Symbols, sketched symbols, and blocks

You can use symbols, sketched symbols, and blocks to annotate drawings. Symbols are predefined annotations such as surface texture, features control frame, or datum identifier. Sketched symbols are user-defined annotations. Blocks are AutoCAD block objects.

Sketched symbols

 

You can create sketched symbols in a drawing or a drawing template. Symbols created in a drawing are available only in that document, but symbols created in a template are available to all drawings based on that template.

In the browser, click the Drawing Resources folder, and then click the Sketched Symbols folder to see a list of available symbols. After you place a symbol, each instance is listed in the Sketched Symbols browser folder for the current sheet. Define your own folders, under the Sketched Symbol folder, to organize your symbols.

Here are some guidelines to help you create and use sketched symbols:

  • Insertion Points snap to other drawing entities and can be used to move, rotate, and resize placed symbols.
  • Use the symbol connection points to connect other drawing entities to sketched symbols.
  • Create sketch geometry with commands on the Sketch tab, and then constrain and dimension it.
  • Include block definitions from a translated AutoCAD file. Nested blocks are exploded into a single sketched symbol. Translated entities are sketched lines and arcs.
  • Translate any 2D geometry in an AutoCAD file into a sketched symbol.
  • Bitmaps (.bmp files). Bitmaps are OLE objects that can be linked to the drawing or embedded.

    When you edit the .bmp file, a linked bitmap image in the sketched symbol is updated automatically. If you embed the bitmap, the copy in the drawing is not updated when you edit the .bmp file.

  • Sketched symbols can be associated with model properties. If a leader is deleted, the symbol loses its model association, but restoring the leader can recreate the association.

    Instead of deleting a leader, consider turning off its visibility. Invisible leaders retain symbol association with model properties.

  • You can insert prompted entries in sketched symbols. If two or more prompted entries are included in a sketched symbol, you can reorder prompted entries: Right-click the sketched symbol in Drawing Resources and select Reorder Prompted Entries from the menu. Then change the order of prompted entries in a dialog box.
NoteSketched symbols do not have layer properties, but the sketch geometry used to create them resides on a layer.

Blocks

You cannot create AutoCAD blocks in Inventor. If blocks exist in an AutoCAD dwg file then they will be available when the file is opened in Inventor. You can also import AutoCAD blocks using the Import Block command. Blocks can only be imported to .dwg files. The block definition is not editable in Inventor.

In the browser, click the Drawing Resources folder, and then click the AutoCAD Blocks folder to see a list of block definitions. After you place a block, each instance is listed in the AutoCAD Blocks browser folder for each sheet.

Here are some guidelines to help you use blocks:

  • Block instances can be placed, scaled, moved, and rotated within a drawing sheet.
  • Attributes values on block instances can be modified. Right-click on the block and select Edit Attributes.
  • Each block instance has a Static property. If the Static property is disabled, grip points are displayed when the block is selected. Use the grip points to rotate and scale the block. If Static is enabled, the grips are not displayed.
  • The properties (color, line type, and line weight) can be modified for a block depending on the setting in the block definition.

By Layer

The object inherits the properties of the layer the block is placed on.

By Block

The object inherits property overrides for the block, then properties of the layer.

Override

The object maintains the property and does not inherit properties from the layer or property overrides. For example, you set the object property to red in the block definition, the object will always be red.

 

Procedures

Create a sketched symbol

 

You can create sketched symbols in a drawing or a drawing template. Symbols created in a drawing are available only in that document, but symbols created in a template are available to all drawings based on that template.

In drawings and drawing templates, expand the Drawing Resources folder in the browser to show available symbols in the Sketched Symbols folder. A sketched symbol can contain geometry, text, iProperties, and imported bitmap images. New sketched symbols are added to the Sketched Symbols folder.

  1. Open a drawing file or drawing template.
  2. On the ribbon, click Manage tabDefine panel Symbol.

    If you prefer, right-click the Sketched Symbols folder in the browser and select Define New Symbol.

  3. Use the commands on the Sketch tab to create the symbol.
  4. To add an insert point to the sketch,
    • Click a point in the sketch to select it.
    • On the ribbon, click Sketch tabFormat panel Set Insertion Point Grip. A sketched symbol can have only one insert point.
  5. To add connection points to the sketch,
    • Click a point in the sketch to select it.
    • On the ribbon, click Sketch tabFormat panel Connection Point Grip.
    • Add as many connection points as needed.
  6. Right-click and select Save Sketched Symbol. Enter the new symbol name in the dialog box. The symbol is added to the Sketched Symbols folder in the browser.
NoteAfter you have created sketched symbols, click Annotate tab Symbols panel User to place sketched symbols. Available sketched symbols are listed in the Symbols dialog box.

Tips

  • To make sketched symbols available to all new drawings, add them to the template you use to create drawings.
  • To assign symbols to a specific layer, use the Style Editor to modify the Object Defaults style.
  • If needed, use the Drawing Resource Transfer Wizard to copy symbols from a drawing to another drawing or template file.
  • To place and move a sketched symbol precisely on a drawing, add one insert point and several connection points.
  • To update all symbols of one type, right-click a symbol and select Edit Definition. The changes are applied to all symbols of that type in the drawing.
  • To reorder prompted entries included in a sketched symbol, right-click the sketched symbol in the Drawing Resources folder and select Reorder Prompted Entries from the menu. Available only if 2 or more prompted entries exist in the sketched symbol.

