Creates the geometrical constraints automatically creates geometric constraints between sketch geometry. When activated, CATIA applies the geometric constraints while you create the sketch. Activate Creates the dimensional constraints to automatically add dimensional constraints when creating geometry using the Tools toolbar. SmartPick allows you to pick on end points, arc centers, midpoints, intersections, and other control points. SmartPick also sets geometric constraints between elements, including parallelism, perpendicularity, and tangency.

The following symbols display in the Graphics window to show which geometric constraints exist on the geometry. To deactivate SmartPick temporarily while drawing, hold the SHIFT key.

Colors

Defines all the color options for Sketcher. Default color of the elements sets the color of the geometry created in Sketcher. Visualization of diagnosis sets the colors for the constrained and under-constrained elements. Other color of the elements sets the colors of the remaining features in Sketcher.

Techniques For Curve Creation

noreply@blogger.com (Navin) — Wed, 12 Mar 2008 09:12:00 +0000

Curve Creation Techniques

Overview: When you create sketch geometry, there are different methods that you can use to define the shape, size, and position of the curves.
Clicking in the Graphics Window Versus Entering Values on the Sketch Tools Toolbar
The two methods of creating curve geometry include picking in the Graphics window and applying the constraints separately, or to using the Sketch tools toolbar to enter specific data.
The advantage in using the Graphics window is that you can quickly create the rough profile and then use the exact constraints that you need to finalize the geometry. The disadvantage is that there are more open degrees of freedom to constrain, initially making curves more difficult to control.
As you become more comfortable with constraints, creating curves on-the-fly is the fastest and easiest method for defining a profile with the proper design intent, especially when used in conjunction with SmartPicks and active Geometrical Constraints.
The advantage in using the toolbar method is that the constraints can be applied at the time of creation, (if Dimensional Constraints is active on the Sketch tools toolbar). The disadvantage is that many of the automatic dimensional constraints may not properly define your design intent, such that you will have to delete and recreate, or redefine the constraint.
Entering a value in the Sketch tools toolbar locks that value, allowing you to either pick in the Graphics window to define the rest of the geometry or use the toolbar to enter the rest of the definition. Using a combination of methods allows you to use defined values, while still having the flexibility of picking in the Graphics window.
Pay close attention to what you are entering in the Sketch tools toolbar. Remember that the Sketch tools toolbar asks for different information, depending on what curves you are creating, and changes as you progress through the definition. In other words, after entering data, the toolbar changes and then looks for the next set of values. Use TAB to move between text boxes in the toolbar. TAB stores the entered value in the toolbar and makes the next text box active. Pressing ENTER only stores the entered value.

Pop-up Menu During Curve Creation

The pop-up menu is also an invaluable tool when constructing geometry. Right-clicking another element when creating geometry displays the pop-up menu.

Depending on your selections, the pop-up menu changes, allowing you to create geometric constraints between the two elements. For lines, the pop-up menu allows you to apply parallel and perpendicular constraints. Right-clicking a circle or arc during line creation allows you to apply tangency constraints.
Right-clicking geometry also allows you to copy the geometric properties of the curve, such as length and radii.

Right-clicking a dimensional constraint allows you to copy the constraint value and paste it into another constraint.

Tips
• Use a horizontal or vertical constraint instead of specifying an angle of 0, 90, 180, or 270 degrees.

Sketch Chamfer in CatiaV5

noreply@blogger.com (Navin) — Tue, 11 Mar 2008 08:27:00 +0000

Process: Creating a Sketch Chamfer
1. Select Insert Operation Chamfer.
2. On the Sketch Tools toolbar, select the trimming option.

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3. In the Graphics window, pick the first line.
4. Pick the second line.
5. On the Sketch Tools toolbar, select the Chamfer option.

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6. Move the cursor to the required quadrant.
7. Pick a point on the chamfer.
Or
On the Sketch Tools toolbar, enter the parameters and press TAB.
CATIA creates the chamfer and its dimensions.
Options
Trimming Options
Depending on which option you select in the Sketch Tools toolbar, CATIA trims the chamfer or corner differently.

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Trim All Elements
Trims all the elements.
Trim First Element
Trims only the first elements.
No Trim
Specifies that no elements are trimmed.
Standard Line Trim
Trims the elements to the corner, using the standard line element.
Construction line trim
Trims the elements to the corner using the construction line element.
Construction Line No Trim
Specifies that elements are not trimmed, but only changed into construction line elements.

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Chamfer Options
Allows you to specify which Chamfer option you want to use.

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(In the original release, the GA release of R12, dimensions are sometimes not created for chamfers.)

Angle and Hypotenuse
Specifies angle and chamfer hypotenuse.
First and Second Lengths
Specifies first and second chamfer lengths.
First Length and Angle
Specifies first chamfer length and chamfer angle.

Tips
• You can create multiple corners by holding CTRL and selecting multiple corner points of a profile before selecting the Corner command. This technique requires you to enter a radius.

Constraint Colors For Catia V5

noreply@blogger.com (Navin) — Mon, 10 Mar 2008 09:44:00 +0000

Constraint Colors
To help you constrain geometry, CATIA applies different colors to the curves, depending on the dimensions and constraints you apply to them. The following table outlines the colors used.

