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 clickingArc.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.
