Dialog Box: New Drawing

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

Label
The name is entered automatically. As an example, a model whose ID is Ex410Mockup.
Ex410Mockup (first drawing).
Ex410Mockup_2
Ex410Mockup_3
etc.
Scale
Select a suitable scale.
  • The program remembers the previously selected scale during the working session.
  • The scale is presented for detail views and section views
Sheet/No sheet
Select the sheet.
  • No Sheet is an alternative.
Once you have selected the scale and the sheet, you can see the placement of the projections on the sheet at the bottom of the dialog box.
  • If necessary, you can change the scale or sheet.
Template
You can select a template document from which the settings displayed in the dialog box will be read.
The following items are currently not available in the template document:
  • Eur/USA view
  • Projection space
  • Sheet, if the drawing of the template document is old
  • Section views
Projection
The default is setting Eur, and the alternative is USA.
Select the main projections
Select the main projections
  • a: front
  • b: top
  • etc.

Click Select a if you want to select the so-called front projection from the model.
If you selected the front projection from the model, the program displays the Select b button, which allows you to select the top projection from the model.
Flatten sheet metal model
If a sheet metal part is in the model window and you want a flattening projection for the drawing, select flatten sheet. When you click Confirm, the properties of the parallel drawing are opened.
  • flatten sheet
  • When the other projections of the drawing have been created, the program opens a dialog box and asks for the properties of the flattening projection Flattening to a Drawing
Select another projection
If no other projections are selected, the default is None
Select another projection, if necessary.
    • ISO, 45 Back Right.
    • ISO, 45 Front Right.
    • ISO, 135 Back Left.
    • etc.
Show the viewing direction from the model
If you select Viewing direction, the program opens the Viewing Direction dialog box

Enter 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) or
Click Select at Model, and select the model face that defines the direction of the projection.
The option Attach to surfaces binds the direction of the projection to the selected face.
Perspective
The option does not affect the main projections.
Select Perspective, if you want the projection, for example ISO 45 Back Right, displayed as perspective.
Exploded view
The option does not affect the main projections.
Select the Exploded view, if you want the projection, for example ISO 45 Back Right, displayed as exploded.
Presentation
The default drawing mode of the projection in a model drawing is wireframe, 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.
  • Wireframe is a traditional mechanical drawing consisting of lines.
  • Shading is a quick method, but you cannot dimension the drawing.
  • Shading+Wireframe
    • When this drawing mode is selected, you can dimension any other projection except a perspective projection
  • LightWorks shading (requires the Visualization add-on option).
    • You cannot dimension the drawing.
  • Lightworks shading+Wireframe (requires the Visualization add-on option) When this drawing mode is selected, you can dimension any other projection except a perspective projection.
Advanced
Available when you have selected the shading or LightWorks drawing mode.
Advanced settings for shaded drawing modes:
  • Select Precision. A greater number is more accurate, but the drawing will also be heavier.
    • 500: fast
    • 2000: normal. This is usually sufficient for paper prints.
    • 4096: best
  • Select on or off Remove background.
  • Select on or off Anti-aliasing.
  • Select on or off Edges visible.
  • Select on or off Use extended photorealism.
Advanced settings for LightWorks drawing modes:
  • Select Precision.
    • 500: fast
    • 2000: normal. This is usually sufficient for paper prints.
    • 4096: best
  • Select on or off Remove background.
  • Select on or off No shadows.
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.
  • If the shape lines of the projection in the drawing are drawn incorrectly, edit the projection and change this selection.
  • Defaults starting with version 29.0.00 (Vertex 2023).
    • In Vertex G4, the part model drawing is done with exact silhouettes by default.
    • In Vertex G4, the assembly model drawing is done without the exact silhouettes by default.
    • In Vertex G4 plant, both part and assembly model drawings are done without exact silhouettes by default.
Also for spline surfaces
Precise silhouette lines (edge lines) are drawn for the part's spline faces.
  • If the shape lines of the projection in the drawing are drawn incorrectly, edit the projection and change this selection.
Centerlines
Defines the automatic drawing of centerlines for circles, arcs, sphere and cylinder surfaces.
  • Center lines of the arc will be drawn when the arc sector meets the minimum default value: 180 degrees.
  • It is not recommended to add centerlines to an assembly drawing, as their generation slows down the processing of large assembly drawings.
For example, a drawing of a polar hole pattern
  • In a polar pattern, a circle or an arc of a circle is drawn as a guide line.
  • Centerlines is selected on the left.
  • Centerlines and Auxiliary geometry are selected on the right.
(Centerlines) Also for pipe parts
The centerlines of pipe parts will be visible in the projection.
  • A: No centerlines
  • B: Centerlines
  • C: Centerlines and Centerlines for pipe parts.
Auxiliary geometry
Auxiliary geometry such as guide lines, cross sections, and auxiliary planes are drawn.
Note that you can also draw auxiliary geometry in a single projection.
In a shaded projection, the auxiliary geometry is drawn if the part is visible in the drawing.
Example: A chair frame modeled using a guide curve and cross section.
  • On the left, the auxiliary geometry is visible and on the right is not.
Hidden Lines
The hidden lines are drawn with dashed lines.
  • Hidden lines are not drawn on the left.
  • On the right, hidden lines are drawn.
Colored Hidden Lines - You can define the color of the dashed lines being hidden in the Settings. Define the Color of Hidden Lines
Machining features
Machining features are visible if you select Machining features.
  • The visibility of machining features in the model does not effect their appearance in the projection of the drawing.
  • Get to know machining features Machining Feature
  • On the left, a normal drawing with the machining features not visible.
  • On the right, a drawing showing the geometry of the machining features.
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.
  • A: Draw as virtual shape lines (thin). This setting is best suited for the part models.
  • B: Draw as shape lines
  • C: Lines are not drawn. This setting may be well suited for profile structures.
Automatic dimensioning
If you select Automatic dimensioning, the Settings button opens next to it.
The button opens the dialog box Automatic Dimensioning Settings.
  • Select the desired dimensions and click OK.
Note:
  • You can add a projection to the model drawing. Select the context-sensitive function Projection in the drawing.
  • You can edit the projection settings. Select the projection and then select the context-sensitive function Properties.