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Gray elements are construction elements that help you create sketch curves. Sketch curves are used for solid and surface-based features.

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Yellow elements are non-modifiable elements. The solid model usually controls the size and shape of these elements. They are created when you intersect or project edges or faces onto the sketch plane.

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White elements are under-constrained. Under-constrained elements are curves not controlled by CATIA parameters. You can simply drag these elements to a new size and location.

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Green elements are fully constrained elements; CATIA parameters control the position and size. To modify the elements, you must change the controlling dimension. The profile is fully-constrained when the entire closed profile displays in green.

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Brown elements are ones you cannot change. Elements in the sketch are inconsistent or over-defined and the geometry cannot be updated. Often, you will see this color on a dimension when you attempt to place it on a yellow element.

Purple elements are over-constrained. There are too many dimensions controlling their shape and position. This is not a desirable color to see in your sketches. The sketch no longer responds to changes to dimensions. You need to resolve the constraints that are causing the conflict.

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Red elements are inconsistent; the resulting shape from the dimensional values are not possible. Just as with purple, red is not desirable in your sketches.

Orange continues to mean that the object is selected.

Tips
• You do not have to fully-constrain a sketch, but it is good practice not to leave many open degrees of freedom. Some companies require sketches to be fully-constrained before releasing a part.
• When you see a purple or red element after you have placed the constraint, you may consider undoing the operation and changing the way you place the constraint.
• Be aware that when you are placing dimensions between two elements, CATIA may temporarily change the color to indicate over-constrained when you pick the first element. Select the second element and the color should restore to green.

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Sketch Practices For Catia V5

noreply@blogger.com (Navin) — Mon, 10 Mar 2008 04:26:00 +0000

Sketcher Best Practices

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Overview: As you may have experienced, successfully constraining sketches can sometimes be an art form. The key is

to place the dimensions and geometric constraints in such a way that they adequately capture your design intent. Most likely, you will

develop your own set of best practices as you gain experience with the Sketcher workbench. In the meantime, below you will find some

suggestions that make constraining sketches easier.

General Suggestions
In general, geometric constraints control the shape, orientation, and function of sketch curves. For this reason, it is a good

modeling practice to apply geometric constraints first. This step is especially true for horizontal and vertical geometry, or parallel and

perpendicular geometry. For instance, angles are sometimes created when lines are not parallel, rather than the desired distance dimension.

In this case, proper tangency positioning is important, because arcs will not stay aligned without the constraint present.

The second step is to add dimensional constraints after you add the base geometric constraints. Dimensional constraints help control the size

and location of the sketched profile. Designers add dimensional constraints in various ways; it usually comes down to personal preference.

Some individuals start with angular and radial dimensions, and then create length and offset dimensions, others move around constraining

important areas first, while others add constraints in a clockwise or counterclockwise progression.

As you add dimensions, pay attention to the way remaining geometry reacts when you change a value. Fix missing geometric constraints as

necessary. For example, if you see that a line changes from its horizontal position, repair it before attempting to add a dimension relative

to it.

Inferred Constraints
Automatically creating geometric and dimensional constraints can be helpful, but be careful of unnecessary constraints, particularly

coincident constraints, which can lock arc centers in position or constrain two lines in a collinear alignment. Looking for the dotted lines

of a coincident constraint at a distance can help you to resolve many over-constrained and conflicting constraint situations.

Remember, you can press SHIFT to suppress automatic constraints temporarily and you can use the SmartPick tool to help create the profile.

Testing Sketches
Use Select to drag under-constrained elements in the Graphics window to interrogate the profile for the open degrees of freedom.

Remember, an element in green may not be fully constrained. You can also determine how the rest of the profile will react given the current

constraints.

Sketch Analysis, another tool to consider using, determines whether extraneous geometry exists in the sketch, and if the sketch is closed.

See Sketch Operations, Sketch Analysis for more detail on Sketch Analysis.

Drawn Profile Size Versus Real Size
Several Options exist that you let you adjust your initial sketch when it is too big or too small. You can:

1. Redraw the profile (a time intensive solution).

2. Use Select to move the elements closer to their final position (a good solution only when some elements are incorrectly scaled).

3. Scale the entire profile (great solution if your entire profile is out of scale). Sometimes it is also helpful to create all the

dimensional constraints before going back and editing them to their final size. See Transformation for more detail.

Pay attention to the Sketch Tools toolbar when creating the first few elements in your sketch. Make sure those first elements are relatively

close, plus or minus 15% of the final size. You can decide the placement and size of the remaining elements based on these 'known' elements,

which becomes especially effective when the initial elements are some of the larger elements in the sketch.

Sketch Complexity
The 'keep it simple' rule definitely applies when creating sketch profiles. It is not necessary to add all the details to one sketch,

and you can use multiple sketches and solid features to create your final part. Using simple profiles in your sketch makes constraints easier

to use. To do so, you leverage the stable geometry in the first sketch to help constrain the later sketches.

Leave out unnecessary details that can be applied externally as solid features, such as sketch corners (fillets) and sketch chamfers. Add

sketch corners only when they help capture design intent, such as a tangent distance dimension relative to other geometry.