Manage symbols with folders

Define folders under your Sketched Symbols folder in the drawing browser. Use them to group your symbols as dictated by your design needs. You can choose to populate your drawing browser with folders before you create symbols. Then, as you create symbols, you move them into the appropriate folders. Alternatively, you can create all symbols, then define your folders and move the symbols into them. Use these techniques, or a combination thereof, to order your symbols in the drawing browser.

You have two methods available to create your symbol folders. You can create empty folders, or pre-select symbol nodes and add them to new folders. User-defined symbol folders are represented by distinctive icons ( Open Folder: : Closed Folder: ) and they exhibit the same open and close behavior as other Inventor browser folders.

Create new folder

Right-click the Sketched Symbols folder, or one of your user-defined folders, and select Create New Folder. The new folder is created as a child node of the folder on which you right-clicked.

Add to new folder

Select sketched symbol nodes, right-click and select Add to New Folder. To add multiple nodes simultaneously, you can select nodes in a contiguous or non-contiguous group then add them to the new folder.

NoteIn certain situations, all non-contiguous node selections are not added to the new folder. When this happens, a warning message is displayed. If you click Accept in the warning dialog, nodes that cannot be added to the new folder remain selected and in-place.

Edit folders: drag and drop behavior

You can drag and drop single or multiple browser nodes into your folders. Likewise, you can remove nodes from your folders. The drag and drop behavior is similar to that of the Windows Explorer.

NoteIn certain situations, all non-contiguous node selections are not dragged to the new folder. When this happens, a warning message is displayed. If you click Accept in the warning dialog, nodes that cannot be transferred to the folder remain selected and in-place.

Place symbols

You can open the Symbols dialog from your folder nodes and place symbols in your drawing. Right-click a folder or symbol node and select Symbols. You cannot drag symbols from your folders and drop them into the drawing window.

Delete folder

Right-click your symbol folder and select Delete Folder. The folder is deleted, but the folder items remain. You cannot simultaneously delete multiple folders.

Tip

  • Copy and paste does not support user-defined symbol folders. As a result, if you copy and paste the Sketched Symbols folder or a drawing sheet, the sketch symbols within your folders are pasted, but your folders are not. Consider the creation of drawing templates in which these common folders and symbols are already defined.

Add a sketched symbol to a drawing

 

You can add sketched symbols as annotations to the active drawing file. In the browser, available symbols are listed under Sketched Symbols in the Drawing Resources folder.

After you place symbols in a drawing, the browser lists each instance in the Sketched Symbols folder for the sheet.

You can create sketched symbols. New symbols are available only in the current drawing, but symbols created in a template are available to all drawings that use that template.

Tip(Placing symbols in the drawing) Symbol leader lines snap in 15-degree steps. Hold the CTRL key on your keyboard to disable leader line snapping. Then place or move the leader line to the desired position.

Add a sketched symbol to the active sheet

 
  1. On the ribbon, click Annotate tab Symbols panel User.
  2. In the Symbols dialog box, select the symbol to place.
  3. Set the scale and rotation angle for the selected symbol.
  4. Select the Symbol Clipping check box to trim dimension lines, leader lines, and extension lines behind symbols. Clear the check box to show leader or extension lines across the symbol.
  5. Select the Static check box to turn off scale and rotation grip points on the symbol. Clear the check box to allow manual resizing and rotation of the symbol.
  6. Specify if the symbol is placed with a leader. Clear the Visible check box to place the symbol with an invisible leader, which is shown as a dashed line during placement.
    TipSymbols with leaders can be associated with a component and display the component properties. If the leader is not created or is deleted, the symbol is associated to the source model for first created drawing view. Leaders with visibility turned off are not shown on the drawing view, but allow the symbol to retain its model association.
  7. Click OK to close the dialog box, and then click in the graphics window to place the symbol.

    To associate the symbol with a model, move the cursor over the model geometry until the green dot appears, and then click to place the symbol.

  8. Continue to place symbols, right-click and select Done.
NoteSelect and drag the symbol to move it to a new location after inserting it. If the symbol contains connection points , use the connection points to snap to other geometry in the drawing sheet.

Stack a symbol to another symbol

 
  1. On the ribbon, click Annotate tab Symbols panel User.
  2. In the Symbols dialog box, select the sketched symbol to place, set the symbol properties, and click OK to close the dialog box.
  3. Press the Shift key on your keyboard, move the cursor over the square bounding box of an existing sketched symbol until the green dot appears, and then click to place the symbol. The new symbol is stacked at the corresponding side of the selected symbol.
  4. Continue to place symbols, right-click and select Done.

Place a fixed sized symbol

  1. In the browser, right-click the Sketched Symbols in the Drawing Resources folder, and then click Insert.

    If you prefer, double-click the symbol in the Sketched Symbols folder.

  2. Click in the graphics window to place the symbol.
  3. Continue placing symbols. When you finish, right-click, and then select Done.

The symbol is placed using the default scale and rotation angle and leader setting. Right-click and select Edit Symbol to modify settings.

