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Standard Views |
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To build standard views of model in the drawing, follow these steps.
1.Invoke the Standard Views from Model 
command.
2.In the dialog that opens, select the source file of the model. In the graphic area of the drawing, there will appear a phantom of bounding rectangles of the generated views, and on the Parameter Panel – setup elements of their parameters.
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If the selected model contains version and (or) variants of geometric representation, you can select the required design/version in the dialog. The geometry of views will correspond to the selected version/design. If the model contains additional numbers, you can also select the required additional number. |
If necessary, in the process of creation of views, you can re-select a model (implementation, variant) using the Source File field on the Parameter Panel. Working with the field is described in the Parameters linked to the modeltable.
3.If it is required to create views not for all the model but specific parts thereof, set the All solids/Selected solids toggle switch to the Selected solids position. On the screen, there will appear the Source model window, and on the Parameters Panel — the Solids field. Specify the required solids in the Source model window. Their names will be added to the Solids field.
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You can specify only solids located at one level in the Model Design Tree. For example, if when creating an assembly drawing a solid included in its component is specified, you will be able to specify only the solids of that component, and if a solid built in the assembly is specified, you will be able to specify the solids of that assembly. |
4.From the Model orientation in the main view list, select the required orientation. The list contains all, including custom, orientations available in the model.
You can create an orientation which is not there in the model. To that end, enable the display of the Source model window using the Model window display 
button, set the desired model position in the Source model window and press the Fix custom orientation 
button, located next to the list of orientations. You will see the button on the panel if the Source Model Window display is enabled.
Elements of setting orientation are described in detail in the Parameters linked to the modeltable.
5.Determine which views you want to be created.
By default, the system suggests creation of three views: the main view, the front view, and the left-hand view. The group of View pattern buttons allows to change the set of views being created. To enable/disable view creation, click the respective button in the group. You cannot disable creation of the main view.
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Relative position of buttons in the group depends on the projection method which is selected when setting up the parameters of the new view (see section View). |
6.Set the distance between the created views using the Gap between views group of fields. In the Horizontal field, enter the horizontal distance between the bounding rectangles of views (for example, between the main view and the left-hand view), and in the Vertical field – the vertical distance (for example, between the main view and the top view). The values are set in millimeters.
7.Set the scale of created views and the color of their display. Details...
8.If it is required to transfer the layers available in model into the drawing, enable the Transfer layers option.
More information about the transfer of layers...
9.Configure the rendering of view lines. Details...
10.Configure the transfer of objects and detailing elements into views. To that end, in the Objects section, enable the required options in the Model Objects and Symbols from model lists.
More about transferring objects and detailing elements...
11.Specify which designations should be created automatically in the views. To do this, in the Create group, under the Objects section, enable the corresponding options in the Symbols in the drawing list.
More information about designation creation...
12.Check the status of the Connect to model properties toggle switch in the Drawing properties pane. If the toggle switch is in position I (enabled), then the values of properties set in the source model will be transferred to the drawing, and not, if in position 0 (disabled).
More about transferring properties from the model when creating a view...
13.Select the point which will be used as the datum point of the main view. To that end, in the View Base Point group, press one of the following buttons:
Center of bounding rectangle or contour,
View Origins.
14.Set the snap point of the main 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 the snap point is specified, creation of views is completed. In graphic region, there appear images of views, and in the Drawing tree – icons of views and their names.
During execution of the operation, several views are created at a time, one of which – main view – represents an arbitrary view from the model, and all the other views are projective curves.
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If there are unsaved changes in the model, you will be prompted to save the model when you create its associative view. Click Yes to save the model file or click nan to cancel saving. In any case, the model image in its current view is created in the associative view. |
See Also
