| You can create sheet metal annotations in flat pattern views of sheet metal parts. The following types of annotations are available in the drawing:
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Bend Notes, Bend Tables, and Bend Tags
A bend note adds fabricating information to sheet metal bend, contour roll, and cosmetic centerlines. To add a bend note, click the Bend command and select a bend, roll or cosmetic centerline in the drawing view. Bend notes are associated with a drawing view.
Click Annotate
tab
Table
panel
General to
create a bend table. Select a sheet metal part as the source file,
or a drawing view of the sheet metal part (and the corresponding
source file is selected automatically). If the selected source file
includes several sources for table data, select the appropriate
source from a list.
Bend tags associate rows in a bend table with the view geometry. Bend tags are formatted by the Dimension style, and do not have a leader by default. Drag the bend tag text away from the original position to add a leader to the bend tag.
If you select a drawing view to specify the source of table data, bend tags are added to the selected drawing view automatically after the bend table is inserted in the drawing. To add bend tags in a drawing view manually, right-click the bend table and select Add Tags to View. Then select the drawing view.
Notes:
Punch Notes, Punch Center Recovery, and Punch Tables
The appearance of punch features in the drawing view corresponds with the representation selected in the model. If punch features are fully formed in the model, visible and hidden model edges are displayed in the drawing view.
Click Annotate
tab
Feature
Notes panel
Punch to
create a punch note. Then select a punch feature in the drawing
and place the note.
A punch note includes data related to the punch, for example the punch ID, angle, direction, depth, quantity note, and so on. The default style of punch notes is set on the Notes and Leaders tab of the Dimension Style panel.
Before you create a punch table, recover punch centers. Punch centers are represented by center marks in a drawing view.
If you create a view-based hole table and select to include recovered punch centers, all visible punch center marks are included in the hole table as individual rows. The corresponding tags are created in the drawing view.
On the Annotate tab, Feature Notes panel, use Hole Table to create a punch table. If needed, change Default Filters in Hole Table Style to include recovered punch centers in the hole table by default.
Notes:
Dual dimensions in bend and punch annotations
Bend and punch notes can display dimension values in alternate units. Set the dual units display on the Alternate Units tab of the Dimension Style.
To display dual dimension values in a bend or punch table, add the alternate unit columns to the table by using the Column Chooser dialog box.
Note: If dual unit format is selected, precision and tolerance values are also displayed in the dual format.
Create or edit a bend table
| A bend table lists the information related to bends in flat pattern views of sheet metal parts. |
Create a bend table
Table
panel
General .Note: If you select a drawing view while creating a bend table, the bend direction in the table corresponds with the direction of bends in the view. If you select a sheet metal part file as the source for a bend table, the default bend direction is displayed in the bend table. To revert the bend direction, edit the bend table, right-click the Bend Direction column, and select Reverse Direction.
Optionally, following step 2, you can:
Note: Alpha character Bend ID relies on the specific character set of the language used during installation. As an example, the bend order number '27' would be displayed as 'AA' if the Alpha option was selected and the language of installation was English.
Tip: To exclude particular characters from the alphanumeric auto-indexing sequence, change the Character Exclude options on the General tab of the Standard Style panel.
Create bend tags
Bend tags associate rows in a bend table with the view geometry.
If you select a drawing view while creating a bend table, bend tags are added to the selected drawing view automatically after the bend table is inserted in the drawing.
To add bend tags in a drawing view manually:
Note: Bend tags are formatted by the Dimension style, and do not have a leader by default.
Tip: Drag the bend tag text away from the original position to add a leader to the bend tag.
Edit bend tables
Tip: To display dual dimension values in the bend table, add the alternate unit column to the table by using the Column Chooser dialog box.
Create or edit a bend note
A bend note adds fabricating information to sheet metal bend centerlines. Bend notes are associated with a drawing view. Each individual bend centerline is treated as an individual bend object in the drawing (with respect to both bend notes and bend tables).
Create a bend note
To begin, create a Flat Pattern drawing view for a sheet metal part.
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Note: The default placement of the bend note is above the selected bend centerline. The bend text is constrained to the midpoint of the centerline and offset by the Origin Offset value from the Dimension Style.
Edit a bend note
Tips (Drag Editing):
Note: The appearance of the bend note with a leader is determined by Leader Text Orientation and Leader Text Alignment settings defined in the current Dimension style.