Move, rotate, or resize a symbol

  1. Select a sketched symbol in the graphics window to show its points.
  2. Click a point, and do one:
    • To move the symbol, click the green point, and then drag to the appropriate location.
    • To rotate the symbol, click the blue dot, and then drag to the appropriate orientation.
    • To resize the symbol, click one of the yellow dots, and then drag to the appropriate size.
TipIf an insert or connection point is coincident with a resize grip, the insert/connection point takes precedence. You must resize using an alternate grip or change the scale in the Edit Symbol dialog box.

Add a block to a drawing

 

You can add blocks as annotations to the active drawing file when working in a .dwg file. In the browser, block definitions are listed under AutoCAD Blocks in the Drawing Resources folder.

After you place blocks in a drawing, the browser lists each instance in the AutoCAD Blocks folder for the sheet.

You cannot create block definitions in Inventor. Blocks can be created in AutoCAD and imported into Inventor.

Place a block using the AutoCAD Blocks dialog box

  1. In the browser, expand the AutoCAD Blocks folder in the Drawing Resources folder.
  2. In the browser, right-click on any block and then click AutoCAD Blocks.
  3. In the AutoCAD Blocks dialog box, select the block to place.
  4. Set the scale and rotation angle for the selected block.
  5. Click OK to close the dialog box, and then click in the graphics window to place the block.
  6. Continue placing blocks. When you finish, right-click, and then select Done.
NoteSelect and drag the block to move it to a new location after inserting it.

Place a block using the Insert command

  1. In the browser, expand the AutoCAD Blocks folder in the Drawing Resources folder.
  2. In the browser, right-click the block, and then click Insert.
  3. Click in the graphics window to place the block.
  4. Continue placing blocks. When you finish, right-click, and then select Done.

The block is placed using the default scale and rotation angle. Right-click and select Edit AutoCAD Block to modify settings.

Move, rotate, or resize a block

  1. Select a block in the graphics window to show its points.
  2. Click a point, and do one:
    • To move the block, click the green point, and then drag to the appropriate location.
    • To rotate the block, click the blue dot, and then drag to the appropriate orientation.
    • To resize the block, click one of the yellow dots, and then drag to the appropriate size.
TipThe amount the block is rotated or scaled is maintained. The value is displayed in the AutoCAD Blocks dialog box.

Add a datum identifier symbol

 

Use Datum Identifier to create one or more datum identifier symbols. You can create a datum identifier with a leader line or as a stand-alone symbol. The color and line weight of the symbol are determined by the object layer.

 
  1. On the ribbon, click Annotate tabSymbols panel Datum Identifier.
  2. To place the symbol, do one of the following:
    • To create a symbol without a leader line, double-click a location for the symbol. The Format Text dialog box opens.
    • To create a symbol without a leader line associated with geometry, double-click a highlighted edge or point. The symbol is attached to the edge or point, and the Format Text dialog box opens. You can drag the symbol to change its location. If you drag the symbol along the edge, an extension line is created. If you drag the symbol away from the edge, a leader is created.
    • To create a symbol with a leader line, click a location for the start point of the leader line. If you click a highlighted edge or point, the leader line is attached to the edge or point.
  3. If you are creating a leader line, move the cursor and click to add a vertex to the leader line. You can only add one vertex.
  4. When the symbol indicator is in the desired position, click to place the symbol and open the Format Text dialog box.
  5. Enter the appropriate label for the symbol.

Continue placing datum identifier symbols. When you finish placing symbols, right-click, and then choose Done from the menu to end the operation.

Show Me how to place a datum identifier symbol

Add a datum target symbol

 

Use Datum Target to create one or more datum target symbols.

The color, target size, line attributes, and measurement units of the symbol are determined by the Datum Target style of the layer and object style of the symbol.

 
  1. On the ribbon, click Annotate tab Symbols panel Datum Target.
  2. Select the target type from the palette.
  3. In the graphic window, click to set the start point for the datum.
    • Leader datum start point sets the terminator for the leader line.
    • Line datum start point sets one end of the datum line.
    • Rectangle datum start point sets the center of the rectangle. Click again to define the area.
    • Circle datum start point sets the center of the circle area. Click again to define the area.
    • Point datum start point places the point indicator.
  4. Move the cursor, and then click to add a vertex to the leader line.
  5. When the symbol indicator is in the desired position, right-click, and then choose Continue to place the symbol and open the Datum Target dialog box.
  6. Enter the appropriate dimension value and datum for the symbol.

Continue placing datum target symbols. When you finish placing symbols, right-click, and then choose Done from the menu to end the operation.

Show Me how to place a datum target with a circle

Show Me how to place a datum target symbol with a line

Show Me how to place a datum target symbol with a point

Show Me how to place a datum target symbol with a rectangle

NoteTo stack datum targets, right-click an existing datum target, and then select Attach Balloon from the menu.

Add a feature control frame symbol

 

Use Feature Control Frame to create a feature control frame symbol. You can create a feature control frame with a leader line or as a stand-alone symbol.

The color, target size, line attributes, and measurement units of the symbol are determined by the feature control frame style.