Construction Geometry
While keeping simplistic profiles can be helpful, we encourage you to use extra geometry to help constrain the sketch. For example,

if two arc centers are required to have a horizontal alignment, add a construction line between the two center points to constrain them. This

horizontal constraint on the construction line keeps the arc centers vertically constrained.

Remember, you can create points along a curve you can use when dimensioning and constraining. You can also constrain other curves to these

points for location control.

TYPES OF CONSTRAINTS

noreply@blogger.com (Navin) — Sat, 08 Mar 2008 09:44:00 +0000

Distance
Creates a distance dimension between elements.

See Full-Size Image
Length
Creates a length dimension on an element.

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Angle
Creates an angular dimension between two linear elements

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Radius/Diameter
Creates a radius dimension on an arc and a diameter on a circle.

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Semimajor Axis
Creates a semi-major dimension on an ellipse.

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Semiminor Axis
Creates a semi-minor dimension on an ellipse.
Symmetry
Creates symmetric geometry about a reference line or axis. The first two elements selected must be the symmetric geometry. The third object is the symmetry line.

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Midpoint
Creates a midpoint constraint between a point and a line.

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Equidistant Point
Sets two points to be the same distance from a reference point. The reference point is the last point selected.

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Fix
Fixes the element at its current point in space.
Coincidence
Makes two points coincident.

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If you select two lines, CATIA makes them collinear. If you select two arcs, CATIA makes them concentric and equal in radius.
Concentricity
Makes two arcs or circles concentric.

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Tangency
Creates a tangency constraint between two curves or a curve and a line.

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Parallelism
Sets two lines parallel to each other.

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Perpendicular
Sets two lines perpendicular to each other.

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Horizontal
Sets a line to be horizontal.

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The horizontal direction depends on the H axis of the sketch.
Vertical
Sets a line to be vertical.
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The vertical direction depends on the V axis of the sketch.
Tips
• You can double-click a constraint icon to make the command automatically repeat. Select another command, like Select, to stop.
• Use SmartPicks when creating geometry to save you from having to explicitly specify the constraints.
• You can activate as many constraints as necessary on the Constraint Definition dialog at one time. As you select the constraint type the geometry updates in the Graphics window. If the constraint is not correct, you can deactivate it, but the geometry will not return to its previous location unless you cancel the dialog

Basic Sketch-Based Features

noreply@blogger.com (Navin) — Fri, 07 Mar 2008 12:08:00 +0000

See Full-Size ImageOverview: Sketch-based features are fundamental in creating solid models. The basic features include pads, pockets, shafts, and grooves, with all the options working in a similar manner. You select the sketch, which contains the required profile, and then you specify the limits of the feature. In general, pads and shafts are created material and pockets and grooves are removed material.Pads and Pockets Pad and Pocket are similar commands. The main difference is that Pad creates material while Pocket removes material.The pad and pocket dialogs are divided into the same sections, First Limit, Second Limit, Profile and Direction.
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See Full-Size ImageThe First and Second Limits specify the height and depth of the pad and pocket, respectively. Access Second Limit and the Direction options by clicking More>>. You can enter a height or depth value or specify a limiting plane or surface.
See Full-Size ImageThe advantage of specifying a plane or surface is that as the model updates, the pad or pocket updates to reflect the changes.The Profile area allows you to select a profile to create a pad or pocket. You can use the Sketcher icon in the dialog to edit existing profiles or create a new sketch on a face or plane.
See Full-Size ImageYou can use both open and closed profiles for pads or pockets, but the existing geometry must be able to trim the resulting solid.The Direction option allows you to define the direction of the pad or pocket.
See Full-Size ImageThe default option is set to Normal to profile. Other options include Mirrored extent, Reverse Direction, and Reverse Side. Mirrored extent mirrors the pad or pocket about the sketch plane. Reverse Direction reverses the direction of the pad or pocket, while Reverse Side reverses the side that creates material. For pads, this option is only available for open profiles

Sketcher in CATIA

noreply@blogger.com (Navin) — Fri, 07 Mar 2008 09:04:00 +0000

Solving Inconsistent Elements
See Full-Size ImageOverview: Sketcher, the cornerstone of CATIA, is one of the most useful tools in CATIA. It allows you to quicklycreate parametric profiles to begin a part. Not only does it create the base profile for the model but also nearly all subsequent solidoperations are sketch based. In fact, CATIA is one of the most heavy sketch-based modelers around. Although Sketcher is a powerful tool,numerous times elements become inconsistent. This is usually due to someone creating elements out of scale or having conflicting dimensionsand geometry. Below are some strategies to solve some common problems.Auto Constraint Auto Constraint is one of the most useful tools in the Sketcher workbench. It allows you to quickly add both dimensional andgeometric constraints to sketch elements. Before you create the constraints make sure you think about what you want to constrain and whatreference elements you need. Blindly selecting all the elements and any reference element will create a mesh of meaningless dimensions.Instead, think about the design intent. Choose the elements that you need to control dimensionally and by which edge in the model, and thenapply the automatic constraints.Dragging Elements Since CATIA gears the Sketcher around the rapid creation of profiles, there are times that it is difficult to constrain a sketch. Youmight find that increasing the value of a dimensional constraint causes the sketch to become over constrained, or some of your sketch curvesreact to the change in an undesirable manner. A number of things can cause over constraints, but it is usually the designer creating a sketchout of scale. Dragging the sketch elements allows you to dynamically move the elements to position them so they are constrained correctly. Toallow direct dragging of elements select Tools Options, Mechanical Design, Sketcher and activate Allow directmanipulation in the Options dialog.Animate When you roughly create elements and then apply constraints one at a time, sometimes the sketch becomes inconsistent. This is due tocreating the elements out of scale and CATIA cannot resize the elements to the correct size without causing conflicts. Animate Constraintallows you to narrow down where the values in the sketch become inconsistent. When you narrow down the selection, modify the dimensioncausing the problem to the value at just below where the sketch becomes inconsistent and then modify the other dimensions in smallincrements. By doing it this way, you should be able to solve any inconsistent dimensions that appear.Scale If you cannot drag the elements into the correct position or use Animate to pinpoint the problem areas, use Scale to increase ordecrease the size of the elements. Deactivate Duplicate mode in the dialog to only move the elements...................