Display or hide alternate unit dimensions
Bend notes can display dimension values both in primary and in alternate measurement units. Edit the Dimension Style to change the settings.
Change the bend note style
The Dimension style controls the default style of bend notes.
Styles
and Standards panel
Styles Editor .
Create or edit a punch table
| Use the Hole Table command to create a punch table. If appropriate, change Default Filters in Hole Table Style to include recovered punch centers in the hole table by default. Before you create a punch table, recover punch centers. Punch centers are represented by center marks in a drawing view. If you create a view-based hole table and select to include recovered punch centers, all visible punch center marks are included in the hole table as individual rows. The corresponding tags are created in the drawing view. |
Create
panel
Base .
In the Drawing View dialog box, select a sheet metal component as
File. Select Flat Pattern view and Recover Punch Center in the Sheet
Metal View section.
Symbols
panel
Center
Mark and select particular
punch features.
Table
panel
Hole
View . Select the drawing
view, click a point to place the origin indicator, and then click
to place the punch table.Note: Recovered punch centers can be selected individually by using the Hole Table - Selection command. Or, select feature set (all punch center instances from a single feature) by using the Hole Table - Selected Feature command.
Tip: To
include recovered punch centers in the hole table by default, choose Manage tab
Styles
and Standards panel
Styles Editor .
In the Styles and Standards Editor dialog box, expand Hole Table
and click a hole table style. Open the Options tab of the Hole Table
Style window, and select the Recovered Punch Centers option in the
Included Features section.
Note: To edit punch tables, use the same method as for editing hole tables.
Create or edit a punch note
| Use Punch to create punch notes. A punch note includes data related to the punch, for example the punch ID, angle, direction, depth, quantity note, and so on. The default style of punch notes is set on the Notes and Leaders tab of the Dimension Style panel. |
Create a punch note
To begin, create a Flat Pattern drawing view for a sheet metal part.
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Edit a punch note
Tip: To add text to a punch note, right-click the punch note in the drawing and choose Text from the menu. Then enter the text in the Format Text dialog box.
Display or hide alternate unit dimensions
Punch notes can display dimension values both in primary and in alternate measurement units. Edit the Dimension Style to change the settings.
Change the punch note style
Styles
and Standards panel
Styles Editor .
Edit Punch Note
Use the Edit Punch Note dialog box to edit the punch note text, to change precision, tolerance, and units of the displayed punch parameters, or to edit quantity note.
Access: | Right-click a punch note, and select Edit Punch Note from the menu. |
Edit Field | Edits the punch note text. Edit the text manually, or in Values and Symbols, click a value or symbol to add a punch parameter or symbol.. Note: To stack text, type a correct stacking sequence, select it, right-click and choose Stack. |
| Inserts the Punch ID parameter in the text field. |
| Inserts the Punch Direction parameter in the text field. |
| Inserts the Punch Angle parameter in the text field. |
| Inserts the Punch Depth parameter in the text field. |
| Inserts the Quantity Note property in the text field. |
| Selects a symbol from the list to add it to the punch note. |
| Opens the Precision and Tolerance dialog box so you can add tolerance information to values included in notes. |
| Opens the Quantity Note dialog box so you can change the display of the quantity note property. |
Part Units | Check the box to use model units. Remove the check mark to use the measurement units specified by Dimension Style. |
Precision and Tolerance
Sets the precision and tolerance attributes for punch notes.
Access: | Right-click a punch note, and select Edit Punch Note from the menu. In the Edit Punch Note dialog box, click Precision and Tolerance. Click Manage
tab |
Use Global Precision | Sets parameter precision to the precision defined by the Precision setting on the Units tab of the active dimension style. When selected, individual Precision parameters are not available. Clear the check box to set individual precision for punch angle and punch depth. Effects settings in the Tolerances column. |
Unit Precision | Primary sets individual precision for punch angle and punch depth. Click the arrow to select a precision setting from the list. Not available if Use Global Precision is selected. Alternate sets precision for punch depth value in alternate units. Click the arrow to select a precision setting from the list. Not available if Use Global Precision is selected. If Linear Format on the Units tab of the Dimension style is set to Fractional, precision settings are shown as fractions. Decimal precision corresponds to fractional value, such as 1/8 is shown as .125. Format is also represented on Tolerances. |
| Displays Tolerances options. | |
Tolerances | Sets the tolerance values for the selected punch parameter. Check the box next to a symbol representing the parameter to set tolerance values. Upper Sets the value for the upper tolerance. Enter the upper tolerance value. Lower Sets the value for the lower tolerance. Enter the lower tolerance value with a negative sign of operation. Not available if the selected method does not support a tolerance range. Method Sets the tolerance method. Click the arrow, and then select from the list. Precision, Precision (Alt) Sets the number of decimal places to display in the punch note. Values are truncated and rounded to the specified precision. Click the arrow, and then select from the list. |
Quantity Note
Use the Quantity Note dialog box to change the display of the quantity note property in punch notes. Quantity Note is not displayed if the Punch Note is used in the context of a Punch Table or if the quantity is less than 2.
