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9. Seal

Exercise 9: Seal

Version compatibility

This exercise was carried out with version 27.0 (Vertex 2021).

Table of Contents

In this exercise you will learn to

  • Mirror the sketch geometry.
  • Sketch placement on the guide curve.
  • Operations: Guide curve and Cross Section.
  • Sweep.

Functions used

  • Sketching: Smart line chain, Two Point Line, Acr with Tree Points.
  • Sketching constraints: Distance, Radius, Angle.
  • Sketching: Delete Section of Line.
  • Sketching: Mirror.
  • Sketching: Round.
  • New Sketch (When the line segment is selected).
  • Operation: Guide curve.
  • Operation: Cross Section.
  • Part: Sweep.

Create a new part

  • File > New > Part.
    • Enter the label (which is also the name of the model and by default will be the name of the drawing).
    • Enter the archive information by clicking Arc.Data.
    • Select the project for the model.
    • OK.

Start sketching

  • New Sketch > To horizontal (XY) plane To vertical (XZ) plane To lateral (YZ) plane

Sketch the part of the control curve to be mirrored and mirror it

  • Function: Smart Line Chain.
    • Sketch a line chain, in the figure A.
    • Stop the function (Press Esc or Middle button of Mouse).
  • Fence the geometry, in the figure B.
    • Select a point in space (when no function is in progress), in the figure 1) and hold down the mouse button.
    • Move the cursor so that the selected geometries remain inside, in the figure 2).
    • Release the mouse button. Now the elements are selected.
  • Mirror the geometry, in the figure C.
    • Right-click function: Mirror, in the figure 3).
    • Click the horizontal line of the origo as the mirror line, in Figure 4).

Mirrored geometry

Gets symmetry conditions automatically.

Complete the sketch with a line and an arc.

  • Function: Two Point Line.
  • Function: Acr with Tree Points.

    • Note that the tangentiality option is selected for the arc
    • If not, select it from the Mini Toolbar.

Give Coincidence and dimensions

  • Function: Coincident.

    • Click to the line, in the figure A).
    • Click the vertical line of the center cross.

  • Function: Dimension.

    • You can add all the dimensions shown in the figure with the function Dimension.
    • Instead, you can also use constraints: Distance, Angle and Radius.

Perform the guide curve operation

  • Stop sketching (the green OK button).
  • Select: Guide Curve.
  • Click OK.

Create a sketch for the Guide curve

  • Select one line from the control curve, in Figure 1).
  • Right-click function: New Sketch, in Figure 2).
  • Accept the relative position of the sketch (0.5) with a line, in Figure 3).

Sketch for the line segment

The selected line can be a segment, a circle, an arc, an ellipse, a spiral, a sline or the line edge of a part.

If the intention is to create a Sweep, then the sketch may be located anywhere on the line. The default point, in the middle, then works well.

If the intention is to create a Loft, in which the line has several different cross sections, the following dialog can be used to determine the location of the sketch (and cross section).

  • Relative pos.: value 0 ... 1 (0 represents one end of the line and 1 represents the other end).
  • Dist. from the start: Enter the distance (in millimeters) from the first end of the line.
  • Dist. from the end: Enter the distance (in millimeters) from the second end of the line.

Check the view of the model before starting to sketch

  • If Perpendicular is selected in the sketch settings, the sketch may be in the position, the direction you think is up is down.
  • It is advised to start sketching first in an isometric projection and then turn the sketch in a perpendicular direction with the Right-click function: Perpendicular.

Sketch the cross-sectional shape of the seal

Sketch a rectangle:

  • Function: Two point rectangle.

  • Click the origo as the first point (center of the blue cross).
  • Click the second point.

Sketch a circle:

  • Function: Circle with Center and Radii Point.

  • Click the center of the lower segment. (So that the center of the circle gets the conincident constraint on the line).
  • Select the location of a point on the circumference of the circle.

Remove unnecessary line segments:

  • Function: Delete Section of Line.

  • Click the portion of the lines you want to delete.

Add dimensions and round corners

Add dimensions:

  • Function: Dimension. (or functions: Distance and Radius), in Figure 1).

Round the corners:

  • Function: Round.

  • Select four corner points, in Figure B).
    • The second, third, and fourth points are selected by pressing the Ctrl key.
  • Right-click function: Round.
  • Enter the radius: 1.5.

Perform the cross section operation

  • Stop sketching (the green OK button).
  • Select: Cross Section.
  • Click OK.

Create a part by swiping the cross section along the line chain

  • Click a line and cross section. (Second element with Ctrl key)
  • Right-click function: Sweep > Boss.
  • The program opens the Sweep dialog.
    • You can study more about this in the OnLine Help (F1).

Sweep with a cross section in the library

  • Function: Add boss using cross-section from library
  • Select a cross section from the Profile library.
  • Click the guide curve line or edge of part.

Select the last line to be swept

  • Click: Add, in Figure 1).
  • Click the line to add, in Figure 2).
  • Right-click function: OK (Add the selected line to the list of Sweep Elements).
  • OK

About the sweep

The program finds all lines tangential to the selected line and adds them as Sweeping Elements.

  • If necessary, you can add lines that belong to the same line chain (but not tangential) using the Add.
  • If necessary, you can delete tangential lines. Use the Delete.
  • The dialog also includes the possibility that the sweep can be trimmed from either end to either a surface, a section, or a point.
    • If necessary, an offset can be entered for this trimming.

Note that the cross-section must be able to pass through the arcs of the steering geometry so that it does not have to rotate around itself.

Save the model

  • File > Save or click
    or press

Further processing of the model (presented in Exercise 5. Swivel lever)

You can add a material item to the model with the right-click function Item Data.

  • These will also appear in the parts list of the model drawing.

You can create a drawing for the model:

  • In the feature tree, select Drawings.
  • Right-click function: New Drawing.

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