Sheet metal annotations in drawings

 

You can create sheet metal annotations in flat pattern views of sheet metal parts.

The following types of annotations are available in the drawing:

  • Bend notes
  • Bend tables
  • Punch notes
  • Punch tables

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 tabTable 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:

  • Each individual bend centerline is treated as an individual bend object in the drawing (with respect to both bend notes and bend tables). In the sheet metal model, the number of bend centerlines is not equal to individual bend features. (The contour flange, contour roll, lofted flange, and hem features produce multiple bend centerlines in one operation).
  • Contour Roll and Cosmetic centerline features are automatically collected into any generated bend table.
  • Contour roll centerlines do not report KFactor or direction information (in bend tables or notes).
  • Bend centerlines, Contour roll centerlines, and general drawing centerlines added to a drawing view are all unique object types and are mapped to separate layers. You can optionally wish to edit the default attributes for these objects (using the Style and Standard Editor) to allow for visual differentiation within your drawings. Refer to Styles in drawings for additional details.
  • Depending on the attributes applied during creation, Cosmetic centerlines can produce empty fields or custom formatting of text strings in bend tables or notes.
  • If it is necessary to change the Bend ID sequence: open the sheet metal part, edit the flat pattern and make the required changes using the Bend Order functionality.
  • If the Bend Order sequence has been modified, the resulting sequence of Bend IDs within any bend table can require sorting using the Table Edit functionality.
  • 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.
  • To correct the bend direction in legacy drawings, drag the bend note or table to a new position.
  • Bend tables are not associated with a drawing view. The bend table is not deleted if you delete the drawing view selected on creating the bend table.
  • If the selected sheet metal file does not contain a flat pattern or contains a flat pattern created in Inventor 2010 or earlier using the DataM unfolder, the file is not recognized as a valid table data source.
  • Bend Tables for sheet metal materials provide values for the bend allowance at specific bend radii and bend angles for a given material thickness, and have no relation to Bend Tables in drawings.

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 tabFeature 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:

  • Punch Direction in punch notes and tables is determined by the drawing view. If Punch Direction is DOWN for a punch in a punch note or table related to a front view, it is UP for the same punch in a back view.
  • To correct the punch direction in a legacy punch table, drag the punch table to a new position.
  • The appearance of punch features in the drawing view corresponds with the representation selected in the model. That means, if punch features are fully formed in the model, visible and hidden model edges are displayed in the drawing view. You can choose to include punch center marks in the Drawing View dialog box, but you cannot display the 2D representation of punch features in the drawing view.
  • Punch centers cannot be individually unloaded from the drawing view. The only way to remove a recovered punch center is to edit the view and cancel the selection of the Recover Punch Centers option. Any annotations attached to punch center marks are deleted.
  • Set the visibility of punch centers by using the Visibility option in the right-click menu. To display hidden punch center select Show Hidden Annotations in the right-click menu of the drawing view.
  • Center marks associated with punch centers cannot be moved or rotated, but the center mark extensions can be independently resized by dragging.
  • When flat pattern drawing views display punch centers, center marks are added, moved, and deleted to reflect any change in the source sheet metal file.
  • Unconsumed punch centers in the punch feature sketch are not displayed as recovered punch centers.
  • The default formatting for recovered punch centers is specified by the active style. To edit the punch centers style, open the Object Defaults Style panel and change the setting for Visible Simplified Representation and Hidden Simplified Representation.

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.

NoteIf dual unit format is selected, precision and tolerance values are also displayed in the dual format.

Procedures

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

  1. On the ribbon, click Annotate tabTable panel General.
  2. On the drawing sheet, select a view of a sheet metal part.
    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.
  3. Click OK to place the table on the drawing sheet. The table is placed with a default title of: TABLE. Columns for: BEND ID, BEND DIRECTION, BEND ANGLE, and BEND RADIUS are included by default.

Optionally, following step 2, you can:

  • Select the Column Chooser in the Rows and Columns area of the Table dialog box. Add or remove columns from the bend table you are about to produce.
  • Select the Alpha Bend ID Format radio control in the Bend ID area of the Rows and Columns area of the Table dialog box. Report the Bend ID using an alphabetic sequence identifier. By default, the bend table is produced using a numeric bend sequence identifier.
  • Enter a character string in the Prefix field in the Bend ID area of the Rows and Columns area of the Table dialog box. Include the entered string in front of the alpha or numeric Bend ID in the resulting table.
NoteAlpha 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.
TipTo 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:

  1. Right-click the bend table.
  2. Select Add Tags to View from the menu.
  3. Select the drawing view to place bend tags.
NoteBend tags are formatted by the Dimension style, and do not have a leader by default.
TipDrag the bend tag text away from the original position to add a leader to the bend tag.

Edit bend tables

  1. Right-click a bend table, and select Edit from the menu.
  2. Make the desired edits in the Edit Table dialog box:
    • Click Renumber to renumber items in the table consecutively according to the current order. The initial numbering rules for the bend table are respected.
    • Right-click the Bend Direction column and select Reverse Direction to revert the direction for bends in the table.
    • For more procedures, see the Edit a table page in Help.
  3. Click Apply to save changes, and OK to close the Edit Table dialog box.
TipTo 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.