 
  1. On the ribbon, click Annotate tab Symbols panel Feature Control Frame.
  2. To place the symbol, do one of the following:
    • To create a symbol without a leader line, double-click a location for the symbol. The Feature Control Frame dialog box opens.
    • To create a symbol without a leader line associated with geometry, double-click a highlighted edge or point. The symbol is attached to the edge or point, and the Feature Control Frame dialog box opens. You can drag the symbol to change its location. If you drag the symbol along the edge, an extension line is created. If you drag the symbol away from the edge, a leader is created.
    • To create a symbol with a leader line, click a location for the start point of the leader line. If you click a highlighted edge or point, the leader line is attached to the edge or point.
  3. If you are creating a leader line, move the cursor, and then click to add a vertex to the leader line.
  4. When the symbol indicator is in the appropriate position, right-click, and then select Continue to place the symbol and open the Feature Control Frame dialog box. The options in the dialog box are determined by the active drafting standard.
  5. Enter the information for the symbol and close the dialog box.
  6. If appropriate, you can rotate the feature control frame clockwise or counter clockwise. Right-click the feature control frame and choose an option.
  7. Continue placing feature control frames. When you finish placing symbols, right-click, and then choose Done from the menu to end the operation.

Show Me how to place a feature control frame

TipThe leader attachment, frame appearance, availability of symbols in Feature Control Frame dialog box, and other properties are controlled by Feature Control Frame Style. To change the settings, choose Manage tabStyles and Standards panel Styles Editor, select a feature control frame style, edit the style settings and then save the changes.

Add a feature identifier symbol

 

Use Feature Identifier to create a feature identifier symbol with a leader line.

 
  1. On the ribbon, click Annotate tabSymbols panel Feature Identifier.
  2. To place the symbol, do one of the following:
    • To create a symbol without a leader line, double-click a location for the symbol. The Format Text dialog box opens.
    • To create a symbol without a leader line associated with geometry, double-click a highlighted edge or point. The symbol is attached to the edge or point, and the Format Text dialog box opens. You can drag the symbol to change its location. If you drag the symbol along the edge, an extension line is created. If you drag the symbol away from the edge, a leader is created.
    • To create a symbol with a leader line, click a location for the start point of the leader line. If you click a highlighted edge or point, the leader line is attached to the edge or point.
  3. If you are creating a leader line, move the cursor, and then click to add a vertex. You can only add one vertex.
  4. When the symbol indicator is in the desired position, click to place the symbol, and then open the Format Text dialog box.
  5. Enter the appropriate label for the symbol, and then click the check mark to close the dialog box.

    Show Me how to place a feature identifier symbol

Continue placing feature identifier symbols. When you finish placing symbols, right-click, and then select Done from the menu to end the command.

Add a surface texture symbol

 

Use the Surface command to create a surface texture symbol. You can create a surface texture symbol with a leader line or as a stand-alone symbol. The color and line weight of the symbol are determined by the active surface texture style and layer associated with symbols. The diameter of the optional all-around symbol is specified in the leader style.

 
  1. On the ribbon, click Annotate tabSymbols panel Surface.
  2. To place the symbol, do one of the following:
    • To create a symbol without a leader line, double-click a location for the symbol. The Surface Texture dialog box opens.
    • To create a symbol without a leader line associated with geometry, double-click a highlighted edge or point. The symbol is attached to the edge or point, and the Surface Texture dialog box opens. You can drag the symbol to change its location. If you drag the symbol along the edge, an extension line is created. If you drag the symbol away from the edge, a leader is created.
    • To create a symbol with a leader line, click a location for the start point of the leader line. If you click a highlighted edge or point, the leader line is attached to the edge or point.
  3. If you are creating a leader line, move the cursor, and then click to add a vertex.
  4. When the symbol indicator is in the desired position, right-click, and select Continue to place the symbol and open the Surface Texture dialog box. The options in the dialog box are determined by the active drafting standard.
  5. Set the attributes and values for the symbol.

    Show Me how to place a surface texture symbol

Continue placing surface texture symbols. When you finish placing symbols, right-click, and then select Done from the menu to end the operation.

Edit symbols in drawings

Sketched symbols can include text, sketch geometry, bitmaps, and model properties.

Sketched symbols with leaders can be associated with model properties. Changes to the model properties are automatically updated with the symbol. If a leader is not created or is deleted, the symbol loses its association to model properties.

TipYou can turn off visibility of a leader when creating or editing the symbol. The hidden leader allows the symbol to retain its association with model properties, but is not shown on the drawing sheet.

Edit symbol values or elements

You can change any value or element that was assigned when a symbol was created.

  1. In the graphics window, right-click one or more symbols of the same type, and then select the appropriate edit option Select:
    • Edit Arrowhead to select a new arrowhead style. Click the arrow to select a new style and then click the green check mark.
    • Add Vertex/Leader to add a leader with one or more optional vertices.
    • Delete Leader. Use caution; a symbol whose leader has been deleted loses its association with model properties.
    • Edit Definition to modify the original symbol sketch. All instances of the symbol update with the changes.
    • Edit Symbol to change the selected symbol settings in the Symbol dialog box.
    • Properties to modify symbol properties. Change Line Type, Line Weight, Color, and Scale.
  2. Edit values or geometry as needed. The changes are displayed in the graphics window.

Move a symbol using a leader

You can move a symbol by lengthening or shortening any segment of a symbol leader line or by moving the symbol, the start point, or any vertex. You can move datum identifiers, callout symbols, and feature control frames by moving their leaders.

