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.
Add a thread mark that appears in the drawing as a dimensioned thread and in the model as a visual image.
Add a chamfer to the edge.
Functions to be used:
We review sketching tools.
Operation: Guode curve and Cross Section.
Sweep > Boss.
Thread symbol.
Bevel.
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 the first feature
New Sketch > To vertical (XZ) plane
Sketch the shape
Use the Smart (Smart line chain) function, for example.
Start sketching from the origo so that the cursor also catches the vertical line in the center cross.
Add a coincident constraint between the vertical line and the center point of the lower arc.
Dimension according to the figure.
Dimension 15 is defined between the upper arc and the end point of lower arc.
If the addition of dimension (15) does not seem to be successful, first drag the end of the arc to a suitable distance.
(from sketch to operation selection).
Operation
Guode Curve.
If the geometry is not visible after the operation
You can display the auxiliary geometry (guide lines, auxiliary planes and cross sections) with the G key or the Show Reference Geometry function of the Tool Strip:
Create the cross section
Select a line (e.g. a straight line).
Right-click function: New Sketch.
The program opens a dialog that allows you to adjust the position of the sketch.
Accept the default (Relative position and value 0.5) so that the sketch plane will be in the middle of the line.
Sketch the shape
The function: Circle. (Circle with Center and Radii Point).
Place the center point at the origo of the sketch.
Add a Diameter constraint: 10.
Operation
Cross Section.
Placement of the sketch on the line
See the sketch placement on the line for more details:
Sketching course - in modeling of part
9. Seal.
Paragraph: Create a sketch for the guide curve.
Create a part of the cross section and control curve
Select line.
Select cross section (Remember the Ctrlkey).Right-click function:
Right-click function: Sweep > Boss.
Accept the sweep dialog defaults (no trimming).
Add a Thread Symbol
Click to the cylindrical surface on which you want to add a Thread Symbol.
Click to the line where the thread symbol begins.
The Thread feature dialog opens.
Default thread standard ISO, SFS44498 (mm threads).
The program can suggest an Outer thread for the pin and an inner thread for the hole as the Type.
The dialog tells you the diameter and length of the cylinder surface.
Select Diameter: M10.
Enter Depth: 30.
Select Pitch: 0.75.
OK.
Thread Symbol and and real 3D thread
The thread mark feature appears in the drawing where the thread can be dimensioned, but it does not make a real thread to the model to ensure fast program operation in assembly with many threaded parts.
Real threads must be modeled separately using a spiral and a thread-forming cross section.
Add bevels
Select a line at both ends of the part (Remember the Ctrl key).
Right-click function: Add Round/Bevel > Single Edge Bevel.
Enter the bevel length dimensions: 1 and 1.
OK.
Give item data to the part
Right-click function: Item Data.
Press: Get Item.
Press the preselection button in the Main Group field.
Select: Steel
Select: Bars
Select: Hot Rolled Round bar
OK.
Select: RB010or some other suitable item (by double click).
Also fill in part information, e.g. 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).
A couple of notes about the drawing:
In order to dimension the tolerated dimension 10 + -1, a guide line must be drawn at between the ends of the chamfers.
Because a line is projected on the drawing that is not a valid other part to the dimension.
The M10x0.75 dimension is obtained when the line at the end of the helical feature is clicked in the dimensioning.
diameter 10 dimension is obtained when a cylinder is clicked.
