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

Mining and Power Engineering

Janusz Skrzypacz

CAD/CATIA

CAD/ CATIA

LECTURE 4

A Part creation by a profile extrusion (2h)

If we want to create a part by extrusion a profile through a path which is a line perpendicular to the profile, we have to use PAD function. We can find this one in Sketch-Based Features group located at the Insert top menu or at the Toolbar

The dialog box of the PAD function is presented on the picture 1. The mining of the options is explained below.

Fig. 1 The dialog box of the PAD function

Profil/surface – a profile which will be extruded. General rule is that a profile must be closed and it can contain some internal sub profiles which always generate pockets (fig.2). It is possible to use an open profile only when Thick option is selected.

First limit – first limit of extrusion,

Second limit – second limit of extrusion,

              Type:

·                Dimension – extrusion to defined dimension,

·                Up to next – extrusion to a next surface,

·                Up to last - extrusion to a last surface,

·                Up to plane – extrusion to defined plane,

·                Up to surface – extrusion to defined surface,

Reverse Direction – the change of extrusion direction,

Mirrored extend – symmetrical extrusion in both directions,

Thick – creation of a part in which the thickness is added only to profile edges (fig.3),

Thickness1 – internal thickness of Thick element,

Thickness2  - outer thickness of Thick element,

Neutral Fiber  – this option defines symmetrical thickness relative to profile edges,

Merge Ends  – cutting a Part by the existing Parts (fig. 4).

Fig. 2 The result of the PAD function when a profile includes an internal sub profile

Fig. 3 An example of the PAD function when Thick option is selected

Fig. 4 An example of the PAD function when Merge Ends option is selected

The reverse function to the PAD is POCKET. It means that result of this function operation is a pocket (recess) in a Part which shape is determined by profile extruded through a path that is a line perpendicular to the profile. We can find this function in Sketch-Based Features group located at the top menu Insert or at the Toolbar  .

An example of POCKET function is shown in figure 5. The dialog box looks the same as in case of PAD and meaning of all options is the same as well.

Fig. 5 An example of the POCKET function

Generally definition of a multisections profile (profile which include some internal sub profiles) is not recommended but in some special cases such action could be necessary. In order to have control on extrusion process of every section separately it should be used MULTIPAD function. This function can be found in Sketch-Based Features group located at the top menu Insert or at the Toolbar . An example of such function and their dialog box are presented in figure 6. The base profile consists of outer profile (rectangular) and one internal profile (circle). The first limit and second limit options are available for every profile that can be selected in Domains section.

Fig. 6 An example of the MULTIPAD function

Elements with thread are common use in machine build process. In order to create a thread one has to use a THREAD function. This one can be found in Dress-Up Features group located at the top menu Insert or at the Toolbar .

An example of the THREAD function is shown in figure 7 where the dialog box is presented as well. The options from dialog box are explained below. The thread is not marked on the 3D model due to saving computer recourses but is presented on 2D drawings.

Lateral Face – circumferential surface  where the thread will be generated,

Limit face – frontal face where the thread will be started from,

Type – thread type,

Thread Depth – thread length, measured from Limit face

Fig. 7 An example of the THREAD function

EXERCISES

Exercise 1

According to profile presented below create a Part by usage PAD function (extrusion 50 mm) and save the Part. Next delete the part in such a way to leave the profile.

Basing on the profile create three parts in order to use MULTIPAD function according to fig. 9 to 11.

Fig. 8 Exercise 1 - base profile

30

20

Fig. 9 Exercise 1 - part that should be created

10

Fig. 10 Exercise 1 - part that should be created

Fig. 11 Exercise 1 - part that should be created (the stiffener height is 15 mm)

Exercise 2

Let's create a Part according to drawing bellow. Use PAD and POCKET function only.

Consider a correct sequence of the operation. Don't attempt to look at next pages.

Suggested steps

STEP 1

STEP2

STEP 3

STEP 4

STEP 5

Project co-financed by European Union within European Social Fund