This exercise was carried out with version 27.0 (Vertex 2021).
Table of Contents
In this exercise you will learn to
Create a part using a guide curve and cross section.
Saving a sketch to the library and reading it from the library.
Copy line of the previous geometry to the sketch.
Using the library feature as a cutout feature
Create the drawing so that the direction of the front projection is selected.
Functions to be used:
We review sketching tools.
Sketching: save to Library and Open sketch.
Sketching: Copy to Sketch Plane.
Operation: Guode curve and Cross Section.
Sweep > Boss.
Item Data.
Drawing > New Drawing.
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.
Create a Guide Curve
New Sketch > To vertical (XZ) plane
Sketch the shape
Sketch lines, polyline. (Start from the origo and direction the line down).
Add dimensions. (90 and 70).
Click a corner point.
Right-click function: Round. (50).
Operation
Guide Curve.
Create Cross Section
New Sketch > To horizontal (XY) plane.
Sketch the shape
The function: Rounded rectangle of radius 10.
Start from the origo.
Add dimensions to the rectangle: 40 and 30.
Use the Offset function to add a parallel copy to the line.
Note the option: Line chain to same side.
Note the option: Choose line chain.
Note the option:Automatic preview.
Enter Distance: 4.
Click the (Shape) line.
Select the side (inside the rectangle)
OK.
Operation
Cross Section.
The Rounded Rectangle
The program first asks for the corner radius.
Next, the program asks you to click to the center of the rectangle. ("Add rectangle. Select point 1")
Finally, the program asks you to click the corner point of the rectangle. ("Add rectangle. Select point 2")
A rounding is drawn only if it fits in a rectangle.
If the shorter dimension of the rectangle is less than the 2 * radius dimension, the program draws an acute-angled rectangle.
Create the pipe using a cross section and a guide curve.
Click the Cross Section.
Click the Guide Curve.
Right-click function: Sweep > Boss.
The program finds and selects a tangential line, and opens the dialogSweep.
Accept the defaults.
OK.
Sweep Dialog
At the top of the dialog you can choose whether the sweep will Boss or Cutout the geometry.
Sweep Elements:
The program itself searches for all lines tangential to the selected line.
You can also use the Addbutton to select lines in the chain that are not tangential.
Use the Change button to change the selected line to another line (rare).
Use the Delete button to delete the selected lines (at the end of the line chain).
Keep cross section direction
Normally, the cross-section is always kept perpendicular to the sweep line.
With this selection, the cross section slides along the curve in the original position.
1st and 2nd End Trimming.
By default, the ends are not trimmed, but the end can be trimmed when the part is modeled in an assembly, on a clicked faces, on another part, or at a point found in the model.
With the offset value, the sweep can be extended beyond the line chain (negative value) or left shorter than the line chain extends (positive value).
Create the first flange
New Sketch > To horizontal (XY) plane.
Sketch the shape
A Rounded rectangle of radius 9.
Start from the origo.
Add dimensions to the rectangle: 70 and 60.
Sketch one circle of the same center with the corner rounding, diameter: 8.
Mirror the circle around the vertical axis.
Mirror the circles around the horizontal axis.
Save the sketch: (Because it is used at the other end).
Right-click function: Save to Library.
Select a folder or create a new folder.
Enter the draft a name, e.g. flange1.
Complete the sketch: (with lines copied from the previous geometry)
Copy the lines on the inside edge of the pipe to the sketch, so that the flange does not become sealed.
Select lines (Remember the Crtlkey).
The choice of lines is more illustrative if you turn the model a little so that it is no longer perpendicular View.
Right-click function: Copy to Sketch Plane.
Operation
Boss > Extrude.
Lenght: 8.
Invert the direction or drag the direction from the arrow toward the part (i.e., inward from the sketch plane).
Save the sketch before the operation
Lines copied from geometry
Lines copied from the previous geometry of the part get an identical constraint to the previous geometry.
The identical constraint can be removed.
The identical constraint cannot be added interactively. Instead, a coincident constraint or constraints must be used for this need.
It is not advisable to store a sketch with identicalconstraint in the sketch library, as the lines with such a constraint will later try to find a "partner" in the new model, and when they fail, the draft may "break down."
If you trim a line that has identical constraint, then the original line is converted to a contruction line and a trimmed line is generated in its place.
Create the second flange
Select the face.
Right-click function: New Sketch > Face.
Sketch the shape
Right-click function: Open Sketch.
Refress Browser (if the sketch you saved is not displayed).
Place the sketch
Turn the sketch if necessary.
Place it with coincidentconstrain.
Copy the lines on the inside edge of the pipe to the sketch, so that the flange does not become sealed.
Select lines (Remember the Crtlkey).
Right-click function: Copy to Sketch Plane.
Operation
Boss > Extrude.
Lenght: 8.
Invert the direction or drag the direction from the arrow toward the part (i.e., inward from the sketch plane).
Create a groove for the seals on flange (bottom)
Right-click function: Library feature > Cutout.
Double click a feature: Features > Standard > Basic_Shapes > rectange_profile.
Enter value of Dimension Table dialog:
a = 46
b = 36
h = 1
r = 12
s = 4
Place the cursor on the face of the part and make sure that the position of the feature is on the correct face.
Place the feature, for example, with the Centeringconstraint.
You may also need to use the Parallel constrain.
OKcompletes the feature addition.
Press G to show and hide auxiliary geometry (feature has guide lines)
Create a groove for the seals on flange (top)
Right-click function: Library feature > Cutout.
Double click a feature: Features > Standard > Basic_Shapes > rectange_profile.
Enter value of Dimension Table dialog:
a = 46
b = 36
h = 1
r = 12
s = 4
Place the cursor on the face of the part and make sure that the position of the feature is on the correct face.
Place the feature, for example, with the Coincident constraint.
OKcompletes the feature addition.
Give item data to the part
Right-click function: Item Data.
Click on the line in the lower dialog, in the figure 1).
Right-click function: Add row after, in the figure 2).
Click the preselection button in the Material field, in the figure 3).
Select: Aluminium (by Double click).
Select: AlMgSi1 (by Double click).
Also fill in part information (upper dialog), eg weight.
Press: Calculate.
OK.
Create a drawing for the part
See more detailed instructions for the exercise: 5. Drawing of the model.
Drawing > New Drawing (In the feature tree).
In the dialog New drawing, select data:
Scale: 1:1
Sheet: A3
Select projections: front, top and left.
Tangential lines: Draw as virtual shape lines (thin).
Remove selection: Auxiliary geometry.
OK:progress to the archive data.
Review and accept the archive information
The program copies the archive data to the drawing title bar.
