New Drawing

The dialog box is opened when you create a new drawing from a part or assembly. The number of drawings is unlimited.

New Drawing of a Model

Select the drawing properties in the dialog box.

• Projection label / Header / Scale / Sheet
• Projection
• Other projection
• Drawing mode

------------------------------------------------------------------------------------

Projection label / Scale / Drawing template

Label

The name is entered automatically. For example, name Ex410Mockup (first drawing). Alternatively, you can click Search.

Ex410Mockup

Ex410Mockup-2

Ex410Mockup-3

etc.

Header

The header text is placed as the projection's title, if you create the projection Detail View, Section, New Projection. The title text and its position can be edited. You can also leave the title text empty.

Move Text from a Grip Point

Scale

The default projection scale is 1:1. Select a suitable scale. When the projection is a detail view or a section view, the scale will be displayed in the title.

If you select a new Sheet, refresh the scale by selecting Search.

Scale: autofree or autofix – Dynamic projection

The projection area can be defined so that it is drawn inside the selected rectangle always, by the function Continuous line chain. This is useful when the drawing represents a model whose dimensions vary greatly. In this way, the projection stays in the right place at all times, and the scale is defined in such a way that the geometry fits inside the rectangle.

If you draw a rectangle by the function Lines> Rectangle, Open Polyline or Closed polyline, the line chain is not continuous. Make the line chain continuous with the function Line Trimming> Concatenate Lines. If you wish to hide the rectangle, move the continuous line chain to layer 110 (hidden layer).

Concatenate Lines

If you select either Autofree or Autofix as the scale, the program will ask you to indicate a continuous rectangle line that defines the projection area limits.

The projection is scaled to the area defined by the rectangle in accordance with the calculated scale, or the projection finds the preselected scale that best fills the area, but does not cross its boundaries. When updated, the projection is always scaled in accordance with these rules.

• Autofree - The projection is scaled to the area defined by the rectangle, based on the calculated scale.
• Autofixed - The projection looks for the preselected scale that best fills the area but does not cross its boundaries.

You can reduce the size of the projection by reducing the size of the projection line (drag and drop).

The scales are defined in the settings using the keywords scale -1, Auto free and scale -2 Autofixed. Edit Settings

Sheet/No sheet

Select sheet, A4, for example. The alternative is No Sheet.

If you change the sheet, refresh the scale by selecting Search.

------------------------------------------------------------------------------------

Projection

Projection

The default is setting Eur, and the alternative is USA.

Select the parallel projection. For example, select a: front etc.

Select the projection (direction) from the model by first clicking Select a, and select the face from the model.

flattening

If a sheet metal part is in the Model window, select the projection flattening. When you click Confirm, the properties of the parallel drawing are opened.

Projection Settings dialog box

Flattening Image Properties

Flattening to a Drawing

Other

If you select Other, indicate the model face that defines the direction of the projection.

Show from model

If you select Show from Model: Indicate the model face to define the direction of the projection.

Set Viewing Direction

If you select Set Viewing Direction, define the viewing direction in the dialog box as angle values Alpha, Beta, Gamma and click OK. The default value iis (A: 0, B: 0, G: 0).

Perspective

Select the projection, isometrics projection, or select the standard projection, for example. Select Perspective.

If you select Perspective, automatic dimensioning cannot be selected.

Explosion

In the case of an assembly, you can select Explosion, for example. Requires that exploded positions have been defined in the assembly model.

Defining the Positions of an Exploded Assembly

------------------------------------------------------------------------------------

Drawing mode

Drawing mode

The default drawing mode of the projection in a model drawing is wire frame, unless another drawing mode was selected when creating a new drawing for the model. You can also select the drawing mode of a perspective projection in the drawing.

• Wire Frame
• OpenGL shading If you wish that a model's edges are drawn in the projection when using this drawing mode, select Advanced. The selected drawing mode defines the available choices.For example, the OpenGL Shading mode opens a dialog box, where you can select properties.
• OpenGL Shading+ wire frame When this drawing mode is selected, you can dimension any other projection except a perspective projection. You can soften the drafting of the lines by selecting Antialiasing.
• LightWorks Shading (add-on) When this drawing mode is selected, the projection also includes shadows. You can remove the shadows from the projection by selecting No shadows.
• Lightworks Shading+ wire frame (add-on) When this drawing mode is selected, you can dimension any other projection except a perspective projection.

Advanced

Can be selected for all other drawing mode except Wire Frame.