TipWatch for the move symbol to display next to the cursor. If necessary, zoom in to select the point you want.

Move a datum identifier or symbol

  1. In the graphics window, move the cursor over the symbol or leader line to display grip points.
  2. To move the datum identifier or symbol to a new location, drag the grip point closest to it.
  3. To move the datum identifier or symbol off an edge, drag the base grip point off the edge. Autodesk Inventor creates an extension line for the datum identifier.
  4. To change the edge the datum identifier or symbol references, drag the base grip point to the desired edge. You can also change the datum identifier so that it references a feature control frame by dragging the base grip point to a feature control frame.

Move a feature control frame

  1. To move a feature control frame, click the feature control frame, and then drag it to the desired location.
  2. If you drag the feature control frame parallel to the referenced edge, Autodesk Inventor creates an extension line.
  3. If you drag the feature control frame away from the referenced edge, Autodesk Inventor creates a leader.
  4. To make the feature control frame leader collinear with a dimension leader, drag the feature control frame leader arrowhead to the dimension leader arrowhead. To separate the leaders, drag the feature control frame away from the dimension.

Change the terminator

You can change the terminator for individual symbols.

  1. In the graphics window, right-click the symbol, and then select Edit Arrowhead from the menu to open the Change Arrowhead dialog box.
  2. Click the arrow and select the terminator from the list.
  3. Click the check mark to change the terminator.

Copy and paste symbols

You can copy existing symbols and paste them in your drawings as new symbols to quickly and easily create new symbols.

  1. In the graphics window, right-click the symbol and select Copy. To select multiple symbols, hold down the Ctrl key as you select symbols.
    TipTo clear the selection, click anywhere on the drawing sheet.
  2. Right-click a blank area in the drawing sheet, and select Paste. The copied symbol or symbols are attached to the cursor.
  3. Click to place the copied symbol or symbols. If you click a highlighted edge or point, the copied symbol is attached to the edge or point.
  4. Continue placing the copied symbol or symbols. When you finish placing symbols, right-click and choose Done.
NoteYou cannot copy and paste balloons and parts lists or copy leader text from one drawing to another.

Change a symbol style

On the Annotate tab, Format panel, click the arrow on the Style list and select a style when creating a symbol or to modify a selected symbol. Optionally, edit the default settings for the symbol in Style and Standard Editor.

Add a leader or vertex

You can add a branch to an existing leader to enable pointing to multiple locations.

  • To add a leader, right-click an existing leader and select Add Leader/Vertex. Click an attachment point on view or sketch geometry and then click the leader line where you want the new leader to attach.
  • To add a vertex, right-click select an existing leader and select Add Leader/Vertex. Click a point on the existing leader where you want to add the new vertex and then drag the new vertex point to create a bend in the leader line.

Edit blocks in drawings

You can edit the position, size, and attributes of block instances. You cannot edit the block definition in Inventor. Open the drawing in AutoCAD to modify the block definition.

Edit block attributes

You can change any attribute that was assigned when a block was inserted.

  1. In the graphics window, right-click the block , and then select Edit Attributes.
  2. Modify the attribute values in the Edit Attributes dialog box.
  3. Click OK.

Open the block in AutoCAD

You can open the current dwg file in AutoCAD in order to modify block definitions. AutoCAD must be installed on the computer.

  1. Right-click one or more blocks, and then select Open in AutoCAD.
  2. Click OK in the Inventor message dialog box. The current file is closed in Inventor and opened in AutoCAD.
  3. Make the necessary changes in AutoCAD then save and close the file.
  4. Open the file in Inventor.

Copy and paste blocks

You can copy existing blocks and paste them in your drawings as new blocks to quickly and easily create new blocks.

  1. In the graphics window, right-click the block and select Copy. To select multiple blocks, hold down the Ctrl key as you select blocks.
    TipTo clear the selection, click anywhere on the drawing sheet.
  2. Right-click a blank area in the drawing sheet, and select Paste. The copied block or blocks are attached to the cursor.
  3. Click to place the copied block or blocks.
  4. Continue placing the copied block or blocks. When you finish placing blocks, right-click and choose Done.

Pattern symbols or blocks

You can create a rectangular pattern of symbols or AutoCAD blocks on a drawing sheet. This command creates multiple copies of symbols or blocks with a uniform distance between instances. This command works with Inventor symbols, sketched symbols, and AutoCAD blocks. The pattern operation is a copy operation and the position of the symbols is not associative.

  1. Right-click an inserted symbol or block in the browser or in the graphics window and select Pattern Symbols/Blocks.
  2. Select additional symbols or blocks to pattern.
  3. The default Direction 1 is horizontal and Direction 2 is vertical. Select the Direction button then select a line in a view or sketch to change the direction.
  4. Enter the count (number of symbols/blocks) and the spacing (distance between instances) for Direction 1.
  5. Enter the count and spacing for Direction 2.
    NoteYou can create a single directional pattern by setting the count equal to 1 for either Direction 1 or Direction 2.

Import AutoCAD block definitions

You can import blocks from any dwg file into the current dwg file. A block instance is inserted onto the current drawing sheet and listed in the AutoCAD Blocks folder under the Sheet node in the browser. The block definition is listed in the browser in the AutoCAD Blocks folder in the Drawing Resources folder.

