powered by CADENAS


Manual Sketch 1 – “raw“ cap nut

In order to create a 3D solid, several drawing sections must be run through. You begin with a 2-D sketch[2], which is created in the so-called 2-D Sketcher.

  1. Select New Sketch... from the context menu.

  2. Click on Select new sketch....

--> The 2-D Sketcher is opened.

In the following steps, the 2-D sketch of the cap nut is to be made into the following form:

[Note] Note

To create the drawing, follow the notes in the footer of PARTdesigner. There is some information according to the current state of the drawing or the next step. Creating vertical and horizontal center line
  1. Click the Vertical line . --> A vertical line is attached to the cursor.

  2. Move the cursor along the line to the x/y zero point until --> the Snap (a tracking point for setting the intersection points) appears.

  1. Fix the line with a simple mouse-click. --> The Change parameter context menu opens.

  2. Since the line should run through the 0 point, leave the default value (0,0) and click OK.

  3. By right-clicking again, the mouse loses its function (vertical insertion).

  1. In the same way (steps a) to d)), insert a horizontal lines .

These steps are also documented in the feature tree on the left so that you can later retrace or repeat your steps.

[Note] Note

Deleting elements

  1. Click on the Entity (e.g., line) or step you no longer want in the list pane on the left.

  2. Click on the button Delete last step . Determine height of hexagon
  1. Position a vertical line at the right to the y-axis.

  2. Input field Change parameter: Enter the distance to y-axis M (Height of the hexagon).

[Note] Note
  • If you accidentally enter a variable that is not in the variable list, the message Unknown variablewill appear in the dialog box instead of OK (see figure). You cannot create it in the drawing.

  • If there are syntactical mistakes in the Change parameter pane, a message appears. Check the string and correct the invalid characters. Define total height

Enter a vertical line above the y-axis at a distance of H. Define diameter of a spherical head

Position two horizontal lines (one above, one below the x-axis) at a distance of DK/2. Define horizontal position of spherical head

Hight of passage between (half-)head and cylindric part.

Enter a vertical line right to the y-axis at a distance of H-DK/2. Describe the spherical head with a semicircle

The spherical head of the cap nut is described by a semicircle in the 2-D Sketcher:

  1. Click on the button Circle with center point and radius/point.

  2. Lead the mouse to the point of intersection of the x-axis and the vertical H-DK/2 until the snap shows up.

  3. Fixate the center of the circle with a simple mouse-click.

  4. Enlarge the Radius of the circle, until it is tangent to DK/2 on both verticals.

  5. Fix the Circle by a single mouse click.

Circle center point

Radius Trim the sketch, Part 1

Remove unnecessary drawing elements using the above commands until the sketch looks like the figure to the right.

Use the following three buttons.

Trim element with other : This enables single lines to be cut or lengthened.

  1. Click button Trim element with other.

  1. Select the element range to delete by clicking on it.

  1. Move the cursor to the point of intersection until the snap appears .

  1. Click once on the snap --> and the unwanted elements are removed.

Cut element between 2 elements : This command allows you to separate an element area between two points.

  1. Click on the button Cut element between 2 elements.

  1. Click button Cut element between 2 elements.

  1. Move the cursor to the 1st point of intersection until the snap appears.

  1. Move the cursor to the 2nd point of intersection until the snap appears.

--> The undesired area is removed.

Delete Element

  1. Click on Delete Element.

  2. Select the element to delete. -> It gets deleted. Create external chamfers on the hexagon

In order to display the external chamfers on the cap nut hexagon, t two angled lines, a vertical and a horizontal one must be drawn in.

  • Angled line right

  1. Click the Line at angle to line with length button. Using this function you can create Lines at any Angle to an imaginary vertical line.

  1. Highlight height M as line of reference. --> The new line follows the cursor.

  2. Determine the starting point (1) (intersection point between right horizontal line DK/2 and hex height M ) with the snap and click to set.

  3. From this point, draw a Line at the left and fixate it.

  4. In the Change parameter dialog box, enter the angle[3] –15° (descending line) and the length 5.

Before you can draw in the second angled line, you need the Start point of the chamfer.

The position of starting point results from the intersection between y-axis and a further horizontal (distance DW/2).

  • Angled lines bottom

  1. Add horizontal line above the x-axis at a distance of DW/2 .

  1. Click the Line at angle to line with length button and highlight it as a line of reference to the y-axis.

  1. On the right, draw an ascending line from the Start point (intersection point between right horizontal line DW/2 and y-axis) and click to set.

  1. In the Change Parameters dialog box, enter the angle 90-15° and the length 5.

[Note] Note

The length of the angled lines is purposely overly dimensioned at first. This applies also to the distance S (width across flat) between the horizontal line and the x-axis, which you draw below.

In conjunction with the 2, The sketch will be reduced to the final dimensions later on.

  • Width across flats

Draw a horizontal line above the x-axis at a distance of S. Trim the Sketch, Part 2

Remove the excess lines and the left intersection with the y-axis until your drawing looks like the illustration to the right. Set rotational axis

By circling around a Rotation axis (x-axis), the 2-D contour becomes a solid.

  1. Right-click on the x-axis.

  1. From the context menu, select Attributes, Rotation axis --> The x-axis is now shown as a dotted line. Close Sketch 1

In order to close sketch 1, click on the button Accept changes . --> The display switches back to the 3D view work area. There you can see the contour of the cap nut raw solid.

[2] In the menu area History the sketch shows up as "Skizze".

[3] The chamfer angle 15° (-15°) is taken from the table book.