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Projection View |
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The projection view is built in one of the orthogonal directions relative to the associative view (reference) available in the drawing.
To create a projection view, follow these steps.
1.Call the Projection view command 
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2.Specify the reference view to create a projection view. In graphic area, there will appear a phantom of dimensional frame of the view, and on the Parameter Panel – elements for tuning its parameters.
3.Move the cursor in the direction you want to create a view, for example, to generate a right-side view – from left to right, a top view – top down, etc.
To generate an isometric projection, move the cursor diagonally.
The movement of the view phantom is limited by the projection link between the phantom and the reference view: top and bottom views can be moved in the vertical direction only, and the right-side and left-side views – in the horizontal direction only. You can disable the link between views using the Projection link toggle switch. In this case, a view can be positioned in any place, as well as be rotated by a set corner – on the Parameter Panel, the Rotation angle field appears, where the value of angle is entered.
4.Set the name and number of the view using the respective fields. The number of the view can be any number other than the numbers of already existing views.
5.Set the scale of the view and the color of its display. Details...
6.If it is required to transfer the layers which are available in the model into a view, enable the Transfer Layersoption.
More information about the transfer of layers...
7.If the reference view is created from an assembly model with the configured spacing settings, then in the created view it is possible to display this assembly in a spaced view. To that end, enable the Explode Assembly Components option.
8.If the reference view was created from a model in which there is a sheet solid and the flat pattern parameters configured, then in the view being created it is possible to display a sheet solid in the unfold view. To that end, enable the Flat pattern option.
9.Configure the rendering of view lines. Details...
10.Configure the transfer of objects and Detailing elements to the view. To that end, in the Objects section, enable the required options in the Model Objects and Symbols from model lists.
More about the transfer of objects and detailing elements...
11.Specify which designations should be automatically created in the views. To do this, in the Create group in the Objects section, enable the corresponding options in the Symbols in the drawing list.
More details on designation creation...
12.Configure the structure of the view caption. Details...
13.Select the point which will be used as the datum point of a view. To that end, in the View Base Point group, click of the following buttons:
Center of bounding rectangle or contour,
View Origins.
14.Set the snap point of the view. To that end, specify the position of point in the graphic region using the mouse, or enter its coordinates in the Snap point field of the Coordinates group on the Parameter Panel.
After setting the point, the view is created automatically. In the graphic region, there appears an image of the view, and in the Drawing tree – its icon and name.
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The image of a model in the resultant projection view depends on the selected projection method (see the Viewsection). For example, to generate a left-hand view, move the cursor from the reference view to the right, if the By first anglemethod is selected, and to the left, if the By third angle method is selected. You can also rotate the view with another side by changing the projection method. |
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If the reference view has a break, then projection view is automatically built with a break. |
15.After the view is created, the command is not completed. You can create the desired number of projection views by setting the necessary parameters and specifying the snap point. The supporting view remains the same.
16.To complete operation of the command, click Finish 
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See Also
