7. Eye Screw

Exercise 7: Eye Screw

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.

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.

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.

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).
    

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

Download the Eye Screw model (VX_PART7.vxz) here