You can define a maximum size in pixels of the image rendered to the projection when using OpenGL and LightWorks Shading drawing modes at Max size in pixels. The recommended pixel resolution is 2000, at most 6000. The larger the pixel resolution value, the greater the detail in which the projection will be rendered. For paper printouts, 2000 pixels is usually a sufficient resolution. Note that a high resolution makes the projection update in the drawing slower. You can also select: Anti-aliasing, Remove Background and/or OpenGL Sihouette Lines.

In PDF and PostScript (driver code 7 5) printing, projections shaded and visualized with resolution value 0 have their original resolution in the printout regardless of the sheet size used in printing.

Exact Silhouette Lines

The silhouette lines (edge lines) are drawn exactly. Coarse drawing speeds up refreshing the projections, but, for example, the dimensioning of an arc will fail.

Also for spline surfaces

Precise silhouette lines (edge lines) are drawn for the part's spline faces.

Center Lines

Center lines are automatically drawn for circles and arcs. Center lines of the arc will be drawn when the arc sector meets the minimum default value: 180 degrees. You can change the value of the sector projection-specifically. Center lines will be drawn in the projection of a part drawing, even if the Center Lines option is unselected when creating a new drawing.

The function Center Lines has to be selected specifically to an assembly drawing and it's projection. The function is disabled as default, because it slows down the processing of large assemblies.

The center lines of a polar hole pattern

The drawing of polar hole patterns follows the mechanical engineering rules.

In the sketching mode, define the radius of the feature pattern to the desired value, if you have used the default value (R100).

The radius is displayed in the projection if Auxiliary geometry is selected.

If you select the two following options, the center lines of the part will be drawn in the projection through all the geometry. Can also be selected for pipe parts.

• Center Lines
• Auxiliary Geometry

Hidden Lines

The hidden lines are drawn with dashed lines.

As an example, a part model.

1. Hidden Lines – No hidden lines.
2. Hidden Lines – Hidden lines visible.

Colored Hidden Lines - You can define the color of the dashed lines being hidden in the Settings. Define the Color of Hidden Lines

Auxiliary Geometry

You can set the auxiliary geometry of a model to be displayed in the projection. Auxiliary geometry is 3D sketches, guide curves, and cross-sections.

As an example, the guide curve controlling the shape of a handle.

1. Auxiliary Geometry (visible)
2. Auxiliary Geometry

Machining Features

A machining feature is displayed in the projection if you select Machining Features. The visibility of a machining feature in an assembly has no effect on a projection of a model's drawing.

Machining Feature

Also pipe parts

The center lines of pipe parts will be visible in the projection.

The visibility of the pipe part center lines is also affected by the projection property Auxiliary Geometry.

If you select both, the pipe part center lines will be drawn in the projection through all geometry.

• Center Lines
• Auxiliary Geometry If you do not select Auxiliary Geometry, hidden lines (center lines of pipe parts) will be removed from the projection.

Automatic Dimensioning

You can add dimensions to an active projection of a drawing automatically.

1. Select a projection from the model drawing.
2. Select the context-sensitive function Properties.
3. Select Automatic dimensioning.
4. Click the Settings button and define the dimensioning settings.
5. Select OK.

Automatic Dimensioning

Tangential lines

Apparent shape lines will be created between tangential faces. Select drawing as a shape line or thin line, or disable the drawing of tangential lines in the projection.

• As Shape Line (default) (A)
• As Thin Line (B)
• Lines Are Not Drawn (C)

You can select the drawing of tangential lines specifically for each drawing. The setting is not saved in a drawing.

Limit from Model

Limit from Model

1. Double-click the projection in the model drawing.
2. In the Drawing Settings dialog box, click the Limit from Model button.
3. Select the limiting face from the model, and move it with the cursor.
4. Select Confirm.

Draw Section Hatches

Draws a section hatch that is defined as a part property.Hatch Hatch

------------------------------------------------------------------------------------

Add sketch dimensions to a projection

You can set 3D limiting. Limit Visibility in a Model

Set the dimensions of a 3D planar sketch to be visible in the model drawing.

Add Sketch Dimensions to a Model Drawing

After selecting the properties of a projection for editing, do as follows:

1. Select Insert Sketch Dimensions to Projection in the dialog box.The 3D model window becomes active.
2. In the feature tree of the part, double-click the Sketch the dimensions of which you wish to insert into the projection.After the sketch has been selected, the Projection Settings dialog box is opened.
3. Select OK.

New Drawing of a Model

Projections in a drawing: