Navigation:  Drawing Creation > Drawing Views. Detail Views

This chapter describes an auxiliary element of T-FLEX CAD system – the drawing view. Additional views, detail views, local section views and sections – all these instances are supported by Drawing View. This functionality handles situations when elaboration to the images on the main views is required. This can be an additional view, and, in particular, a scaled view. The functionality allows collecting together on one page elements from different pages, inserting an image (or a portion thereof) from one page into another page in various scales, even create a simple assembly from parts contained in the same document.

 

Main concepts

A drawing view is an element of T-FLEX CAD that allows displaying contents of one page (or a portion thereof) on another page, scaled to the desired factor. It is a rectangular area of specified size used for displaying the contents of another page.

The page displayed within a drawing view can either be selected from the list of existing pages in the document or additionally created for the drawing view. The newly created page is assigned the type "Auxiliary". A drawing view can be nested, that is placed within another drawing view.

Location of the drawing view box on the main page can be specified by either direct selection of the fixing point and the view rotation angle or with the help of the fixing vector located on the view page.

The main purpose of a drawing view is to display on one page drawing elements of different scales. For example, one can create a drawing of some object on one page and then create drawing views of this object on other pages that will display portions of this drawing to various scales.

Besides, drawing views can be used simply for collecting the contents from different pages. This may be used for adding to the main drawing some additional, local views and sections created on other document pages in different scales. This capability is the most common way of using drawing views in T-FLEX CAD. Note that the images on the detail views can be copied from other pages of the current document when the drawing view is created (see section “Creating Detail View”), and enhanced with captions of the view notations (see section “Creating Detail View with Caption”).

The image displayed on a drawing view can be created or edited either on the original page of the drawing view elements, or directly in the view area of the main page by activating the view.

 

 

Creating drawing views

Drawing views are created using the command “SD: Create Drawing View”:

 

After invoking this command, the following options will appear in the auto menu:

       <О>        New Drawing View

       <V>        New Detailed View        

       <С>        New Detailed View with Caption

Working with Draggers of Drawing View

For defining location, rotation angle and dimensions of the drawing view, a special type of the cursor in the form of the dynamically movable rectangle with markers is used. Markers can be used for modifying location, rotation angle, the scale and the size of the view, location of the fixing vector or fixing point.

The markers are used as follows: a marker is activated simply by pointing the cursor and clicking . Then the marker can be moved to the desired position. The second click fixes the new position of the view. Alternatively, the marker can be “dragged” by moving the cursor with the mouse button held down. In this latter case, the placement of the view in the new position occurs on releasing the mouse button.

As the placement or parameters of the view are modified, the original state stays in display.

To change the view box size, the square-shape markers are used, located in the corners and at side midpoints of the view box. When pointed at by the cursor, the latter changes to a two-headed arrow .

The marker provides for modifying the view scale, that is the scale factor of the page display in the view box. The exact value of the scale can be entered in the view parameters dialog box.

The marker allows changing the view rotation angle about the fixing point. (In the case the view was based on an existing page and a fixing vector, this will be the rotation angle of the fixing vector.)  The exact value of the rotation angle can be entered in the view parameters dialog box.

For moving the view image relative to the page, on which it is located, the marker or the marker of the fixing point of the view (in the form of the filled square) can be used.

Location of the fixing point of the view is shown with the marker in the form of the unfilled square. When  creating the drawing view on the basis of the existing page with the help of the fixing vector, the location of the given marker coincides with the origin of the fixing vector.

For modifying the fixing point of the view, point at the marker for fixing the view while holding the button <Shift>. After that, to select the fixing point, you can pick (by pressing ) one of the characteristic points of the view box (corners of the view box and the midpoints of its sides). You can also specify the fixing point of the view arbitrarily by using <Ctrl>+ .

It is also possible to change the location of the fixing point of the view with the help of the option of the auto menu for the command of creating/editing the drawing view.

For moving the drawing view area (that is, the drawing view box relative to the page displayed in the view), the marker is used.

Originally, the boundaries of the box coincide with the boundaries of the displayed page. Shifting the view with respect to its page makes sense only when a portion of the page is supposed to be displayed on the view. In this case, the “Clip Image” flag is usually checked in the parameters dialog box, and the view box manually reduced to the desired size.

Creating Drawing View

After entering into the command “SD: Create Drawing View” the option becomes active by default. This option allows the user to create a simple drawing view. The created view can display the contents of already existing page of the current document as well as of the new page, automatically created by the system for the given drawing view.

To fix the view at a node, one can use the following automenu option:

       <N>        Set relation with Node

The location of the created view (coordinates X and Y of the fixing point) can be also specified in the command's properties window (in the group “Basic parameters”).

By default, the snap of the drawing view is carried out at the center of the view box. It is possible to select another fixing point of the view with the help of the option:

               Fixing Point of View

After specifying the view location, the user can define more accurately the location, the size and the scale of the view by using the markers around the view box (the use of markers is described in section “Editing drawing views” in more detail).

It is possible to specify parameters of the created drawing view in the command's properties window:

Fixing Vector can be used for placing a drawing view, just like a 2D fragment. This also allows controlling the current page layers visibility as the page is displayed on a view. Use of fixing vectors is described in details in the chapter “Assembly Drawing”.

The group of parameters “Parameters” combines auxiliary parameters of the drawing view:

Scale. Defines the scale factor of the drawing view, which is the scale of transformation of the view page as it appears on the main page.

Rotation Angle. This parameter is inaccessible when using a fixing vector.

Clip Image. When set, the page in the view is clipped to the extents of the actual image contained on the page.

Scale Lines. When set, the thickness of the graphic lines on the drawing view will be affected by the “Scale” parameter.

To complete view creation, use the option . As a result, a rectangular area of the drawing view will be created, with the contents of the specified page or its portion displayed within.

Creating Detail View

The option allows the user to automatically create the detail views on the basis of the drawing view. As a result of its use, the drawing view containing automatically created copy of the selected elements of the drawing will be created. In addition, the image on the drawing view page will be automatically augmented with the view caption.

When using this option, the following will be created:

1.A new drawing view (based on a new “Auxiliary”-type page). The drawing view parameters are set “by default”;

2.A translated copy (as in the command “Drawing|Copy|With translation”) for associative copying of the selected elements onto the drawing view page with specified parameters (scale and rotation angle);

3.The caption for the detail view.

As a result, a rectangular area of the drawing view is created on the main page with copies of selected elements displayed within. The size of the drawing view, as well as the size of its respective page, is defined automatically by the system based on the size of the copied entities. If necessary, the size of the drawing view and its page can be modified manually.

For creating the detail view, it is necessary to do the following:

1.Select the elements to be copied from the original drawing;

2.Select the fixing node for the copied elements;

3.Define location of the detail view (that is, the location of the drawing view containing the detail view).

After invoking the option the options for selecting the copied elements will appear in the auto menu:

       <M>        Select Mode

       <M>        Deselect Mode

       <I>        Select Other Element

When the option is turned on all elements selected on the drawing are added to the list of the copied elements. For quick selection of several elements, you can use the selection with the window. When the option is turned off the selected on the drawing elements will be removed from the list of the copied elements. For quick selection, you can use the selection with the window here as well.

Complete the selection of the elements, which will be copied onto the detail view, by pressing .

After selecting the copied elements, the system will prompt the user to specify the fixing point of these elements (it will serve as the initial point of the copy to be created). The option for selecting a 2D node will appear in the auto menu:

       <N>        Set relation with Node

After choosing the fixing node, the dynamic image of the created detail view attached to the cursor will appear on the screen. The location of the detail view on the drawing has to be selected next. After snapping the view, its location and size can be adjusted with the help of the markers for editing the drawing view.

To make the caption of the detail view change its location according to the modifications of the drawing, it is recommended to fix the drawing view to the 2D node.

Before completing the detail view creation, the dialog for specifying parameters of the created view will remain available in the command's properties window. In this dialog you can specify the precise values for the fixing point of the view, and also the following parameters:

To complete view creation, use the option . For the view constructed, the caption will be automatically created. The obtained view can be edited and augmented, if required.

 

Creating Detail View with Caption

Creating the detail view with the caption with the help of the option is an extension of the case of creating just a detail view (the option ). The option creates the detail views clipped by the specified contour and with automatic creation of the caption for the detail view on the given drawing.

As a result of its use, the caption for the detail view is created on the drawing. The image of the detail view itself is automatically clipped by selected contour (circle, oval or rectangle) and augmented by the view caption. The obtained image can be edited later by using the standard tools of the T-FLEX CAD.

