Dialog Box: Projection Settings

General

Label

If necessary, you can change the projection label.

Header

The header text will be set as the header of the projection.

• Header text is commonly used in detail view and section projections.
• In the section projection, the header is added automatically, based on the section line label, for example A-A.
• For the detail view header, you get the default content when you click on the field, for example DET1
• Edit the header, if necessary.
• The header text is positioned below the projection, but you can drag it to a new location.

Scale

If necessary, edit the projection scale.

• Use the preset button to select the scales allowed for the mechanical drawing.
• You can also enter another scale yourself, but we recommend using them only with isometric projections and perspective projections.
• If there is a need to edit the scale of all the projections in the drawing, then edit the properties of the drawing, not the properties of the projections.

Special scales autofree and autofix

• These special scales are intended for example for drawings of product automation systems, where the geometry of the model may vary as a result of variation, but the projections are nevertheless wanted to fit in the area of the drawing reserved for them.
• For more details, see Use the Scales Autofree and Autofix

Configuration

Select the configuration for the part displayed in the projection. If in addition to the basic configuration (0: Configuration) there are also other configurations, select the configuration which is displayed in the projection to the field.

• Add a Configuration to a Part
• Add a Configuration to an Assembly

Section views

Section Depth

You can edit the section depth value once you have added a section projection in the drawing.

• The default dimension 0 (zero) means that the part is displayed from the point of intersection to the end of the part.
• For example, dimension 1 means that a slice of one millimeter is cut from the part.
• See also: Oblique Section

Select Border Lines

Indicate the border lines in the projection, and click Confirm.

Select the section line.

Assign a new cutting line to the section view in the drawing.

1. Select a line from the drawing.
2. The direction of the arrow will indicate the part of the model to be shown in the section view. Select either of the sides.

Accurate Cut/Quick Cut

If you select Accurate Cut, the projection will be cut accurately.

• You can dimension such a projection without any problems.

If you select Quick Section, the cut is done as a 3D limiting.

• You cannot dimension the parts that area cut.
• The quick cut function is suitable for creating section projections for example large plant models.

Change the properties of the Quick Section cut if necessary

You can set the profiles and pipes dimensionable in a quick section of the drawing with the keyword sectionview_pipes_and_profiles

• The setting value defaults to 0, which means that cut pipes or profiles cannot be dimensioned.
• With the value of 1, dimensioning of profiles and pipes is possible

Change the setting

• Find a Keyword Among All Keywords
• Search a Keyword from a Keyword Group
• Change a Keyword Value

Section marking at start

Select the section mark to be included or excluded at the beginning of the cutting line.

Section hatches

Select whether to draw section hatches or not .

Section marking at end

Select the section mark to be included or excluded at the end of the cutting line.

Exploded view

Defines the projection as an exploded view, in which the assembly is displayed as exploded.

• This requires that the exploded points have been defined for the assembly model.
• See: Explode an Assembly
• See: Exploded Drawing of an Assembly

Detail views

Rectangle

The shape of the detail view is rectangular.

• The projection can also be shaded or LightWorks shaded.

Circle

The shape of the detail view is a circle.

• The projection can only be presented as Wireframe.

Flattening

Drawing Simple Geometry

A flattening projection will only be created from the geometry of a flattening surface selected from a sheet metal part (default).

• Simple Geometry – A flattening projection will only be created from the geometry of a flattening surface selected from a sheet metal part. Also draws the geometry of the forming feature.
• Simple Geometry - The flattening projection will be created by drawing all geometry lines visible in the viewing direction.

Trim Corners

• The trim corners feature only works for those corners created during modeling, which have not been separately trimmed in the flatten projection.
• If the corners are trimmed separately, the actual geometry is drawn regardless of this selection.
• Corner trimming should only be used for thin sheet materials and such bending methods, where the bending can be done in such a way that curling occurs in the corners of the sheet.

Trim Corners – The flattening projection is drawn without corner openings.

Trim Corners – A corner opening is drawn in the flattening projection.

Note: The Trim Corners function is the default, take this into account when creating a DXF file. You can change the default in the system settings.

Bendlines

Select bend lines to be included or excluded .

Holes Perpendicular

In practice: the non-perpendicular hole is converted into a maximum size (oval) hole that must be cut into the sheet in order for the shaft or similar pin to fit diagonally through the plate.

Holes perpendicular - The hole is drawn in such a size that the shaft still fits through the hole when the sheet is bent.

Holes Perpendicular – The holes drawn according to the edge lines of the hole.

Draw hatch

Select hatches (section hatches) to be included or excluded .

Reference points

Select the reference points to be included or excluded .

• Reference points are drawn at the grip points of the (cut-out) features.
• These are useful for positioning sheet punching tools.

Drawing mode

Drawing mode

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.
• Note: In assembly drawings, exact silhouettes are not very important, so it is better to clear the setting for them. The update of images showing large assemblies in particular is considerably faster if exact silhouettes are not drawn.

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.
• Note: It is not recommended to add centerlines to an assembly drawing, as their generation slows down the updating 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.

 Gravity Center

Gravity center shows the model's center of gravity in the projection, if the model has a mass calculation.

• Select the gravity center to be included or excluded .
• Update the location of the gravity center by pressing F5 key. If the mass is not up-to-date, it will be updated at the same time.
• You can also delete the lines of the center of gravity by deleting the line, but in this case updating the projection will return them back to view.
• Dimensions can be added to the lines of the gravity center, and when the drawing is updated, the dimensions are also updated.
• You can also draw your own Gravity Center mark.

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.
• 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.

• 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.

Limit from Model

With the Limit from Model function, the portion of the 3D model cut off by a cube can be shown in the projection of the drawing.

• Limit a 3D Model in the Direction of the Coordinate Axes

1. Double-click the projection in the model drawing.
2. Click the Limit from Model button.
3. Select the limiting face from the model, and move it with the cursor.
4. Click another and etc. face and move the limiting face with the cursor.
5. Select Confirm. (Confirm = V key, middle mouse button or the context-sensitive function OK.)

The same function can be used to correct the limits.

• You can remove the limiting cube only when you drag the cube outside the limits of the model's geometry.

Draw Section Hatches

Draws section hatches defined in the properties of the part on the part to be cut.

• Select section hatches to be included or excluded .
• Hatch

Add sketch dimensions to a projection

With the functions, you can add the dimensions of one sketch to the projection of the part model drawing.

• Add Sketch Dimensions to a Model Drawing
• The dimensions of the sketch are drawn in their places and in the scale where they are in the selected sketch.
• The scale of the sketch in question should be changed from the Auto scale to the same scale in which the drawing or, more precisely, the projection is.
• Add Sketch Dimensions to a Model Drawing

Add sketch dimensions to projection

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.