Advantages of Solid Modeling

noreply@blogger.com (Navin) — Fri, 07 Mar 2008 07:17:00 +0000

Solid Modeling Intentions

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Overview: Solid modeling is the process of creating and modifying solid objects. Each solid object has topology defining the surface area and volume of that object. Faces, edges, and vertices comprise the topology.

Advantages of Solid Modeling
One of the main advantages of solid modeling is the ability to analyze the model. You can calculate detailed mass properties, such as weight, volume, and moment of inertia, for a solid body. You can also perform structural or fluid flow analysis, such as that of plastic injection molded parts.

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Other advantages of solid modeling include:
- Creation of a 'virtual solid', geometrically identical to the actual part.
- Ability to rapidly create and change models.
- Powerful feature associativity and feature positioning.
- Greater ease in modifying designs.
- Drafting associativity with a solid model.
- Substantially improved design visualization.
- Mass properties information.
- Easy-to-create rapid-prototyping output.
- Evaluation of form, fit, and function.
- Associative manufacturing data.
- Using an assembly to design new components in the context of an entire product model.
- Checking interference between parts.

Design Intent
Design intent refers to the ability to capture geometric conditions, dimensional relationships, and relative positions between features on solid models.

Years ago, you did not have the ability to record the steps used in building a solid body. This process is known as explicit solid modeling. You create a solid body without capturing a history of the individual features used in its construction, which makes the process of modifying the solid body complex and time-consuming.

A CAD software application that can capture design intent is known as a 'parametric modeler'. CATIA has robust parametric modeling functions. The program also gives you a choice to add, or later remove, design intent. At the start of a design, you may not know what sort of design intent is necessary. By using parameters, positional constraints, instances, and feature editing, you can change or add design intent to the solid model.

Methods for Creating Pads

noreply@blogger.com (Navin) — Fri, 07 Mar 2008 05:40:00 +0000

Process: Creating Pads using Up to Plane
1. Select Insert Sketch-Based Features Pad. The Pad Definition dialog displays.
2. Pick the profile in the Graphics window.
Or
Select the sketch in the Specification Tree.
3. In the Type list, select Up to plane.

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4. In the Graphics window, pick the Limit. The picked feature displays in the Limit text box.

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5. In the Offset text box, enter a value.

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6. Click OK to create the pad.

To Create Pads in CATIA

noreply@blogger.com (Navin) — Thu, 06 Mar 2008 13:27:00 +0000

See Full-Size Image

4. In the Graphics window, pick the Limit. The picked feature displays in the Limit text box.

See Full-Size Image

5. In the Offset text box, enter a value.

See Full-Size Image

6. Click OK to create the pad.

Visual tutor for solid edge

noreply@blogger.com (Navin) — Thu, 06 Mar 2008 10:31:00 +0000

Modeling Philosophy Overview

Overview: Solid Modeling is the process of creating and modifying solid objects. Each solid has topology defining the surface area and volume of that object. A solid is comprised of faces, edges, and vertices, which define its topology.

Feature-Based Design

Solid Edge creates a model with a method called feature-based design. A feature is an option in Solid Edge that lets you create a shape and form it into a solid. There are many different types of features that add or remove material from the model. A feature-based solid model is a collection of several features. This process makes describing a model much easier because the model is broken down into several smaller features that are easier to define. The feature order describes the way the part is built and it shows the sequence that the model was constructed.

Variables

When a feature is created, there are a series of variables created as well. A Variable Table stores all the necessary dimensions that describe the various features in a solid model. Each variable or dimension can be modified to change the size of the associated feature.

Feature Editing (Parametric)

Imagine your model is nearly complete with all the required design elements in place. Due to a last-minute change, based on the results of a finite element analysis, the wall thickness of each web needs to increase for the required part strength. An additional request to increase the size of the blends must also be made to make the design easier to manufacture.

If the model was only curves and was created in 2D, the changes could take several hours to complete and several different views would need modification. You may need to delete and recreate most of the 2D curves. In feature-based design, you make the change in minutes by altering the parameters used to define the features.

Solid Modeling Advantages (Parametric)

One of the main advantages of solid modeling is the ability to analyze the model. Solid Edge calculates detailed mass properties such as weight, volume, and moment of inertia for a solid body. You can also perform analysis directly on a solid model. Other advantages of solid modeling include:

- The ability to rapidly create and change models.