When creating the detail view with the caption, the following will occur:

1.Creating the new drawing view (on the basis of a new page of the type “Auxiliary”). The values of the parameters of the drawing view are set “by default”;

2.Creating a copy with translation for associated copying of the selected elements onto the drawing view page with the specified scale and rotation angle. Clipping the image to be copied by the automatically created hatch of the specified form;

3.Creating detailing elements for the detail view (view caption, caption of the detail view).

After invoking the option it is necessary to do the following:

1.Select the fixing node for the elements which will be copied;

2.Specify the center of the selection area for the detail view;

3.Specify the form and size of the selection area for the detail view;

4.Specify the location of the leader line jog for the detail view caption;

5.Specify the location of the detail view (that is, the location of the drawing view with the detail view).

Note that in the described sequence of steps, there is no step for selecting the original elements to be copied. When creating the detail view with the caption, the collection of the copied elements is determined by the view selection area – all 2D elements at least partially contained in the specified area will be copied.

For selecting the fixing node, in the auto menu of the command the following option will be available:

       <N>        Set relation with Node

The fixing node will determine the initial location of the fixing point for the created view. If, upon specifying the fixing node, the user selects an arbitrary point on the drawing (with the help of ), then at this point the free node, which will be selected as the fixing node, will be automatically created.

After specifying the fixing node, the system will ask to specify the center of the selection area. This can be done by picking an arbitrary point in the drawing's window (with the help of ) or by specifying exact coordinates in the command's properties window.

The center of the selection area can be also defined by selecting a 2D node or offset of the center point from the fixing node (selected at the previous step). For selecting the 2D node the following option is used:

       <N>        Set relation with Node

For specifying the offset of the center of the selection area from the fixing node, the following option is used:

       <A>        Set Relative Position

After selecting the center of the selection area, the form and dimensions of the area need to be specified.

After specifying the view selection area, the location of the leader line jog for the view caption has to be defined. Dynamic image of the leader line jog will follow the cursor. Pressing in the drawing's area will fix the jog location. The jog location can be also specified in the command's properties window (by specifying the coordinates of the starting point of the jog in the group “Basic parameters” of the properties window).

For changing orientation of the jog for the view caption, the following auto menu option can be used:

       <Z>        Change leader line jog orientation

After specifying the jog location, the dynamic image of the created detail view, attached to the cursor, will appear on the screen. The location of the view on the drawing has to be specified next.

To make the caption of the detail view change its location according to the modifications of the drawing, it is recommended to snap the copied element to the 2D node. After snapping the view, its location and size can be adjusted with the help of the markers for editing the drawing view. Complete the view creation with the help of the option .

For the constructed view, the caption will be automatically created. The obtained image can be edited and augmented, if required.

 

Creating Detail View with Breaks

On any detail view the user can create breaks, if necessary. The number of breaks on a single view is not limited. To create breaks, use the following option:

After invoking this option, the system will transfer to the mode of creating/editing breaks on the current view. In the command properties window an additional section “Breaks” appears in which all breaks created on the given view and their parameters will be included.

Note that if the breaks are not yet present on the current view, then after entering into this mode the new break will automatically be created. If the view already has the breaks, then the new break is not created and the system waits for selection of one of the existing breaks for editing its parameters. In this case it is possible to create the new break by pressing the button next to the list of breaks in the command’s properties window. To remove the break, we use the button.

The following options will be available in the automenu:

By default, the system prompts us to create a horizontal break. This will be shown on the view as a hatched rectangular domain. The hatch lines show the direction of the space compression (perpendicular to the break lines).

The next figure shows an example of the view with the break.

If several breaks are created on the view, then the current break (that is being created or edited at the present moment) is displayed with green color, and the remaining breaks are shown with grey color.

Location of the right and left boundaries of the break can be modified simply by selecting the boundary line with the help of and by moving it to the desired location. By pressing again we fix the new location of the boundary.

When moving the break’s boundary, the additional option is available in the automenu:

With the help of this option, the break’s boundary location can be snapped to a 2D node.

End.  The value that determines the location of the right boundary – for horizontal break, or the upper boundary – for break at an arbitrary angle.

If the values are specified as variables, then after the numeric value the corresponding name of the variable is indicated in square brackets.

