Specifies advanced display and processing options for the drawing view. The settings on the Advanced tab of the Drawing View Properties dialog box take precedence over their counterparts in the Advanced Edge Display Options dialog box.

Drawing View

Let Solid Edge determine VHL tolerance (recommended)

Specifies whether Solid Edge determines the VHL tolerance for the drawing view. Generally, letting Solid Edge determine the VHL tolerance provides the best results. You should only clear this check box and set VHL tolerance manually if you are having problems with drawing view quality. This option is not available for detail views.

VHL Tolerance

Specifies the VHL tolerance when Let Solid Edge Determine VHL Tolerance is unchecked. Five (5) is the highest value and provides the most accurate display. If you have drawing view problems and want to see if changing the VHL tolerance resolves them, increase the setting one value at a time and use the lowest number that provides satisfactory results. A higher VHL tolerance setting than necessary may degrade drawing view update performance. This option is not available for detail views.

Let Solid Edge determine thread axis tolerance (recommended)

Specifies whether Solid Edge determines the thread axis tolerance for the drawing view. Generally, letting Solid Edge determine the thread axis tolerance provides the best results.  You should only clear this check box and set thread axis tolerance manually if threads for holes that are slightly off parallel or perpendicular to the view plane do not display in the view. This option is not available for detail views.

Thread axis tolerance

Specifies the thread axis tolerance when Let Solid Edge Determine Thread Axis Tolerance is unchecked. You can set thread axis tolerance from 0 to 5 degrees, inclusive.

Let Solid Edge determine tangent tolerance (recommended)

Specifies whether Solid Edge determines the tangent tolerance for the drawing view. Generally, letting Solid Edge determine the tangent tolerance provides the best results. You should only clear this check box and set tangent tolerance manually if edges that should display as tangent in the drawing view instead display as visible or hidden. In such cases, a larger tolerance often corrects the display. This option is not available for detail views.

Tangent tolerance

Specifies the tangent tolerance when Let Solid Edge determine tangent tolerance is unchecked. You can set tangent tolerance from 0 to 5 degrees, inclusive.

Limit edge creation

Only generate edges inside or overlapping cropped boundaries

Reduces VHL drawing view processing time by limiting edge creation for any cropped views or independent detail views. When this check box is selected, only edges completely inside or overlapping the view cropping boundary are generated. When this check box is cleared, all edges inside, outside, and overlapping the view cropping boundary are generated.

Note:

Geometry created with the Draw In View command is not affected by this setting.

Show edges created by cutting plane line vertices

When you create a section view using a cutting plane that is defined by multiple line segments, you can use this option to show or hide the resulting edges in a drawing view.

When this option is cleared, edges created by cutting plane line vertices are hidden when you update the drawing view. When this option is set, these edges are visible. The default setting is cleared.

This option applies to 2D section and revolved section views. It does not apply to 2D broken-out section views.

Note:

Not all edge cases are handled by this processing rule. For those edges that are not, you can use the Hide Edges command to hide them.

Simplify B-spline edges

Always

B-spline geometry from part edges is always converted to simple geometry.  

Only edges outside of the plane of the drawing view

Only B-spline geometry from part edges non-parallel to the plane of the drawing view are converted to simple geometry.

Never

B-spline geometry from part edges is never converted to simple geometry.

Part intersections

Processing part intersections can yield better drawing view results in cases such as press fits, where parts slightly intersect. Changing this setting causes the drawing view to become out-of-date.

Do not process intersections (fastest)

Specifies that part intersections are not processed. This is the fastest option.

Process intersections

Without creating face intersections (fast)

Creates part edges within the intersections of overlapping bodies. The edges formed between intersecting faces of overlapping bodies are not created.

Create face intersections of threaded parts (slow)

Creates face intersections of overlapping bodies for threaded parts on which outer diameter and inner diameter threads overlap.

Create all face intersections (slowest)

Creates face intersections for all overlapping bodies. This is the slowest option.

Section View

Process partially hidden cut faces

Ensures hatching on partially hidden interior cut faces is visible only in the area that should be visible given the section view direction. This can eliminate the need to remove excess hatching using the Draw in View function. This option is available for all types of section views, including broken out sections. For complex section views, where this option may slow drawing processing, you may want to clear this check box.

Hatch ribs in section view

Provides control over the hatching displayed on cut ribs in a section view. You may want to uncheck this option when the cut line is along the rib, and not across the rib.

• When checked, cut ribs are always hatched.

  Note:

  When this option is checked, a list of ribs is not generated for selective rib display using the Override Rib Hatching dialog box, and the Override Rib Hatching command is not available.

• When unchecked, the body is hatched, but the ribs are not. This results in a visible edge between the hatched primary body and the unhatched rib.

  You can use the Override Rib Hatching dialog box to selectively choose which ribs you want to hatch and which ribs you do not.

  To learn how to do this, see the Help topic, Set rib hatching in section views.

The default for hatching on ribs in section views, revolved section views, and broken out section views is set on the Drawing Standards tab (Solid Edge Options dialog box).

Draft Quality View

View quality

Specifies the relative accuracy of the line strings that represent the part edges in the draft quality view. The higher the view quality, the smaller the facets on the line strings that represent the part edges are. View quality ranges from 1, the fastest and least accurate setting, to 3, the slowest and most accurate setting. To maximize performance, you should use the lowest value that produces the results you want. The default of 2 is suitable for most applications. If you need higher quality, convert the draft quality view to a high quality view.