Drawing Derivation - Settings for: Drawing Sheets, View Groups, Views + Sheet Developments

Drawing > Itemisation/Detailing > Drawing derivation

In the Drawing parameters of the Derived drawing dialogue window, you can specify various settings which influence the layout and representation of the derived drawing. These settings can be specified for:

• Drawing sheets,
• View groups,
• Views and
• Sheet developments,

by clicking the corresponding button.

Settings for Drawing Sheets

In this dialogue window you specify the settings for the sheets of a derived drawing.

The Settings for drawing sheets dialogue window

• Distances
  Specify the horizontal and vertical distance between the view groups.
• Layout
  Here you specify the size of and the frame for the drawing sheet.
• User-defined
  The sheet size will be defined by explicit specification of width and height. If the Adjust scale to frame size checkbox is active, the view groups/views generated by the derived drawing will be automatically scaled in such a way that they fit into the created drawing frame. Please note that this setting can slow down the drawing derivation, as an optimally scaled arrangement will require multiple scaling of all generated views.

• DIN_...
  The sheet size will be defined by the size of a predefined DIN frame, e.g. DIN_A3. If you want the scale of the view groups/views to be automatically adjusted to the frame size, activate the Adjust scale to frame size checkbox.
• Fit DIN frame
  If you select this option, HiCAD automatically selects a DIN frame which contains the created view groups entirely and in an unscaled state. The Adjust scale to frame size option checkbox will be greyed out when this option is selected.

In addition, you can specify for DIN formats that an appropriate drawing frame will be inserted and the corresponding title block will be filled in automatically.

Please note:

• The derived drawing will be spread over several sheets if required.
• When arranging view groups on a drawing sheet, the representation of BOMs and title blocks will be automatically taken into account as well (if you activated the representation of these elements).

Settings for View Groups

In this dialogue window you specify the representation of view groups.

The Settings for view groups dialogue window

• Distances
  Specify the horizontal (1) and vertical (2) distance between the views of a view group.

Distance between views

• Scale
  Select the desired scale in the listbox. If you want axonometric views to be automatically adjusted, activate the corresponding checkbox. The axonometric view will then be adjusted in such a way that is will not require more space than the rest of the view group. A typical use case would be a beam or profile in shortened representation. In such cases the unshortened axonometric view will be downsized.

Adjusted axonometry

The All views checkbox is only active for subsequent changes of settings!

• Visualisation
  Specify the visualisation type of the views:
• Glass model,
• Hidden Line or
• Hidden Line dashed.
  

The visualisation can be specified separately for standard views, sectional views and axonometric views. Default values are:

• Standard views: Hidden Line dashed
• Sectional views: Hidden Line
• Axonometric views: Shaded with edges

The All views checkbox is only active for subsequent changes of settings.

• Beam shortening

Activate this checkbox to display Steel Engineering beams and profiles in shortened representation.

Please note the following:

These shortenings of views will not take effect in axonometric views with shaded representation. Furthermore, it can happen that beams are not displayed in shortened representation if the Automatically adjust axonometric views in the Scale area has been activated. In this case it may be possible that a scale for the axonometric view will be found that does not lead to a shortening according to the selected shortening parameters.

• BOM
  If this checkbox is active, a corresponding BOM is inserted in the view group of an assembly.

Example of a view group with BOM and frame

The RMS file specified in the API script partslist.CS (HiCAD EXE-directory) determines the BOM layout. By default, this is the file rmS_dstv_stueckliste.RMS.

• Frame
  If this checkbox is active, a frame is placed around the view groups. You can delete the frame of a view group manually if desired. Right-click the frame and select the Delete frame function in the context menu.

When arranging view groups on a drawing sheet, the representation of BOMs and title blocks will be automatically taken into account as well (if you activated the representation of these elements).

Settings for Views

Here you specify the settings for views, e.g. the type of dimensioning, the representation of designation tags, the part environment (adjacent parts) etc.

The Settings for views dialogue window

• Dimensioning
  The views of the workshop drawing can be dimensioned automatically. The following options are available:
• Do not create
  If you do not want to use any dimensions, activate this option.
• Conventional
  If this option is active, the settings defined via the Dimensioning Settings function in the Management menu are used for the dimension.
  

• Dimensioning rules
  Dimensioning rules are always part of a Configuration. If you have activated the Drawing parameters, From configuration option in the workshop drawing dialogue window, the dimensioning rules of the selected configuration (e.g. COLUMN/COLUMN) will be used. If the Drawing parameters, Set in dialogue option is active, the dimensioning is performed according to the rules of the DEFAULT Type of use.