 
  1. Open an existing dwg file or start a new file using a dwg template.
  2. On the ribbon, click Annotate tabSymbols panel Import AutoCAD Block.
  3. Browse to and select the dwg file that contains the block definition.
  4. In the Block Definition area, select the block to insert.
  5. Set the scale and rotate values.
  6. Click Insert.
  7. Click in the graphics window to place the block.
  8. If the block definition has attributes, enter the values in the Edit Attribute dialog box and click OK.
  9. Click again to place additional blocks.
  10. Right-click and select Done to end the command or Restart to return to the Insert Block dialog box.

If there is no preview available for the block, a "?" icon is shown in the Block Definitions area of the Import AutoCAD Block dialog box.

When inserting a block with the same name as an existing block in the target file, the new block is inserted as "Copy of [duplicate name]" in the target file.

Dynamic blocks are inserted using the default configuration from the block definition.

Add symbols to prompted entries

 

A prompted entry prompts you for an entry when this property is defined in a title block, border, or sketched symbol. In addition to text, you can add a character, such as a diameter symbol to a prompted entry.

  1. On the taskbar, click Start Programs Accessories System Tools Character Map.

    The Microsoft Windows Character Map dialog box displays.

  2. Double-click the appropriate symbol.
  3. Click Copy, and then paste the value cell in the Prompted entry or Edit property fields dialog box.
NoteSymbols added in the Format Text dialog box from the Insert symbol menu, use the AIGDT (Autodesk Inventor Geometric Dimensioning and Tolerancing) font. You can change the font of symbol by copying symbols from the Microsoft Windows Character Map dialog box.

References

Symbols

Adds sketched symbols to a drawing sheet. You can rotate and scale the symbols as you add them, add leaders, and associate the symbols to views on the sheet.

Access:

  • Ribbon: Annotate tab Symbols panel User
  • In the Model browser, click to expand the Drawing Resources folder and then click to expand the Sketched Symbols folder. Right-click one of the entries and select Symbols.

The Symbols dialog box lists symbols defined in the Drawing ResourcesSketched Symbols folder in the browser. Symbols created in the current drawing are saved only in this file. Symbols created in a template file are available in all drawings using the template.

Symbol list

Shows the symbols available in the drawing. The default order is the same as the browser. Click to a symbol to select it.

Contents can be sorted using drag and drop or right-click in the list and choose Sort by Name.

Scale

Sets the scale for the symbol, relative to the drawing sheet.

Rotate

Specifies the degrees of rotation around the symbol insertion point. If the symbol does not have a defined insertion point, rotates the symbol around its center.

Symbol Clipping

Select the check box to trim dimension lines, leader lines, and extension lines behind symbols attached to a drawing view. Clear the check box to show leader or extension lines across the symbol.

Static

Specifies if the symbol can be manually resized and rotated on the drawing sheet. Select the Static check box to turn off scale and rotation grip points on the symbol. Clear the check box to allow manual resizing and rotation of the symbol.

Leader

Places the symbol with a leader. Select the check box to add a leader. Clear the check box to place the symbol without a leader.

When editing a symbol, clearing the Leader check box deletes the leader.

The Visible check box specifies whether or not the leader is visible. If not visible, the dashed leader line is shown while the leader is created or the symbol instance is manipulated. Not available if the Visible leader check box is not selected.

Edit Property Fields, Prompted Texts, Attributes

Sets or changes the values of prompted entries and iProperties in a title block, border, or sketched symbol. The iProperties are edited in the Properties dialog box, which is displayed when you click iProperties in the Edit Property Fields dialog box.

If a sketched symbol is created without a leader or edited to delete a leader, it loses its association with model properties. Restoring a leader re-associates the symbol with model properties.

Access:

In the browser, right-click a sketched symbol, border, or the Field Text entry of a title block, and then select Edit Field Text.

The dialog box displays automatically when you insert a title block, border, or sketched symbol containing prompted entries in the drawing.

Property Type list

Selects the type of property to display in the table. Properties of all other types are filtered out from the table. Choose All to display the list of all iProperties and prompted values.

Property Field

Lists the titles of iProperties and prompted values included in the selected title block, border, or sketched symbol.

NoteTo change the titles of prompted values you must edit the definition of the format or symbol in the Drawing Resources folder.

Value

Shows the current value for each property and prompted entry. Only values for prompted entries can be edited in the Edit Property Fields dialog box. To edit a value, double-click to select it, and then enter the new value in the edit box.

NoteTo edit iProperties, click iProperty to display the iProperty dialog box.
 

Displays the iProperties dialog box. You can edit the iProperties, save the edits, and return back to the Edit Property Fields dialog box.

NoteWhen using the Drawing Resource Transfer Wizard to copy drawing resources from a source to one or more target drawings, prompted entries may not transfer correctly if they do not match exactly in the source and target files.
TipTo change the order of prompted entries in the Property Fields list, right-click the corresponding object (for example title block or sketch symbol) in Drawing Resources, and select Reorder Prompted Entries from the menu. Then change the order of prompted entries in the Reorder Prompted Entries dialog box.

Reorder Prompted Entries

Use the Reorder Prompted Entries dialog box to change the order of prompted entries included in a drawing resource, for example in a sketched symbol or title block.

The ordered list of prompted entries is displayed in the Edit Property Fields and Prompted Texts dialog box.