Access: | Right-click a punch note, and select Edit Punch Note from the menu or double-click a punch note. In the Edit Punch Note dialog box, click Edit Quantity Note. Click Manage
tab |
Note: To change the default setting of the quantity note, access the Quantity Note dialog box from the Style and Standard Editor. To edit the quantity note for a particular punch note in the drawing, open the Quantity Note dialog box from the Edit Punch Note dialog box.
Edit Field | Edits the quantity note text. Edit the text manually, or in Values and Symbols, click a value or symbol to add the QTY property or a symbol in the Edit field. |
| Adds the quantity (QTY) property to the quantity note. |
| Selects a symbol from the list to add to the punch note. |
Number of like punches in pattern or feature | If selected, the QTY property displays the sum of like punches in the pattern or feature. |
Number of like punches in model | If selected, the QTY property displays the sum of like punches in the model. |
Edit Bend Note
Icon pending
Use the Edit Bend Note dialog box to edit the bend note text, or to change precision, tolerance and units of the displayed bend parameters.
Access: | Right-click a bend note, and select Edit Bend Note from the menu. |
Text field | Edits the bend note text. Edit the text manually, or in Values and Symbols, click a value or symbol to add a bend parameter or symbol. Note: To stack text, type a correct stacking sequence, select it, right-click and choose Stack. |
| Inserts the Bend Direction parameter in the text field. |
| Inserts the Bend Angle parameter in the text field. |
| Inserts the Bend Radius parameter in the text field. |
| Inserts the kFactor parameter in the text field. |
| Selects a symbol from the list to add to the bend note. |
Precision/Tolerance Settings | Opens the Precision and Tolerance dialog box so you can add tolerance information to values included in notes. |
Part Units | Check the box to use model units. Remove the check mark to use the measurement units specified by the Dimension style. |
Table
For a selected drawing view of an iPart, iAssembly or presentation of an iAssembly, creates a table that references a Table style for formatting. During creation or table placement, the referenced table style can be changed by selecting a different table style from the style list on the Annotate tab.
Access: | On
the ribbon, click Annotate
tab |
Source
Select View | Specifies the source document that the table references. If you select a view of an iPart or iAssembly or a presentation of an iPart or iAssembly, the data source is automatically selected. For an .xls or .csv file, click Browse to locate the file. If preferred, do not select a source to create an empty table. |
Browse for file | Click to select a file from the list or click Browse to navigate to the file location. Adds the file referenced by the drawing view to the file list. If the selected file is a Microsoft Excel spreadsheet (.xls), Start Cell and Column Header are active on the Open dialog box. Specify the cell from which to start copying data for the table. Note: Data is copied from the first worksheet only, starting at the specified cell. When the source is an .xls or .csv file, data import stops when a blank row or column is encountered. |
Specify table data source | Specifies the source that the table references. If the selected file includes several sources for table data, select the appropriate source from the list. |
Columns and Rows
Columns and Rows | Available when creating a general table. Default is four columns and ten rows, except if the active Table style has the number of columns defined in the Default Column Settings. In that case, the default number of columns is as specified in the style. The number of columns and rows can be edited as desired. |
Column Chooser | Available when the selected file is an iPart or iAssembly. In the Table Column Chooser, selects columns to include in the table. Includes columns designated when the table was defined. For more information, see Table Column Chooser. |
Selected Columns | Shows columns to include in the table when placed. Columns set as keys in the iPart or iAssembly are displayed by default. Click OK and click to place the table on the drawing sheet. Like parts lists, the upper left corner of the table is constrained to selected view geometry or the border or title block. |
Edit Hole Table
Modifies formatting and options of a hole table. Overrides settings specified by the hole table style for the current document.
