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Arbitrary view |
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To build an arbitrary model view in the drawing, follow these steps.
1.Invoke the Model View 
command.
2.In the dialog that opens, select the source file of the model. In graphic area of the drawing, there will be a phantom of a dimensional rectangle of the created view, and on the Parameter Panel – tuning elements of its parameters.
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If the selected model contains version and (or) variants of geometric representation, then in the dialog, you can select the required design/version. The geometry of views will correspond to the selected version/variant. If the model contains executions additional numbersyou can also select the required additional number. |
If necessary, you can re-select a model (execution, variant) in the process of creation of views using the Source File field of the Parameter Panel. Working with the field is described in table Parameters linked to the model.
3.If it is required to create view 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 field Solids. 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 Orientationlist, 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 click Fix custom orientation button 
, located next to the orientation list. 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 table Parameters linked to the model.
5.If the view is to be rotated, then in the Rotation angle field, enter the required value of angle.
6.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.
7.Set the scale of the view and the color of its display. Details...
8.If, for creation of a view, an assembly model with configured spacing parameters is selected, then it can be displayed it in the drawing in a spaced view. To that end, enable the Explode Assembly components option.
9.If, for the creation of a view a model in which there is a sheet solid and the flat pattern parameters were set up is selected, then it is possible to display a sheet solid in the drawing in an unfold view. To that end, enable the Flat patternoption.
10.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...
11.Configure the structure of the view caption. Details...
12.Configure the rendering of view lines. Details...
13.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 details on transferring objects and detailing elements...
14.Specify which designations should be automatically created in the views. To that end, in the Create group, in the Objects section, include the corresponding options in the Symbols in the drawing list.
More details on designation creation...
15.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 details on the transfer of properties from the model when creating a view...
16.Select the point which will be used as the datum point of a view. To that end, in the Datum point of a view group, press one of the following buttons:
Center of bounding rectangle or contour,
Origin of view coordinates.
17.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.
Creation of the view will be completed. In the graphic region, there appears an image of the view, and in the Drawing tree – its icon and the name.
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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 Yesto immediately save the model file or click nanto cancel saving. In any case, the model image in its current view is created in the associative view. |
Once the view is created, the command to Creation of projection view. The created view is automatically selected as the reference view.
18.To complete the command, click Finish 
button in the heading of the Parameter panel.
See Also