Other parameters of a break specified in the properties window are common for all breaks of the same drawing view.

Boundaries of the lines of break’s label are defined based on the marginal graphic lines, individually for each side of each break. When defining the boundaries, the formatting elements (dimensions, texts etc.), and also 2D fragments for which the special viewing mode without clipping was specified are not taken into account.

If necessary, the user can make automatically defined view’s boundaries more precise. To do so, we can use the option:

After invoking this option, it is necessary to indicate two lines of the drawing view.  These lines can be both the graphic lines and construction lines (line, spline or function).

When creating/editing a break it is also possible to specify the following parameters in the properties window:

Distance between break lines determines the distance between the parts of the broken view.

Angle. This parameter specifies the angle of rotation of break lines with respect to a horizontal line. Positive direction is in the counterclockwise direction.

Extension lines length. If this flag is absent, then only that part of the break line will appear on the view which directly intersects the image of the view. Otherwise, the break line will go beyond the view’s margins by the magnitude indicated by this parameter.

Do not move breaks. When this flag is enabled, the view’s lines that remain after applying the breaks do not change their location.

The break of a projection can be bounded by the lines that have various shapes. It can be a straight line, wavy line or zigzag line.

Hide break lines. With the help of this flag visibility of break lines can be controlled. When the flag is enabled the break lines are not displayed on the drawing view.

To edit the list of special elements it is required to press the button to the right of the list. To add the element to the list, select it on the drawing with the help of . By default for all selected “special” elements, the “without clipping” mode is set. To change the clipping mode, it is sufficient to select the required element in the list – the mode will change (cyclically) whenever we click .

On the view the elements included into the list are marked with a frame, and furthermore, the elements for which the « Clipping» drawing method was selected, are marked with slanted lines.

To remove an element from the “Special elements” list, it is required to select it in the list with the help of and press the button. It is also possible to indicate the required element in the drawing’s window by pressing <Ctrl>+ . You can remove all “special elements” with the help of the button.

After all parameters of the break are specified, it is required to complete its creation by pressing

 

Particulars of scaling drawing views

The "Drawing view" element and based on it detail views are created using various T-FLEX CAD instruments (the view page, the drawing view mechanism, the copy functionality). Each of these instruments has its own settings, including the scale:

1. Drawing view page scale (defined under the command ST: Set Document Parameters);

2. Drawing view scale which is the scaling factor of the drawing view page display on the detail view (defined in the drawing view properties dialog box – "Image > Scale");

3. The Scale of the copying the view elements (available in the properties window of the drawing view when using the options and ).

All these scales are superimposed in the image of the drawing view on the host drawing page.

When creating a drawing view using the options of the command "SD: Create Drawing View", the user defines only two of these scales (for example, the scale of the drawing view and the page scale when using the option , or the scale of the view image and the copying scale when working with the options and ). The missing scale is assigned to default value. The user can manually modify the values of all types of scale (see next section), however, in this case, the user needs to clearly understand the mechanism of the scale array.

 

For example, consider the drawing view of a shaft on a diagram in the beginning of this chapter. This drawing view of the shaft in axonometric projection was performed with the page scale equal to 1 and the drawing view  scale equal to 0.5 (1:2). As a result, the image of the view on the main drawing page has the cumulative scale equal to 0.5. By changing the drawing view page scale to 2 (2:1), we will get the axonometric projection of the shaft on the main page to the 1:1 scale. Should we change the view page scale to 4 (4:1), the cumulative scale becomes equal to 2 (2:1).

The detail view (View A) in this example was created using the option . The copying scale and, therefore, the drawing view page scale is equal to 4 (4:1). Meanwhile, the drawing view scale is equal to 1. As a result, the cumulative scale of the detail view image is equal to 4.

 

Editing drawing views

Editing of a drawing view is done by the command "ESD: Edit Drawing View". The command is called as:

 

Upon calling the command, an option appears:

       <*>        Select All Elements        

       <R>        Select element from list

       <Esc>        Exit command

Once all drawing views are selected by the option , they are highlighted, and additional options appear in the automenu:

       <Del>        Delete selected Element(s)        

       <Esc>        Exit command        

Upon selecting a particular drawing view by clicking it , another option appears in the automenu:

               Fixing point of view

       <P>        Set entity parameters

       <I>        Select another nearest element

       <B>        Add or edit breaks

The option allows the user to modify the fixing point of the drawing view being edited.

