7. Eye Screw
Exercise 7: Eye Screw
Version compatibility
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 clicking Arc.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 Ctrl key).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: RB010 or 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).
- 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.
Save the drawing
- File > Save or click or press
Save the model
- File > Save or click or press