- The ability to create a drawing directly from a solid model.

- The ability to create photo-realistic images from a solid.

- To obtain mass properties information.

- To create rapid-prototyping models.

- To evaluate the form, fit, and function relative to the rest of the assembly.

Design Intent

Overview:

By having the capability to create feature-based models and parameters, you can capture design intent while modeling. During the course of a design, there are going to be several key pieces of information that you wish to convey. In the past, this has mainly been communicated in the form of a detail drawing. Now you can embed this information as you construct a model.

Play the video for an overview of Design Intent. This file contains sound, so be sure to adjust your volume accordingly.

Establishing Design Intent

Design Intent is accomplished by capturing specific geometric constraints and dimensional relationships between features on the model. Variables can also be created to capture common information like typical round or blend sizes, common wall thickness, standard draft angles, and much more. The design intent can then be conveyed by how the feature is created and dimensioned.

In addition, Solid Edge lets you convey items, like critical fits information, by adding a tolerance directly to a profile dimension. Other items, like inspection symbols and appended text, can also be added. At the start of a design, you may not know what sort of design intent is necessary. By using variables, dimensions, patterns and feature editing, you can change or add design intent to the solid model at any point in the design process.

Variables

Path: Tools | Variables | Variables

Use this to...

• Define custom variables for a part.

• Link custom variables to system-defined variables.

• Modify custom or system-defined variables.

• Play the video for an overview of how to create custom variables, and introduce design intent into your model. Do not adjust your volume; there is no sound associated with this video.

Key Points

• Variables can be linked to several features.

• Capture Design Intent in a model.

Process: Create a Custom Variable

1. Select Tools | Variables | Variables. The Variable Table displays.

2. In the last open Name cell, type in the name of the variable and press ENTER.

3. In the Value cell, type in the value for the variable and press ENTER.

4. If desired, select the units of the dimension from the Units pull-down.

The default is Distance.

5. Continue entering names and values until you have defined all variables.

6. Click X to close the variables window.

Process: Editing a Variable

1. Select Tools | Variables | Variables. The Variable Table displays.

2. Click the cell that contains the value to modify.

3. Enter a new value and press ENTER.

4. Continue editing values for all desired variables.

5. Click X to close the variables window.

Process: Linking Variables

1. Select Tools | Variables | Variables. The Variable Table is displayed.

2. Click the Formula cell that contains the value to link.

3. Enter the Variable Name and press ENTER. The model updates to reflect the new value and the Value cell turns gray.

4. Continue linking values for all desired variables.

5. Click X to close the variables window.

Sample Part Workflow

Overview: This topic is intended to provide you with an example of a typical process for creating a solid part. While these steps will not always be the same for every part, they can be considered an excellent guide.

Play the video for an example of a typical workflow. This file contains sound, so be sure to adjust your volume accordingly.

Base Feature

When creating a new part, the first feature created is called the base feature. It is typically a type of protrusion, which means that it is going to create material. For a protrusion, you need to initially create the base profile. This profile consists of a series of curves that form a closed shape. This shape is constrained with geometric constraints and dimensions that control the shape and allow you to adjust the size parametrically. After the profile is complete, you then define the height of the protrusion to complete the base feature.

Additional features

After the base feature is complete, you can then create a series of additional features. You can create additional protrusions that add material to the base feature, or you can create cutout features that remove material. Each additional feature contains a profile that is geometrically constrained and dimensioned. These profiles can consist of either a closed or open profile. In addition to protrusions and cutouts, you can also create hole features. A hole feature is one of the few features that contain pre-defined profiles. The shape of the profile is based on the type of hole selected. However, each hole still needs to be geometrically constrained and dimensioned.

Arrays and Mirrors

After you define the basic shape of the part, the next step is to define any patterns that can be created. Patterns are a big time saver because they allow you to create several copies of a feature in one step. The pattern creates a parametric copy of a feature and places them in a rectangular or circular orientation. This is intended to capture design intent by keeping all features the same size as the original. Another big time saver is mirroring. If you are creating a symmetrical part, simply model half of the part. Then use the mirror it to create the other half. This can greatly reduce the number of features required for the part and minimizes the amount of information in each profile.

Treatment Features

Treatment features consist of items like drafts, rounds, and chamfers. These features are usually created near the end of the modeling process. If you create them near the end or the process, they are easier to delete or modify without affecting previously created features. Keep in mind that there may be times when you will need to place a treatment feature a little higher in the list.

Saving

Saving the model frequently can prevent a lot of headaches down the line. We recommend that you save the part often to avoid loss of data. Sure, it reduces the amount of Undo capability, but it beats having to re-create several hours of work that was lost due to a system crash.

Solid edge

noreply@blogger.com (Navin) — Thu, 06 Mar 2008 01:44:00 +0000

Introduction

In this unit ...

Welcome to the Drafting Overview unit. Click this link to see a video introduction. VIDEO-01

Some of the topics covered in this unit are:
- Drafting documents.
- Detailed drawings.
- Property text.
- Object linking.