 
  1. On the ribbon, click Annotate tabFeature Notes panel Bend.
  2. Select a bend centerline (or do a window selection for multiple bend centerlines).
  3. Bend note is generated and placed about the selected bend centerline.
  4. Right-click and select Done to finish the command.
NoteThe 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

  1. Right-click a bend note, and select Edit Bend Note from the menu.
  2. In the Edit Bend Note dialog box, edit the bend note text in the edit field:
    • Click Bend Direction, Bend Angle, Bend Radius, or kFactor in the Values and Symbols section to insert the corresponding property in the edit field.
    • Click the arrow next to the Insert Symbol command to select and insert a symbol.
    • If appropriate, add a stacked text in the note. Type a correct stacking sequence, select it, right-click and choose Stack. If AutoStacking is enabled, fractional numbers with a valid stacking trigger followed by a neutral character are stacked automatically as you type.
  3. To change the precision of the Bend Angle, Bend Radius, and kFactor value, click Precision and Tolerance. Then change Precision and Tolerances in the Precision and Tolerance dialog box:
    • To set precision, select Use Global Precision to use precision setting defined on the Units tab of the active Dimension style. Or, cancel the selection of Use Global Precision, and select the Precision for Bend Angle, Bend Radius, and kFactor.
    • To set tolerances for Bend Angle and Bend Radius, click the More option, select the check box in the Tolerances section. Then select Method, enter the tolerance values, and select the precision.
  4. Select Part Units to use the measurement units of the model. Clear the check mark to use the measurement units specified by the Dimension style.
  5. Click OK to close the Edit Bend Note dialog box.

Tips (Drag Editing):

  • To change position of the note along the bend centerline, click the note text and drag it along the bend centerline to the appropriate position.
  • To create a leader, click the note text and drag it to an appropriate position away from the bend centerline.
    NoteThe 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.
  • To create a linear extension leader, click the note text and drag it behind the endpoint of the associative bend centerline.
  • To flip the bend note, click the note text and drag it in a perpendicular direction towards the bend centerline.

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.

  1. On the ribbon, click Manage tabStyles and Standards panel Styles Editor.
  2. In the Style and Standard Editor dialog box, expand the Dimension item, and click a dimension style.
  3. On the Notes and Leaders tab, select Bend Note Settings.
  4. If needed, edit the default bend note text in the edit field: Click Bend Direction, Bend Angle, Bend Radius, or kFactor in the Values and Symbols section to insert the corresponding property in the edit field. Click the arrow next to the Insert Symbol command to select and insert a symbol.
  5. To change the precision of the Bend Angle, Bend Radius, and kFactor value, click Precision and Tolerance. Then change Precision and Tolerances in the Precision and Tolerance dialog box:
    • To set precision, select Use Global Precision to use precision setting defined on the Units tab of the active Dimension style, or unselect Use Global Precision, and select the desired Precision for Bend Angle, Bend Radius, and kFactor.
    • To set tolerances for Bend Angle and Bend Radius, click the More option, select the check box in the Tolerances section. Then select Method, enter the tolerance values, and select the precision.
  6. If needed, open the Display tab, and change the Origin Offset value.
  7. Click Save and Done to save the changes and close the Style 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.

  1. Recover punch centers in the base view: click Place Views tabCreate 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.
  2. Create center marks for punch features to include in the punch table. To add center marks automatically, right-click the view, and select Automated Centerlines. To add center marks manually, click Annotate tabSymbols panel Center Mark and select particular punch features.
  3. To create a punch table for a drawing view, click Annotate tabTable panel Hole View. Select the drawing view, click a point to place the origin indicator, and then click to place the punch table.
    NoteRecovered 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.
  4. If the punch features are not included in the hole table by default, right-click the hole table and select Edit Hole Table. On the Options tab of the Edit Hole Table dialog box, select the Recovered Punch Centers option in the Included Features section.
  5. To add the appropriate columns to the punch table, right-click the hole table and select Edit Hole Table. On the Formatting tab of the Edit Hole Table dialog box, click Column Chooser, and add the punch-specific columns to the Selected Properties list.
TipTo include recovered punch centers in the hole table by default, choose Manage tabStyles 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.
NoteTo 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.

 
  1. On the ribbon, click Annotate tabFeature Notes panel Punch, to create a punch note.
  2. Select a punch geometry or a punch center mark.
  3. Move the cursor and click to place the punch note. Continue placing punch notes.
  4. When finished, right-click and select Done.

