THE DEVELOPMENT OF THE POTENTIAL AND ACADEMIC PROGRAMMES OF WROCŁAW UNIVERsITY OF TECHNOLOGY

Mining and Power Engineering

Janusz Skrzypacz

CAD/CATIA

CAD/ CATIA

LECTURE 8

Part creation by multi profiles extrusion along multi paths (2h)

PLANE

When a part is created by extrusion many profiles, it is necessary to define additional planes where the profiles will be located. The new plan can be generated by Plane Definition function that is placed on the Reference Element Toolbar. The available options of this one are presented on the picture 1 and listed below – the most useful have been bolded.

Fig. 1 The Plane Definition Dialog box

Offset from plane – plane is created as parallel to base one and moved on a defined distance.

Parallel through point

Angle/Normal to plane – plane is created as rotated to base one about defined angle.

Through three points

Through two lines

Through point and line

Through planar curve

Normal to curve – plane is created as normal to base curve in defined point.

Tangent to surface – plane is created as tangent to base curve in defined point.

Equation

Mean through points

Multi-Sections Solid

When it is necessary to create a part by extrusion many profiles, optionally along a lot of paths the Multi-Sections Solid can be used or Removed Multi-Sections Solid to remove material. The Dialog box of these functions is presented on the picture 2. In upper section of the dialog box the profiles are defined. The order of selection is important; it defines the order of connection between the sections. Under this one there are a lot of options described below.

Fig. 2 The Dialog box of Multi-Sections Solid (Removed Multi-Sections Solid) function.

Guide lines are used to help control the shape of the multi-section solid as it transitions between the profiles. Guide lines must intersect all profiles (fig.3).

Fig. 3 The Dialog box of Multi-Sections Solid (Removed Multi-Sections Solid) function with Guides definition

A spine is used to control the shape of the feature between the profiles. As the feature transitions between the sections it must always remain perpendicular to the spine. A spine is automatically computed when creating the solid. If required, you can use a user-defined spine.

Coupling refers to the way the profiles are connected. Below, there are available several coupling options:

·      Using the Ratio option, the curves are coupled according to a ratio of the total length of each section.

·      Using the Tangency option, the curves are coupled at their tangency discontinuity points. To use this option the same number of tangency discontinuity points must exist in all sections.

·      Using the Tangency then curvature option, the curves are coupled at their tangency discontinuity points first and then their curvature discontinuity points. To use this option the same number of tangency discontinuity points and curvature discontinuity points must exist in all sections.

·      Using the Vertices option, the curves are coupled at their vertices. To use this option the same number of vertices must exist in all sections.

When the Relimited options are cleared, the feature will be limited by either the spine or a guide curve, whichever is the shortest. When Relimited options are selected, the feature will be limited by the start and end sections.

When defining a multi-sections solid, closing points display on a vertex in each of the selected profiles. These closing points indicate how the system will connect the vertices. The directional arrow indicates the direction of the next aligned vertices. Ensure the arrow points in the same direction for each section. Closing points must be aligned for proper orientation of the sections. The multi-sections solid will become twisted if the closing points are not aligned (fig.4).

It is possible to Replace, Delete and Create the Closing Point by pop-up menu under Right Mouse Button.

Fig. 4 The Multi-Sections Solid function operation with different Closing Point definition.

DRAFT ANGLE

Draft features apply an angle to a part surface relative to some reference. Material is added or removed depending on the draft angle and pull direction applied during the operation.

Fig. 5 The Draft function operation

The pulling direction defines the direction from which the draft angle is measured. It derives its name from the direction that the sides of a mold are pulled to extract a molding.

The draft angle is the angle that the draft faces make with the pulling direction from the neutral element. This angle may be defined for each face by creating separate draft features.

The neutral element is used to define the pivot hinge for the drafted surfaces. The drafted surfaces pivot about a neutral curve, the hinge, where it intersects the neutral element.

The neutral element, usually a plane or face, can be the same reference used to define the pulling direction. The neutral element is displayed in blue, and the neutral curve is displayed in pink. The faces to be drafted are in dark red. The geometry that is selected as the Neutral Element remains the same during the draft operation (i.e. it is not affected by the draft).

EXERCISES

Exercise 1

According to the picture 6, create a part by two methods: with Draft function, by Multi-Sections Solid. Let try to redefine the closing points and check the result of the function operation.

Fig. 6 2D drawing for exercise 1.

Exercise 2

Create a part as on the picture 3. The dimension of base profile and path parameters are presented below.

Fig. 7 The base profile for exercise 2

Helix parameters:

·      Pitch – 150 mm,

·      Height – 300 mm,

·      Taper angle - 5 deg.

Project co-financed by European Union within European Social Fund