Completion Time: 20 minutes

Drafting Overview

Overview: In most industries, the main method of communicating designs to manufacturing or other vendors is to create a drawing. Drawings contain information such as size requirements, materials, general practices, and surface textures. The Solid Edge Draft module quickly creates drawings of parts, sheet metal parts, assemblies, and weldments.

Play the video for an overview of drafting. This file contains sound, so be sure to adjust your volume accordingly. VIDEO-02

Template

The file extension for a drawing is *.dft. Opening a *.dft document places you in the Draft module. This environment provides you with all of the tools necessary to create a complete drawing. You access the template by selecting File | New from the main menu.

Working Sheet

You add Drawing Views, dimensions, symbols, and any other annotation unique to your model in Working Sheets. You can add sheets at any time, each with its own paper size and background.

The Working Sheet Setup dialog has a Background tab that lists the different background sheets contained in the Draft template. When you need a different paper size for a certain drawing, you can select one of the Background Sheets from the list. Remember that different backgrounds correspond to different sheet sizes.

Background Sheet

The Background Sheet is a special layer in the Draft application, which holds information common to every drawing that you create. Typical items stored on the background sheet include title blocks, revision block, and any other information that is common to all drawing sheets. The Background Sheet is on a special layer so that when you are working in a drawing, you don't make unintended changes to this information.

Drafting Workflow

Overview: This topic is intended to provide you with an example of a typical process for creating a drawing in Solid Edge. While the specific order of the following process is not required to successfully create a drawing, it does provide you with a general guide for most parts or assemblies.

Play the video for an overview of a drafting workflow. This file contains sound, so be sure to adjust your volume accordingly. VIDEO-03

Drawing File

The first step in the drafting process is to create a drawing file. As mentioned earlier, Solid Edge uses a template file with a *.dft extension, and supplies you with many draft templates for both English and metric units.

Sheet Setup

Most default templates come with an 'A' size through 'D' size background sheet for English templates, or an A1 through A4 background sheet for metric templates. To set the size of the sheet, select Sheet Setup and select the Size tab at the top of the dialog. The sheet size can be defined by a standard size or using a custom size.

Add Views

There are a couple of ways to add views to the part and establish the master model link. The first is to use the Drawing View Wizard. This wizard walks you through the process of selecting the part, and defining the views you wish to add to the drawing. This wizard can add several orthographic views onto a drawing at once. The other method is to use the Parts Library function on the EdgeBar. Simply drag and drop a part onto the drawing. This method creates a top, front, and right side view on the drawing.

Supplemental Views

For simple parts, this step may not be required. For complex parts, this step is necessary to obtain the correct view orientations to detail a feature. The auxiliary view option is used to define a view that is projected from a fold line. A detail view can be used to enlarge a portion of a view containing small details. Section views are used to show internal details by defining a cutting plane through a parent view, and creating the section view based upon that cutting plane.

Symbols

Symbols include items like bolt hole circles, linear centerlines, and center marks. These items are associated to the view and can be added automatically when views are created. They can be dimensioned as well.

Dimensions

The dimensions are associated to the geometry; therefore any changes to the model are automatically reflected in the drawing. Dimensions also have several styles and options. You can create dimensions with tolerances, appended text, and inspection symbols.

Sketch

noreply@blogger.com (Navin) — Wed, 05 Mar 2008 08:47:00 +0000

Sketcher Overview

________________________________________
Overview: Sketcher enables you to create parametric, planar geometry on faces and planes. After you draw the geometry, you use the sketch to create pads, pockets, shafts, and surface geometry.
________________________________________
Sketches
Sketches are sets of 2D, fully-parametric curves. In a typical sketch, you first create base curves, and then add geometric and dimensional constraints to control the size and shape of the curves. By adding these constraints to the sketch curves, you can capture and define your design intent. This approach makes it much easier to modify the sketch shape later.

Sketch Usage
Sketches are commonly used to define section curves for pads, pockets, shafts, grooves, or surface geometry.

Sketches maintain associativity to their parent and child features. If you change the geometry in a sketch, the solid model changes accordingly. Similarly, if a plane or face changes orientation or moves, any sketches attached to that plane or face move with it. You can also add dimensional and geometric constraints to the sketch. Using dimensional constraints, you can create system-defined expressions and link them to other sketch dimensions or to other features of the solid.

Using Sketcher intelligently allows you to quickly modify the model to reflect changes during the product life cycle.

Sketch Placement
You create sketches on a plane or solid planar face. A sketch remains associative to its placement face. If the face changes orientation or location, the sketch changes with it.

When you pick a plane or face as the sketch plane, CATIA sets the horizontal and vertical directions as the main axis of the selected plane. You can manually control the horizontal and vertical directions by selecting the horizontal and vertical reference edges, and the placement face, before creating the sketch.

Sketch Management
Organizing the data within a CAD file is always important when different people are potentially going to use the data. Data organization is especially important when using sketches because you can define sketch information in many geometrical sets, with different sketch names. Depending on the complexity of a design, even a simple, single solid model can contain over 20 sketches. With this amount of data, it is prudent to use good techniques to manage your sketches.

CATIA automatically makes a sketch invisible once you use it to create a feature, such as a pad or pocket. However, it is a good practice to place each sketch into a geometric set. This makes it easier to find the information required in the Graphics window. It is also advantageous to give each sketch a descriptive name by editing the properties of the sketch.