Edit a punch note

  1. Right-click a punch note, and select Edit Punch Note from the menu.
  2. In the Edit Punch Note dialog box, edit the punch note text in the edit field:
    • Click Punch ID, Punch Direction, Punch Angle, or Punch Depth in the Values and Symbols section to insert the corresponding property in the edit field.
    • Click Quantity Note to insert the Quantity Note property in the edit field.
    • Click the arrow next to the Insert Symbol command to select and insert a symbol.
    • If appropriate, add a stacked text in the note. Type a correct stacking sequence, select it, right-click and choose Stack. If AutoStacking is enabled, fractional numbers with a valid stacking trigger followed by a neutral character are stacked automatically as you type.
  3. To change the precision and tolerance of the Punch Angle and Punch Depth value, click Precision and Tolerance. Then change the setting in the Precision and Tolerance dialog box:
    • To set precision, select Use Global Precision to use precision setting defined on the Units tab of the active Dimension style. Or cancel the selection of Use Global Precision, and select the Precision for Punch Angle and Punch Depth.
    • To set tolerances for Punch Angle and Punch Depth, click the More option. Then select the check box in the Punch Angle and Punch Depth row, select Method, enter the values and select the precision.
  4. Select Part Units to use the measurement units of the model. Remove the check mark to use the measurement units specified by the Dimension style.
  5. Click OK to close the Edit Punch Note dialog box.
TipTo 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

  1. On the ribbon, click Manage tabStyles and Standards panel Styles Editor.
  2. In the Styles and Standard Editor dialog box, expand the Dimension item, and click a dimension style.
  3. On the Notes and Leaders tab, select Punch Note Settings.
  4. If appropriate, edit the default punch note text in the edit field: Click Punch ID, Punch Direction, Punch Angle, or Punch Depth in the Values and Symbols section to insert the corresponding property in the edit field. Click the arrow next to the Insert Symbol command to select and insert a symbol.
  5. To change the precision of the Punch Angle and Punch Depth value, click Precision and Tolerance. Then change Precision and Tolerances in the Precision and Tolerance dialog box:
    • To set precision, select Use Global Precision to use precision setting defined on the Units tab of the active Dimension style, or unselect Use Global Precision, and select the desired Precision for Punch Angle and Punch Depth.
    • To set tolerances for Punch Angle and Punch Depth, click the More option. Then select the check box in the Punch Angle and Punch Depth row, select Method, enter the values and select the precision.
  6. Click Save and Done to save the changes and close the Style Editor.

References

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..

NoteTo 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 Sheet metal annotations in drawings dialog box so you can add tolerance information to values included in notes.

 

Opens the Sheet metal annotations in drawings 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 tabStyles and Standards panel Styles Editor, click a style in Dimensions, and open the Notes and Leaders tab. Then select the Punch Note Settings option, and click Precision and Tolerance.

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.

(More)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 tabStyles and Standards panel Styles Editor, click a style in Dimensions, and open the Notes and Leaders tab. Then select the Punch Note Settings option, and click Edit Quantity Note.

NoteTo 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.

NoteTo 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 Table panelGeneral, and then click to select the Default or another defined table style.

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.

NoteData 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.

Column Chooser adds or removes columns in the hole table. Click the command, and change the list of columns in the Hole Table Column Chooser dialog box:

  • Click Add and Remove to move properties from one column to another.
  • Click Move Down or Move Up to change the order of the properties.
  • Click New Property to open the Define New Property dialog box.
  • Click Delete to remove a column from the table.

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.

  • Thru
  • Blind

Threaded holes

  • Thru: Full Thread, Depth Thread
  • Blind: Full Thread, Depth Thread

Counterbored holes and Countersunk holes. If a counterbored or countersunk hole is tapped, the tapped designation is disregarded for grouping.

  • Thru
  • Blind

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.

  • Hole features allows view-based hole tables to include hole features.
  • Circular cuts allows view-based hole tables to include extruded cuts. Clear the check box to exclude extruded circular cuts from view-based hole tables. Circular cuts are recognized only as drilled thru or drilled blind holes, and cannot include mid-plane extrusions.
  • Center marks allows view-based hole tables to include entries with center marks. Clear the check box to exclude center marks from view-based hole tables. Center marks with visibility turned off are not included in hole tables.
  • Recovered Punch Centers allows view-based hole tables to include punch features. Clear the check box to exclude punch features from view-based hole tables. Punch center marks with visibility turned off are not included in hole tables.
 

 

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.

  • Drill Holes includes drilled hole features in view-based hole tables.
  • Counterbore/Spotface Holes includes counterbored hole features in view-based hole tables. May be selected when creating selection-based or feature-based hole tables. Clear the check box to exclude from new view-based hole tables, and make edges or counterbored holes unavailable after you add a hole or create a selection-based or feature-based hole table.
  • Threaded Holes includes threaded holes in view-based hole tables. Allows selection of threaded holes for adding holes or creating selection-based and feature-based hole tables. Clear the check box to exclude threaded hole features when adding holes or creating a selection-based or feature-based hole table, and when creating new view-based hole tables. Makes edges of threaded hole features unavailable after you add holes or create selection-based or feature-based hole tables.
  • Countersink Holes includes countersunk holes in view-based hole tables. Allows selection of countersunk holes for adding holes or creating selection-based and feature-based hole tables. Clear the check box to exclude countersunk hole features when adding holes or creating a selection-based or feature-based hole table, and when creating new view-based hole tables. Makes edges of countersunk hole features unselectable after you add holes or create selection-based or feature-based hole tables.