The option brings up the "Drawing View Parameters" dialog box:

Page. Displays the name of the auxiliary page corresponding to the selected drawing view.

The parameter "Scale" defines the scale factor of this page.

Clip Image, Scale Lines, Drawing Scale, Rotation Angle. These parameters affect the display of the drawing view area on the original page.

Layer, level, Priority. Define the values of the respective system-wide parameters.

 

The selected view is highlighted as a box with markers along the perimeter. The markers control position, rotation angle, scale, view size and the position of the fixing vector or fixing node.

Working with the markers is carried out in the same way as when creating the drawing view (or the drawing view of the element).

The following option completes drawing view editing:

       <End>        Finish Page View editing        

The option enables the mode of creating/editing breaks on the view.

 

Editing the image on a drawing view

The image on a drawing view can be edited in two modes:

1. On the drawing view page – as a regular drawing;

2. On the main page, by activating the appropriate drawing view. The view can be activated "in place" or in a separate window. Drawing view activation is done via the context menu after selecting the drawing view, or via commands in the menu "View|Drawing view".

Upon selecting one of the drawing views by clicking on the drawing page, the following commands become available in the context menu:

Activate Drawing View . Upon calling the command, all elements on the current page, except for the elements of the drawing view, are grayed out. The boundaries of the drawing view and the drawing view page become highlighted.  The graphics of the drawing view can then be edited in a usual way.

Activate in new window . This mode differs from the previous in that a new window is opened for editing that contains the graphics of the selected drawing view.

Drawing View Parameters . Brings on the screen the dialog box of the command "ST: Set Document Parameters" with the selected drawing view page settings.

 

A context menu appears on right clicking over the lines on the view created by copying (in the activated drawing view area on the main page or on the view page), with the following commands under the "Move Copy" group:

 

-"Parameters" - opens dialog of transformation parameters where you can change scale and angle of rotation.

Two extra options appear at this stage:

Model scale correction (enabled by default). This option is available only for “move” transformations  automatically created for the detail view. When this option is enabled, the assigned scale value is replaced by the calculated scale as follows:

 

 

Thus, the scale of original page is considered in the movement result. This allows you to obtain correct image of detail view when scaling is used on the original page.

 

Consider page scales. This flag can be used for the drawing views created with the option , when scale of the original page and view page differ from 1:1 and do not match. When this flag is enabled the resulting view scale will take into account the scale of both pages:

 

Setting this parameter allows you to achieve the correct correspondence of element sizes between the original drawing page and drawing view.

 

Adding to and modifying the image of drawing view

The image created by the and options may need modifications or additions, for example, add chamfers, rounds, clipping line, or place dimensions). One shall keep in mind that these options create graphics based on the "XM: Copy with translation" functionality, therefore, it is subject to all rules and limitations imposed on direct use of this command. Thus, only graphic lines, hatches, 2D fragments and projections are copied. The snapping nodes of the copied lines can't be modified. The copied elements can only be deleted, hidden by the command "ESO: Hide/Show Elements", or their parameters modified (for example, lower the level). Besides, these can be used for snapping the construction lines (see the chapter "Lines") for new element creation. Therefore, if editing a view involves modifying existing graphic lines, two ways of handling are possible:

1. Break association of the copies with the original elements using the command "Explode Copy" of the context menu. As associations are broken, free nodes are created, thus turning the graphics on the view into a sketch suitable for modifications. One should keep in mind that further modifications of the original elements of the drawing will not propagate on the drawing view graphics, thus breaking its parametric behavior.

2. Create new graphic lines based on the copies. To do this, first create construction entities snapped to the copy entities. Then, hide the entities of the copy if necessary. Instead of the hidden lines, create new ones by snapping to the newly created construction entities.

 

Clipping image by an arbitrary hatch

Updating detail view with label

In the context menu of detail views created with the help of the option (detail view with label), additional command “Update drawing view” is available. It allows us to update the structure of the drawing view after the original image has been edited.

The selection of elements is carried out in the domain of the label’s note, with the use of the current filter of elements. Only those elements which were created upon creation of the view or the previous update of the view are removed from the displayed page. The elements added to the displayed page after creation of the view are retained.

Exploding Drawing View