Anchor Block Draft Tutorial

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1 Anchor Block Draft Tutorial In the following tutorial you will create a drawing of the anchor block shown. The tutorial covers such topics as creating: Orthographic views Section views Auxiliary views Dimensions and centre lines Scaling views etc. Starting a new drawing To create a new draft document select File New The dialog box which appears enables you to select a general purpose drawing template. However, we require the Sligo IT drawing template. To access this template, select the [Advanced] button then select ITS-A N.B. If this document is not available to you in your templates folder, ask lecturer to download it. This template has been pre-designed to automatically populate with the boxes under various headings. On opening you will be prompted to insert a view. For the moment select escape [Esc] to cancel. To create a single view of the component select Model View icon. In the dialog box which appears you will be presented with a list of components which are already open. (If the component to be drafted is not currently open, select browse to locate it). Select the anchor component You are now ready to move to the next step. To do so select the arrow on the top left as shown. In order to see the orientation of the view being inserted select Preview option in the Orientation section; then select each of the standard views in turn to find the view required. Select an orientation the same as the elevation in handout. Having identified the correct location select to place the view. To stop SolidWorks prompting you to create additional views, disable the Auto-start projected view. We will create additional views as we need them. S Dalton, IT Sligo (30-Jan-12) 1

2 Changing view properties Once placed you can now change the view settings. Generally it is desirable to show internal detail even though is may not be visible in a regular view. To do this we show hidden detail. To display hidden detail, select the view in question and select the hidden line display style as shown below. Always activate hidden detail in regular orthographic. N.B. Generally speaking hidden detail is not shown is a section view since, (a) a section is already showing internal detail and (b) hatch lines and hidden detail would result in a view which is overly cluttered.. Creating a plan view You are now ready to create a plan view. This is done using the projected view tool. To create the plan views, select the elevation, followed by the projected view icon. Moving the mouse left and right, about and below will produce a preview of the appropriate view for that location according to the projection type chosen. To create the plan view, select a point below the elevation. This should result in the view shown opposite. Note that the view has also inherited the hidden line display style from the parent view. Creating an isometric view To create an isometric view of the component select the projected view icon the move top-left, top-right etc. Four isometric views are possible from any view. Select the location which produces view shown in handout. N.B. View can be repositioned afterwards Adjusting scale Currently the views are slightly larger than we would like. To modify the sheet scale, right click and a blank portion of the drawing sheet and select properties, in the dialog box which appears enter the values 1 to 2.5 (a scale of 0.4). Projection In the same dialog box we can also change the projection type. In this and all our exercised we will use the default projection type first angle projection. S Dalton, IT Sligo (30-Jan-12) 2

3 Creating a section view To create a section view, choose the section view icon, then draw a line through the middle of the plan view. Hover over the edge to infer and alignment to the mid point, then starting about 1cm to the left, draw a line from that point to approximately 1cm to the right. (on completing the line a floating preview of the section will appear attached to the cursor) If arrow A is not pointing in the correct direction (upwards) then choose the flip direction option shown. Finally, place the resulting view directly above the elevation. (This example illustrates a straight section, however many other section types are also possible). Auxiliary views Where it is required to see the true shape of an angled face, an auxiliary view may be used. To create an auxiliary view of the angle face, select the auxiliary view icon followed by the line/face shown; then, select a point to the upper right to place the view as required. Broken out section Sometime it can be desirable to show local detail in section without necessarily creating a whole new view. This can be achieved using a local or broken out section. To create such a view simply create a closed sketch (full sketch tools are available under the sketch tab). Then with the sketch still selected, select the broken out section icon and specify a depth of 24mm. (the represents the distance from the front face of the part). Detail view On other occasions it can be desirable to magnify certain details. This can be achieved using a detail view. To magnify the thread detail, select the detail view icon the draw a circle around the detail in question. (First point identifies the centre and the second sizes the circle) Once created a floating preview will appear attached to the cursor. Move the cursor to a suitable location and then click to place the view. Scale may be modified if necessary. S Dalton, IT Sligo (30-Jan-12) 3

4 Tangent edges The default setting in SolidWorks is to show tangent edges with the same linetype and thickness/blackness as regular edges. It is more appropriate to use a lighter line or none at all. In general we do not show tangent edges in orthographic views. In pictorial views tangent edges are shown using a thinner/lighter line. Right click on the orthographic views and select Tangent Edges Removed. On pictorial views right click and select Tangent Edges with Font. Centre marks and Centrelines It is standard practice on engineering drawings to show centre lines on cylindrical features like holes etc. In views where the feature is round horizontal and vertical centre lines are added. In side view the axis of the feature is represented by a centreline. To add centre mark to circular feature select the centre mark icon, then select the circular features in question. To add centrelines to represent the axis of cylindrical features, select the centreline icon, then select the relevant view. This will add centre lines to all appropriate features. Adding Dimensions As dimensions have already been added at modelling stage it is not necessary to repeat the process at drawing stage. All dimensions added during modelling may be imported into your drawing by adding model items. (Additional dimensions may be added manually) Dimension may be imported for a single feature or for the entire model. Under source select Entire model. At drawing stage it is possible to tag certain dimension for display in a drawing and others not. Then when importing dimensions, you can import only those which are tagged by selecting icon A only. Alternately you may import all dimension by selecting icons A and B. Once imported it is usually necessary to reposition them to tidy up your drawing. As a general rule dimensions should be evenly spaced with smaller dimension on the inside and larger dimension on the outside. S Dalton, IT Sligo (30-Jan-12) 4

5 Populating the titleblock The titleblock comes pre-defined with attributes so that when a part file is inserted into a drawing, attribute data associated with the part will be added to the titleblock. To define these attributes you need to return to the part. To do this select a view followed by the open part icon. Once open select properties from the file pull down menu. Next select the custom tab and then click row 1 under property name and select Drawn By from the pull down list. Then in column 3 enter your name. As each property is defined another row is added automatically. For the next property select description and add the title Ex1 Anchor Blk. Finally specify steel as the material and select [OK]. Using the window pull down menu, return to your drawing. On examining the title block you will see that it has now been populated with the details just supplied. Breaking Alignment Generally speaking orthographic view must be kept in line. However, it is not always possible to maintain alignment due to space limitations. In such cases it is possible to break the alignment. To do this right click on the view, select alignment followed by break alignment. S Dalton, IT Sligo (30-Jan-12) 5

6 Sectioning a rib To improve the strength of the component we will add a rib feature. Working on the centre plane add the rib detail then extrude 16mm using the mid plane option. Next return to the drawing. On returning to the drawing you will notice that the section view has updated automatically to reflect the modification. It is standard practice in engineering drawings to omit section lines from certain features. One such feature is a rib. To turn off sectioning of the rib right click on the section view and select the section scope tab on the dialog box which appears. Any rib feature selected while this box is active will be added to the Rib features to be omitted section and will be removed from the section. Select the rib feature just created in the elevation followed by OK. On selecting OK button, the section view will be updated as shown opposite. This completes the Anchor Block draft Exercise. S Dalton, IT Sligo (30-Jan-12) 6

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