Access:

In the drawing browser, right-click a drawing resource which includes 2 or more prompted entries, and select Reorder Prompted Entries from the menu.

Prompted Entries

Lists all prompted entries included in the selected drawing resource object. Select one or several prompted entries in the list to move them to the desired position.

Move Down

Moves the selected prompted entry (entries) one row down in the list. Available only if one or several contiguous prompted entries are selected.

Move Up

Moves the selected prompted entry (entries) one row up in the list. Available only if one or several contiguous prompted entries are selected.
Tip(Drag and Drop) Drag a prompted entry to the desired position in the list. If needed, hold CTRL to select several prompted entries at the same time, and drag the selection to the desired position. The prompted entries are grouped and inserted in their original order.

AutoCAD Blocks

View blocks are created for each base view and projected view in a DWG drawing sheet when the DWG drawing is saved.

The view blocks display in the browser in the AutoCAD blocks folder under Drawing Resources. You can rotate and scale the blocks as you add them.

Blocks can also be imported from AutoCAD dwg files. Blocks can be inserted onto a drawing sheet similar to sketched symbols.

Access:

In the Model browser, click to expand the Drawing Resources folder and then click to expand the AutoCAD Blocks folder. Right-click one of the entries and select AutoCAD Blocks from the context menu.

AutoCAD Block list

Shows the AutoCAD Blocks available in the drawing. The default order is the same as the browser. Click to a symbol to select it.

Contents can be sorted using drag and drop or right-click in the list and choose Sort by Name.

Scale

Sets the scale for the block, relative to the drawing sheet.

Rotate

Specifies the degrees of rotation around the block insertion point. If the block does not have a defined insertion point, rotates the symbol around its center.

Static

Specifies if the block can be manually resized and rotated on the drawing sheet. Select the Static check box to turn off scale and rotation grip points on the block. Clear the check box to allow manual resizing and rotation of the block.

Import AutoCAD Blocks

Adds AutoCAD Blocks to a drawing sheet from another dwg file. The block definition is copied into the current dwg file and an instance of the block is inserted onto the current sheet. You can set rotate and scale values in the dialog box.

Access:

  • Ribbon: Annotate tab Symbols panel Import
  • In the Model browser, click to expand the Drawing Resources folder. Right-click on the AutoCAD Blocks folder and select Import AutoCAD Block.

Look in

Shows path of the active directory.

File list

The main window shows a list of the subfolders and files in the selected path. Double-click a subfolder to show the files it contains.

File name

Specifies the file to open, enter a file name, or select a file from the listed files.

Files of type

Filters file list to include only files of a specific type. Click the arrow to show list, and then highlight to select a file type.

Block Definitions

Lists the block definitions in the selected dwg file.

  • Thumbnail view
  • List view

Insert

Insert the selected block.

Cancel

Cancels the import block operation and closes the dialog box.

Scale

Specify a scale factor to increase or decrease the size of the block.

  • A value between 0 and 1 will decrease the size of the block
  • A value greater than 1 will increase the size of the block.

Rotate

Specify a value to rotate the block.

Pattern Symbols/Blocks

Creates a rectangular pattern of the selected symbols/blocks. This command works with Inventor symbols, sketched symbols, and AutoCAD blocks. The pattern operation is a copy operation and the position of the symbols is not associative.

Access:

Right-click on any inserted symbol or block and select Pattern Symbols/Blocks. You can right-click on the symbol/block in the browser or the graphics window.

 

Symbols / Blocks selects one or more symbols, sketched symbols, or blocks to include in the pattern.

Direction 1

Aligns selected symbols or blocks in the direction defined by selected line.

 

Direction Selects the direction in which occurrences are added. Direction arrow originates at the selection point. Path can be a line in a view or block on the drawing sheet.

 

Flip Reverses direction of patterned occurrences.

 

Count Specifies the number of occurrences in the column. Must be greater than zero. To specify a single direction pattern, the count must be equal to 1 for Direction 1 or Direction 2.

 

Length Specifies distance between occurrences in the direction of the selected line. Must be greater than zero.

Direction 2

Aligns selected symbols or blocks in the direction defined by selected line.

 

Direction Selects the direction in which occurrences are added. Direction arrow originates at the selection point. Path can be a line in a view or block on the drawing sheet.

 

Flip Reverses direction of occurrences.

 

Count Specifies the number of occurrences in the row. Must be greater than zero. To specify a single direction pattern, the count must be equal to 1 for Direction 1 or Direction 2.

 

Length Specifies distance between occurrences in the direction of the selected line. Must be greater than zero.

Datum Target symbol

 

Specifies the size and label for the datum target.

Access:

Ribbon: Annotate tab Symbols panel Datum Target, and then click the arrow next to the Datum Target command and choose the datum target type from the pop-up menu.

Dimension

Specifies size of the target area. Enter the number.

Datum

Specifies the label for the target.

Edit Unit Attributes

Sets the format for numeric information for measurement units in text, feature control frames, and datum target symbols.

Access:

Select an existing text box, feature control frame, or datum target symbol. Right-click and select Edit Unit Attributes.

Use Standards Notation

Sets the format for the measurement units to the settings specified by the active standard style when the selected symbol was placed.