• Beam annotations
  If you want the beam/profile annotation to be displayed, activate this checkbox. The position of the annotations is determined by the entered value.
• Beam shortening
  Beams and profiles can be displayed as shortened representations in workshop drawings. You can specify the shortening factor (%) and the minimum shortening length for the shortened representation.
• Sectional views
  For attached parts, e.g. front-welded plates, you can automatically create the corresponding sectional view. The viewing direction of the sectional view is from the centre of the beam to the attached plate. The cutting line of the sectional view is created parallel to the attached plate. The distance from the attached element can be specified in the Distance of cut plane input field.

The created sectional views are sectional views with depth limitation. You specify via the Views to be created for: Assemblies option whether the sectional view will be created.

• Designation tags
  In this area you specify, via activation of the corresponding checkboxes, which elements you want to annotate in which views. To select the views, click the View button and activate in the displayed dialogue window the required checkboxes. All annotations are automatically placed close to the part and are arranged collision-free.
• Symbols
  You can also display the system axes annotations, i.e. the axes of a Steel Engineering grid, in a workshop drawing if required. This is however only possible in views for assemblies.If this checkbox is active, you can specify, via a click on the View button, in which views you want to display the axes annotations.

Representation of system axes

In addition, you can narrow the system axes search by activating the Restrict search checkbox and specifying the area to which the search is to be applied. The value determines the distance (1) from the beam axis, resp. from the beam start/end.

Restrict search for system axes

HiCAD displays the annotations specified in the grid parameters.

• Part environment
  The environment of a part, i.e. adjacent parts within a specified area, can also be displayed in workshop drawings. To display the part environment, activate the Show environment checkbox. Click the View button to specify in which views you want to display the part environment.

The Settings tab enables you to set various parameters for the part environment, such as the area for adjacent part search, or the representation of the part environment.

The Settings for part environment dialogue window

• Part search
  Here you enter a distance value determining the area that is used for adjacent part search.
• Limit view
  If you do not want to display the entire part environment, you can limit the view. Activate the Limit checkbox and enter the values for the limitation. Elements outside the specified area will not be displayed.
• Representation
  Parts located within the selected area can be displayed in a different edge and surface colour.Activate the corresponding checkbox and select the desired colour. In addition, you have the option to make the parts transparent - independent of the layer selected.
  
  

Representation of the part environment (yellow), without (left) and with view limitation (right).

Please note:

• AutoLabeling ensures an optimally arranged, collision-free placing of the designation tags close to the corresponding parts. This means that collisions (overlaps) of annotations, item numbers or dimensionings are prevented.
• If you use the dimensioning rules of one of the predefined configurations, and have activated the system axes, the distances to system axes are displayed as negative values for beams or profiles whose start or end is located between the system axes.

Example: Dimensioning rules, Show system axes

Example: Dimensioning rules, no system axes

If you use the drawing parameters of a configuration, the part environment will not be displayed by default. To change this, open the Configuration Editor (ISDConfigEditor.exe) and select GENERAL > DRAWINGS > CREATE > USE CASE-DEPENDENT > TEMPLATE > VIEWS > PART ENVIRONMENT. Set the parameter Part environment (0: no, 1:yes) to 1.

Settings for Sheet Developments

In this dialogue window you specify the settings for the development of sheet metal parts.

The Sheet Development Settings dialogue window

• Type
  Here you specify the scale, determine whether the development will be dimensioned, and specify the handling of angular dimensions in sectional views. Via the Mode list box you can select whether you want a representation with or without hidden edges. Default setting is Without hidden edges.
• Designation of bend lines
  In this area you can select text colour, font, font size and layer for bend line designations.
• Representation
  Activate the appropriate checkboxes to select the blank parameters that you want to be displayed in the workshop drawing.
  If the With sub-parts checkbox is activated, the sub-parts of a flange will also be displayed in the development, i.e. weld nuts. If you activate the With tools checkbox, the contents of the WZNR column in the catalogue will be output for punch tools.

Workshop drawing of a sheet metal part

Please note: 

AutoLabeling ensures an optimally arranged, collision-free placing of the designation tags close to the corresponding parts. This means that collisions (overlaps) of annotations, item numbers or dimensionings are prevented.

 Related Topics

Derive Drawing • Derived Drawing: Change Settings • Derived Drawing - Views to Be Created