________________________________________
Tips
• Always assign the In Work object to the appropriate geometrical set before creating a sketch. Although you can move objects, it may be easier to initially create objects in the correct location.

Creating Sketches

________________________________________
Path:
Insert | Sketcher | Sketch
Insert | Sketcher | Positioned Sketch
Located on the Sketcher toolbar.
________________________________________
Use this to ...
• Create a new sketch.
________________________________________
Key Points
• In CATIA, there are two ways to create a sketch: Sliding (also known as a Non-positioned sketch) and Positioned. In a sliding sketch, you do not have control over the origin or orientation. This can lead to potential errors in your model, such as, if base sketches update, later sketches can become out of place. It is good modeling practice that all the sketches you create are positioned sketches. However, you can update a non-positioned sketch to a positioned sketch.
________________________________________
Process: Creating a Sliding Sketch (Non-positioned Sketch)

1. Select Insert | Sketcher | Sketch. CATIA prompts you to pick a face or plane.

2. In the Graphics window, pick the sketch placement face to activate the Sketcher workbench.

3. On the Workbench toolbar, click Exit Workbench to return to the modeling application.

________________________________________
Process: Creating a Positioned Sketch

1. Select Insert | Sketcher | Positioned Sketch. The Sketch Positioning dialog displays.

2. In the Graphics window, pick a placement face. CATIA projects the sketch origin onto the selected plane or face origin.

3. In the Origin Type list, select the origin definition method.

In the Graphics window, pick the geometry to define the origin.

4. In the Orientation Type list, select the orientation method options. In the Graphics window, pick the geometry to define the orientation.

5. Click OK to create the sketch.

6. On the Workbench toolbar, click Exit Workbench to return to the modeling application.

________________________________________
Options
Sketch Positioning

Defines the two options for creating a sketch.

Positioned
Defines the sketch by selecting a planar face or plane, or by defining two axes. A positioned sketch allows you to define the origin and the reference direction. Using existing edges as references for the sketch direction means the directions update if you modify the underlying edges. Using a positioned sketch is the recommended method of creating a sketch.
Sliding
Creates a non-positioned sketch. The default origin and directions of the selected plane or face define the origin and direction of the sketch. Sliding sketches can be updated to positioned sketches by selecting new reference directions.
Origin

These options define the methods to position the origin of the sketch.

Implicit
Defines the origin as the default origin of the face or plane. Selecting two lines places the origin at the intersection of the two lines. The H direction is collinear with the first line; the second line only defines the side on which the V direction is created, not the orientation.
Part Origin
Defines the sketch origin as the absolute origin of the part.
Projection Point
Defines an origin by projecting a point onto the sketch positioning face or plane.
Intersection 2 Lines
Defines the origin at the intersection of two lines.
Curve Intersection
Defines the origin at the intersection of two curves.
Middle Point
Defines the origin at the mid-point of a line or edge.
Barycenter
Defines the origin at the center of a face.
Orientation

Defines the H and V directions of the sketch. When defining the direction, you can control either the H or V direction. You also have the ability to reverse the direction.

Implicit
Defines the sketch directions as the default directions of the sketch support.
X Axis
Defines the active direction along the X-axis.
Y Axis
Defines the active direction along the Y-axis.
Z Axis
Defines the active direction along the Z-axis.
Components
Defines the active direction by entering vector components.
Through Point
Defines the active direction as the vector through a point.
Parallel to Line
Defines the active direction as parallel to a selected line.
Intersection Plane
Defines the active direction as the line created by the intersection of two planes.
H Direction
Lets you define the H direction of the sketch.
V Direction
Lets you define the V direction of the sketch.
Reverse H
Reverses the H vector.
Reverse V
Reverses the V vector.
Swap
Swaps the H and V directions.
________________________________________
Frequently Asked Questions
1. Can I modify the sketch directions and origin?
A: Yes, you can modify all the sketch definitions by picking the sketch in the Specification Tree and selecting Edit | | Change Sketch Support, or right-click to display the pop-up menu.
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Tips
• Click Exit workbench to quickly exit Sketcher.

Sketch Tools Toolbar

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Sketch Tools Toolbar

The Sketch tools toolbar (select View | Toolbars | Sketch tools) is invaluable when creating sketch geometry. The toolbar enables you to automatically create constraints, and it changes to display the coordinates, lengths, and other information in the context of command you are using. The Sketch tools toolbar also provides feedback as you dynamically move the cursor in the Graphics window, showing you the current length of a line or the diameter of the circle. This information is helpful because sketches are much easier to constrain when the initial geometry is drawn close to the desired size. Additionally, toolbar functions allow you to snap the curves to a grid and create construction geometry.

The Sketch tools toolbar has several distinct areas. The first section contains: Grid, Snap to Point, Construction/Standard Element, and Geometrical and Dimensional Constraints. These first five commands are always present and are the same, regardless of the active sketch command.

The next section contains options that vary, depending on what geometry you are creating or what command you are using to modify your existing geometry. For example, when creating a line, the Sketch tools toolbar displays several different text boxes.
Initially, the toolbar allows you to specify the H (horizontal) and V (vertical) start coordinates. Then the toolbar changes to display the end coordinates. The length of the line and the angle text boxes display at all times while the line command is active.