Check the box to use the settings in the drafting standard. Remove the check mark to change the settings for the selected text box, feature control frame, or datum target symbol.

Primary Units

Changes the format of the primary units of measure for numeric information in the selected text box, feature control frame, or datum target symbol.

Linear

Sets the units of measurement. Click the arrow and select from the list. If no unit type is specified, the unit type of the applicable drafting standard is used.

Decimal Marker

Specifies the character to use as a decimal. Click the arrow and select from the list.

Unit String

Displays the primary unit type after the value in the selected text, feature control frame, or datum target symbol. Select the box to display the unit type, clear the check mark to hide the unit type.

Leading Zeros

Shows or suppresses the display of leading zeros in values. Select the box to display leading zeros, clear the check mark to suppress them.

Trailing zeros

Shows or suppresses the display of trailing zeros in values. Select the box to display trailing zeros, clear the check mark to suppress them.

Alternate Units

Displays or hides alternate units. Select the box to display alternate units, clear the check mark to hide them.

Display style

Sets the display style for alternate units. Click the arrow and select from the list.

Alternate Units

Changes the format of the secondary units of measure for values for numeric information in the selected text box, feature control frame, or datum target symbol. Not available unless Display Alternate Units is selected.

NoteIf a symbol or text box contains multiple numeric values, only the first valid value receives an alternate unit notation.

Linear

Sets the units of measurement. Click the arrow and select from the list. If no unit type is specified, the unit type of the applicable drafting standard is used.

Decimal

Specifies the character to use as a decimal. Click the arrow and select from the list.

Unit String

Displays the alternate unit type after the value in the selected text box, feature control frame, or datum target symbol. Select the box to display the unit type, clear the check mark to hide the unit type.

Leading Zeros

Shows or suppresses the display of leading zeros. Select the box to display trailing zeros, clear the check mark to suppress them.

Trailing zeros

Shows or suppresses the display of trailing zeros. Select the box to display trailing zeros, clear the check mark to suppress them.

Precision

Sets the decimal precision for display of alternate units. Click the arrow and select from the list.

Feature Control Frame

 

Specifies the content of a feature control frame. The options in the dialog box are determined by the active feature control frame style.

The feature control frame can be rotated with options on the context menu.

Access:

  • Ribbon: Annotate tab Symbols panel Feature Control Frame
  • Click to place in the graphics window, and then right-click and select Continue to open the Feature Control Frame dialog box.

Sym

Specifies the tolerance symbol. Click to open the symbol palette and select the desired symbol. The symbols on the palette are determined by the active drafting standard.

Tolerance

Sets the tolerance values.

Tolerance 1 specifies the tolerance.

Tolerance 2 specifies the lower tolerance (ANSI standard only).

Datum Identifier

Specifies the datum identifier related to the feature control frame.

Insert modifier

Adds modifier characters to the text at the insertion point. Click the desired character to add it. The available characters are determined by the active drafting standard.

Notes

Optionally, add notes to the feature control frame.

All Around

Adds an all-round character next to the feature control frame. Select the check box to add the character. Clear the check box to remove it. The diameter of the all-round character is determined by the Leader style.

NoteThe text boxes in the second row are available only if you select a tolerance-type symbol for the row. You can specify in the active drafting standard whether to merge corresponding fields when the information is the same.

Surface Texture Symbol

 

Specifies the content of a surface texture symbol. The options in the dialog box are determined by the surface texture style.

Access:

Ribbon: Annotate tab Symbols panel Surface

Symbols can be created as stand-alone objects, be placed directly on the geometry in a drawing view, or reside on top of a leader line which points to the geometry. Surface Texture Symbols can also be used in notes and in the tolerance block.

Surface Type

Select the desired surface type.

Basic

Material removal required

Material removal prohibited

Miscellaneous

Specifies the general attributes of the symbol.

Force tail adds a tail to the symbol.

Majority indicates that this symbol specifies the standard surface characteristics for the drawing.

All-round adds the all-round indicator to the symbol. The diameter is specified in the Leader style.

Surface characteristics

Defines the values for the surface characteristics. Enter the appropriate values in the boxes.

A specifies the roughness value, roughness value Ra minimum, minimum roughness value, or grade number. Available only when A' has an entered value.

A' specifies the roughness value, roughness value Ra maximum, maximum roughness value, or grade number.

B specifies the production method, treatment, or coating. If the active drafting standard is based on ANSI, this box can be used to enter a note callout.

B' specifies an additional tail for the production method if the drafting standard is based on ISO or DIN. This option is available only when B has an entered value.

C for ANSI, specifies the roughness cutoff or sampling length for roughness average; for ISO or DIN, specifies the waviness height or sampling length. For JIS, specifies the cutoff value and evaluation length.

C' for ANSI, specifies the roughness cutoff or sampling length for additional roughness value. For ISO or DIN, specifies the sampling length for additional roughness value; for JIS, specifies the reference length and evaluation length.

D specifies the direction of lay. Click the arrow and choose the symbol from the list. This option is not available when the removal prohibited option is selected.

E Not available when the Machining Removal Prohibited is selected. Specifies the machining allowance.

F specifies the roughness value other than Ra or the parameter value other than Ra. For ANSI, can also specify the waviness height.

F' specifies the surface waviness for JIS. This option is not used for ANSI, ISO, or DIN standards.