PartDesign Линейный массив

This page is a translated version of the page PartDesign LinearPattern and the translation is 26% complete.

Симметрия

Круговой массив

Верстак PartDesign

Расположение в меню
Линейный массив
Part Design → Apply a pattern → Линейный массив
Верстаки
PartDesign
Быстрые клавиши
Нет
Представлено в версии
-
См. также
Множественное преобразование

Описание

The PartDesign LinearPattern tool creates a linear pattern of selected features or the active body ^{introduced in 1.0}.

An L-shaped pad (B) made on top of a base pad (A, also referred to as support) is used for a linear pattern. The result (C) is shown on the right.

introduced in 26.3: This tool allows to disable individual pattern elements and to edit each offset individually.

Existing rectangular base feature with LP-shaped additive feature → "Linear Pattern" preview mode with deactivated elements (red x symbols deactivate elements, green + symbols reactivate elements) and individually offset top row and right column (grey dimensions: general offsets, red dimensions: individual offsets) → Resulting solid (LinearPattern feature)

Применение

Create

Optionally activate the correct Body.
Optionally select one or more features in the Tree View or the 3D View.
There are several ways to invoke the tool:
- Press the Linear Pattern button.
- Select the Part Design → Transformation Features → Linear Pattern option from the menu.
If there is no active Body, and there are two or more Bodies in the document, the Active Body Required dialog will open and prompt you to activate one. If there is a single Body it will be activated automatically.
The Linear Pattern Parameters task panel opens. See Options for more information.
Press the OK button to finish.

Edit

Do one of the following:
- Double-click the LinearPattern object in the Tree View.
- Right-click the LinearPattern object in the Tree View and select Edit Linear Pattern from the context menu.
The Linear Pattern Parameters task panel opens. See Options for more information.
Press the OK button to finish.

Опции

Choose the mode:
- Transform body: Transforms the whole base feature's shape (default). introduced in 1.0
- Transform tool shapes: Transforms the individual tool shapes of selected features.
  - To add features:
    1. Press the Add Feature button.
    2. Select a feature in the Tree View or the 3D View.
    3. Repeat to add more features.
  - To remove features:
    1. Press the Remove Feature button.
    2. Do one of the following:
      - Select a feature in the Tree View or the 3D View.
      - Select a feature in the list and press the Del key.
      - Right-click a feature in the list and select Remove from the context menu.
    3. Repeat to remove more features.
  - If there are several features in the pattern, their order can be important. See PartDesign PolarPattern.
Direction:
- Press the button to reverse the direction of the pattern.
- Specify the direction reference:
  - Normal sketch axis: The Z-axis of the sketch (only available for sketch-based features).
  - Vertical sketch axis: The Y-axis of the sketch (idem).
  - Horizontal sketch axis: The X-axis of the sketch (idem).
  - Construction line #: A separate entry for each construction line in the sketch (idem).
  - Base X-axis: The X-axis of the Body.
  - Base Y-axis: The Y-axis of the Body.
  - Base Z-axis: The Z-axis of the Body.
  - Select reference…: Select a Datum Line in the Tree View or a Datum Line or edge in the 3D View.
- introduced in 1.0: Specify the length Mode:
  - Extent: Enter the Length from a given point on the first occurrence to the same point on the last occurrence.
  - introduced in 1.0: Spacing: Enter the Spacing from a given point on the first occurrence to the same point on the next occurrence. For n occurrences: Extent=(n-1)*Spacing.
- Specify the number of Occurrences (including the original feature).
- introduced in 26.3: The length or spacing and occurrence values can also be edited with On-View Parameters in the 3D View.
Direction 2: Idem. introduced in 1.1
If the Recompute on change checkbox is checked the view will update in real time.

Properties

Data

Base

ДанныеOriginals (LinkList): A list of selected features. Will be ignored, if the ДанныеTransform Mode property is set to Whole shape.
ДанныеTransform Mode (Enumeration):
Features (default)

Whole shape.

Direction 1

ДанныеDirection (LinkSub): The first direction of the pattern. This can be a straight edge, a datum line, a sketch axis, or the normal of a planar face.
ДанныеReversed (Bool): Default is False. Reverse the first direction of the pattern.
ДанныеMode (Enumeration): Selects how the pattern is dimensioned.
Extent: Uses the total length from the first to the last instance.

Spacing (default): Uses the distance between consecutive instances.
Данные (ReadOnly)Length (Length): Default is 100.0 mm. The total length of the pattern, measured from the first to the last instance.
This is only used when the ДанныеMode property is set to Extent.
ДанныеOffset (Length): Default is 100.0 mm. The distance between each instance of the pattern.
This is only used when the ДанныеMode property is set to Spacing.
ДанныеSpacings (FloatList): Default is [-1.0, -1.0]. A list of custom spacings between instances. If a value is -1, the global ДанныеOffset value is used for that spacing. The list should have one less item than the number of occurrences.
ДанныеSpacing Pattern (FloatList): Default is [20.0]. Defines a repeating pattern of spacings for the second direction. For example, a list of [10, 20] will create alternating spacings of 10mm and 20mm. (Experimental and subject to change. To enable this in the UI you can add a boolean parameter 'ExperiementalFeature' in Preferences/Mod/Part).
ДанныеOccurrences (IntegerConstraint): Default is 2. The total number of instances in the first direction, including the original feature.

Direction 2

ДанныеDirection2 (LinkSub): The second direction of the pattern. This can be a straight edge, a datum line, a sketch axis, or the normal of a planar face.
ДанныеReversed2 (Bool): Default is False. Reverse the second direction of the pattern.
ДанныеMode2 (Enumeration): Default is Extent. Selects how the pattern is dimensionedin the second direction.
Extent: Uses the total length from the first to the last instance.

Spacing (default): Uses the distance between consecutive instances.
Данные (ReadOnly)Length2 (Length): Default is 100.0 mm. The total length of the pattern in the second direction, measured from the first to the last instance.
This is only used when the ДанныеMode2 property is set to Extent.
ДанныеOffset2 (Length): Default is 100.0 mm. The distance between each instance of the pattern in the second direction.
This is only used when the ДанныеMode2 property is set to Spacing.
ДанныеSpacings2 (FloatList): Default is []. A list of custom spacings for the second direction. If a value is -1, the global 'Offset' is used. The list should have one less item than the number of occurrences.
ДанныеSpacing Pattern2 (FloatList): Default is [0.0]. Defines a repeating pattern of spacings for the second direction. For example, a list of [10, 20] will create alternating spacings of 10mm and 20mm. (Experimental and subject to change. To enable this in the UI you can add a boolean parameter 'ExperiementalFeature' in Preferences/Mod/Part)
ДанныеOccurrences2 (IntegerConstraint): Default is 1. The total number of instances in the second direction, including the original feature.

Part Design

ДанныеRefine (Bool): Default is True. Refine shape (clean up redundant edges) after operations.
ДанныеFuzzy Tolerance (FloatConstraint): Default is -1.0. Fuzzy tolerance:
If value > 0: use the value

If value = 0: leave default value

If value < 0: determine value

Pattern

Данные (Hidden)Suppressed Positions (IntPairList): Suppressed instances as zero-based (direction 1, direction 2) indices. Positions outside the current pattern are retained. introduced in 26.3

Transformation