The Sketch tools toolbar for creating a sketch chamfer has options for how to trim the selections. After you select the geometry, the toolbar displays text boxes for the offset(s) and/or the angle.

You can simply click in the text boxes and enter the values or press TAB to cycle to the next text box. When you finish an entry, press TAB to accept the value. After specifying all the values for a particular geometric parameter, like an endpoint, CATIA modifies the text boxes in the toolbar, allowing you to enter the next piece of geometric information. The advantage in using the Sketch tools toolbar, instead of picking in the Graphics window, is that dimensional constraints are applied automatically to the geometry.

Grid
This option creates a visual grid on which you create sketches. Turn this option on by clicking Grid on the Sketch tools toolbar. Other grid options are set under Tools | Options.

Snap to Point
Locates curve endpoints onto the grid points.

Construction/Standard Element
Creates sketch geometry using any of the creation modes described below. This geometry is used to create solids and surfaces.

When the icon is active (highlighted), any new geometry is created as construction geometry. Construction geometry is gray by default, has a dashed line type, and does not display outside the Sketcher workbench. You can convert from standard to construction elements and vice versa by selecting existing curves and then changing the status of the Construction/Standard Element icon.

Geometrical Constraints
Creates automatic geometric constraints in conjunction with SmartPick when creating geometry. When deactivated, geometric constraints are only applied at the time of creation. After you draw curves, CATIA does not save the constraints. It is very likely that that this will be active all of the time.

Dimensional Constraints
Creates automatic dimensional constraints when entering values in the Sketch tools toolbar to create exact geometry. It is very likely that that this will be active all the time.

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Tips
• Roughly create the profile you need. Then use dimensional and geometrical constraints to finalize the profile.
• When creating a continuous profile, you can activate the Tangent Arc command by clicking and dragging the cursor away from the endpoint of the line. Release to activate the Tangent Arc command.

Curve Creation Techniques

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Overview: When you create sketch geometry, there are different methods that you can use to define the shape, size, and position of the curves.
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Clicking in the Graphics Window Versus Entering Values on the Sketch Tools Toolbar
The two methods of creating curve geometry include picking in the Graphics window and applying the constraints separately, or to using the Sketch tools toolbar to enter specific data.

The advantage in using the Graphics window is that you can quickly create the rough profile and then use the exact constraints that you need to finalize the geometry. The disadvantage is that there are more open degrees of freedom to constrain, initially making curves more difficult to control.

As you become more comfortable with constraints, creating curves on-the-fly is the fastest and easiest method for defining a profile with the proper design intent, especially when used in conjunction with SmartPicks and active Geometrical Constraints.

The advantage in using the toolbar method is that the constraints can be applied at the time of creation, (if Dimensional Constraints is active on the Sketch tools toolbar). The disadvantage is that many of the automatic dimensional constraints may not properly define your design intent, such that you will have to delete and recreate, or redefine the constraint.

Entering a value in the Sketch tools toolbar locks that value, allowing you to either pick in the Graphics window to define the rest of the geometry or use the toolbar to enter the rest of the definition. Using a combination of methods allows you to use defined values, while still having the flexibility of picking in the Graphics window.

Pay close attention to what you are entering in the Sketch tools toolbar. Remember that the Sketch tools toolbar asks for different information, depending on what curves you are creating, and changes as you progress through the definition. In other words, after entering data, the toolbar changes and then looks for the next set of values. Use TAB to move between text boxes in the toolbar. TAB stores the entered value in the toolbar and makes the next text box active. Pressing ENTER only stores the entered value.

Pop-up Menu During Curve Creation
The pop-up menu is also an invaluable tool when constructing geometry. Right-clicking another element when creating geometry displays the pop-up menu.

Depending on your selections, the pop-up menu changes, allowing you to create geometric constraints between the two elements. For lines, the pop-up menu allows you to apply parallel and perpendicular constraints. Right-clicking a circle or arc during line creation allows you to apply tangency constraints.

Right-clicking geometry also allows you to copy the geometric properties of the curve, such as length and radii.

Right-clicking a dimensional constraint allows you to copy the constraint value and paste it into another constraint.

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Tips
• Use a horizontal or vertical constraint instead of specifying an angle of 0, 90, 180, or 270 degrees.

Options - Sketcher

Overview: The Options dialog is where you set various sketch options, such as, Grid, Sketch Plane, Geometry, Constraint, and Colors. All these options are available by selecting Tools | Options, Mechanical Design, Sketcher.
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Grid

Controls the virtual grid that displays on the sketch plane. You can use the grid as a reference when creating geometry.

Activate Snap to point to restrict the cursor movement to the grid intersections. Specify the horizontal distance between grid lines by entering values in the Primary spacing text box and specify the spacing between each grid line in the Graduations text box. To specify different vertical grid lines activate Allow Distortions.

noreply@blogger.com (Navin) — Tue, 20 Nov 2007 09:05:00 +0000

Step 1 Go to Sketcher workbench Select XY Plane as Reference Click here Step2 Click the Axis line toolbar from Profile tools toolbar Click here Step3 Select first and second point of the Axis line click here Click here Step4 Again click Axis line tool bar and create second line Click here