Access: | Right-click a hole table and select Edit Hole Table. |
Formatting
Changes attributes for hole table formatting. | |
Title | Sets the text to appear in the hole table title cell. |
Text Style | Specifies which text style formats the title, column header, and data text. Click the arrow to select a text style from the list. |
Heading | Selects heading position in the hole table. Click arrow to select Top, Bottom, or No Heading. Unlike the parts list dialog box, No Heading does not remove column headers from the table. |
Line Format | Click Outside or Inside to specify the lines to format with Line Weight and Color. Line Weight. Click the arrow to select a different line weight. Values originate with preset values for line weight on the Standard style. Color opens the Color dialog box which controls the color of inner and outer lines of the hole table. |
Column Settings | Changes the format of hole table columns.
Property shows the selected columns that appear in the hole table. Right-click to open the Column Chooser or Format Column dialog boxes. Column shows the selected column header names. Modify the appearance of the column header text by changing the text. Resize the column by clicking and dragging the column separator. Width sets the width of the hole table columns. Enter a specific width for each column or click and drag to resize after the hole table is created. |
Options
Changes values for row merging, hole tags, tag order, and view filters in the current hole table.
Row Merge Options modifies settings for merging hole table rows.
None | Preserves legacy hole table formatting. Reformat Table on Custom Hole Match reindexes the hole tags and resorts contents when a Match Custom Hole operation is done. Numbering replaces the alphanumeric hole tags with sequential numbering of the holes in the hole table. | |
Rollup | Combines the hole note cells for the holes of the same type in the hole table. Only the first hole in a series is still listed in the table. The rolled-up cell adopts the formatting of the first row (hole) in the series. Delete Tags on Rollup preserves legacy behavior. Except for the first in a series of hole tags, deletes tags from the associative view. Clear the check box to preserve tags. Secondary Tag Modifier on Rollup causes all hole tags in the table and view to include the secondary numerator. Clear the check box to drop the secondary modifier. For example, A1, A2 and B1 become A, A, and B. | |
Combine Notes | Combines hole note cells for the holes of the same type in the selected hole table. Reformat Table on Custom Hole Match reindexes the hole tags and resorts contents when a Match Custom Hole operation is done. Numbering replaces the alphanumeric hole tags with sequential numbering of the holes in the hole table. | |
Hole Tag Options changes settings for formatting hole tags. | ||
| Preserve Tagging causes permanent hole identifiers for each hole tagged when the table is first placed. Clear the check box to respecify holes when holes are added or deleted from the model). Tagging is preserved only with respect to changes to the model, such as when you add, delete, suppress or unsuppress hole features. Manual changes to the hole table, such as when you resort, change tag order, and filter hole types, are not affected. Use Leader generates a leader for any hole tag dragged away from the hole with which it is associated. Clear the check box to hide the leader of hole tags dragged away from an associated hole. | |
Tag Order sets tag order of holes in a hole chart. Existing hole tables are not affected by these settings. | ||
| Arrange by Position tags holes relative to their position on the selected view. Position is arranged with YDIM as the primary key and XDIM as secondary key. If YDIM and XDIM are equal, hole size is the tertiary sorting key, smallest to largest. Arrange by Size tags holes in order by size (smallest to largest). Size refers to the drill diameter (HDIA) parameter for drilled, counterbored, and countersunk holes. The tap drill diameter (TDDIA) is used for threaded holes. If holes are of equal size, holes are sorted by position. Group Hole Types must be unselected. Holes added from a center mark are added to the end of the list. Group Hole Types tags holes by hole type and then by choice of size or position. Existing hole tables are not affected by these settings. The group order is: | |
| Drilled holes includes extruded cut circles and circular voids.
Threaded holes
Counterbored holes and Countersunk holes. If a counterbored or countersunk hole is tapped, the tapped designation is disregarded for grouping.
Center marks | |
View Filters sets features and hole types to include in a view-based hole table. Existing hole tables are not affected by these settings. | ||
| Included Features selects features to include or exclude in view-based hole tables. Select a check box to include hole features, circular cuts, and center marks or clear the check box to exclude them.
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| Included Hole Types selects hole types to include or exclude in view-based hole tables. Select a check box to include drilled, counterbored, countersunk, or threaded holes. Clear a check box to exclude the hole type from views. Not available if hole features are excluded from view hole tables.
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