Draft Tutorial This tutorial provides step-by-step instructions for the detailing of a drawing of the anchor block shown opposite. As you create this drawing, you will use the following drafting techniques: Placing principal and auxiliary views Editing display properties Placing dimensions and annotations To start a new drawing Select File New then from the dialog box, which appears select Normal.dft followed by OK. To set the sheet size and projection This drawing will be produced on an A3 sheet in First angle projection. To set to A3 both the sheet size and the background must be set to A3. This can be done using sheet setup. Select File Sheet setup. Next select A3 wide on the size tab then on the background tab select A3-sheet.. To set the projection type select Tools Options then select the drawing standards tab then select first for first angle projection followed by [OK]. To insert multiple views Select the drawing view wizard icon. From the Dialogue box which appears select anchor.par. Navigate to the appropriate folder if necessary. S Dalton, IT Sligo 1 October 2004 1
From the next dialogue box, which appears determines whether or not hidden detail or tangent edges are displayed. Accept the default settings by selecting the [Next >] button. You are now presented with a number of choices for the orientation of the principal view. To get a graphical view of the components orientation. Select [Custom ] This view can be orientated to produce the required principal view (i.e. elevation and the view from which the other views are created). This view can be rotated using the standard view orientation tools. In the case the view is correct so select [close] to accept. Next you will now be presented with the dialog shown opposite. Button [A] is selected by default. This represents the orientation of the principal view (i.e. the elevation) as seen in the previous image. You may then choose any of the additional 8 views. 4 orthogonal 4 isometric In this case select only [B] (to create a plan view) followed by [Finish]. On the ribbon bar select a scale of 1:2 (0.5). If the scale is not suitable it can be readjusted later by right clicking on the view and selecting Properties and readjusting the scale. Finally the views may be repositioned as required using the selection tool S Dalton, IT Sligo 1 October 2004 2
To create secondary view It is not essential to create all view in one go. I.e. if a view already exists you can create another view from it using the icon. E.g. To create the left hand end view select the icon, then select the elevation [A] then click [B] to locate the view in the blank space to the left of the elevation. Orthographic views are created by selecting positions North, South, East and West of the principal view. Isometric views, on the other hand, are created by selecting positions NE, NW, SE and SW of the principal view. To create an isometric view select [A] as the principal view then [C] as the view location. This view obscures the title block. Re-position the view and if necessary reduce the scale to suit. N.B. If you need to reposition one of the orthographic views you will need to disable the alignment property, which keeps views in line. This is achieved by, right mouse clicking on the view then selecting unalign. To define the cutting plane and section view. In this case we will section the plan and locate the result above the elevation. To define the section plane select icon then select the plan view. This produces and 2d drawing tool similar to Sketch mode. Using the line command draw a line from B to C. To help locate the line hover over the line at A until the mid point symbol appears, then move out to B before clicking. Ensure the line extends approximately 10mm either side of the view. Finally select [finish] and the line will change to the correct representation for a section line. Finally click to either above or below the cutting plane to determine the correct direction of the arrows. I.e. pointing upwards. To create the section view select the icon, the select the cutting plane just created, then click in the blank space above the elevation to locate the view. S Dalton, IT Sligo 1 October 2004 3
To create an auxiliary view. To create an auxiliary view, select the auxiliary view icon. Next define the surface perpendicular to which the auxiliary view is viewed by selecting surface [A]. (Correct detection of surface A is indicated when the line following the cursor aligns itself with the surface). Finally select B to locate the auxiliary view. To create a detail view. You will now create a detail view of the slot. To define the location of the area to be enlarged, create a circle by select A to define the centre and B to define the radius and finally C to define the position of the view. Accept the default scale of 2:1 displayed in the ribbon bar. Automatic dimensioning. The most desirable approach to dimensioning your drawing is to apply a dimension to each feature as you draw it in part mode. Any dimensions that are applied in part mode can be automatically imported. To dimension the end view, select the above icon and then select the end view. Repeat for the elevation and plan. Use the select tool reposition the dimensions as required. All remaining dimensions may be added using the and icons. Centre lines Centre lines are generally added to any cylindrical feature to represent the axis of the feature. Where these are omitted they must be added manually. Centre lines can be added by two points or by two lines. To add centre lines to the hole in the angled feature select the centre lines icon, select the by two lines option then select line A and B. S Dalton, IT Sligo 1 October 2004 4
To add a prefix to a regular dimension. Sometimes it is necessary to amend a dimension with additional detail. In the next example we will clarify that there are two holes of the same dimension by dimensioning one of the holes and then preceding the dimension by 2 x. Select smart dimension icon. Next select the upper hole in the plan view then, before locating the dimension, select the dimension parameters prefix icon on the ribbon bar. In the prefix box type 2 x followed by [OK]. Then finally specify the dimensions location. Adding callouts (leader lines) and comments. To add additional information to a drawing, use the above icon. In the dialog box which appears fill in the necessary detail using the special character symbols where required followed by [OK]. Next select the item to which the arrow points follows by the text location. Finally complete the drawing by adding any other omitted dimensions. S Dalton, IT Sligo 1 October 2004 5