On the ribbon, click to create a 2D sketch. The sketch is added to the drawing sheet or, if a view is selected, is associated with the active view.
Once you create a sketch, the Sketch tab has commands you can use to create custom borders and title blocks, or to develop your own set of sketched symbols.
You can get model sketches in a drawing view by using Get Model Sketches command. After the model sketch is recovered, the sketch attributes do not automatically update with respect to changes in the model sketch. To update the attributes of the recovered sketch, right-click the sketch in the graphic window or in the browser, and select Reapply Model Properties from the menu.
If you translate AutoCAD data to a drawing, the geometry is placed on sketches in the drawing. AutoCAD line styles are maintained.
A drawing sketch can contain text and 2D geometry such as lines and arcs. If a drawing view is selected when you activate the Sketch commands, the sketch is associated to the view. If no drawing view is selected, the sketch is associated to the drawing sheet.
If you copy a sheet or a drawing view, the associated sketches move with it. You cannot copy or move a sketch independently of its associated sheet or view.
A sketch cannot be copied, but you can copy the geometry in a sketch, and paste it in another drawing.
Tips for sketching in a drawing
The drawing templates contain a Sketched Symbols heading in the Drawing Resources section of the browser so that you can create and save sketches for reuse. Sketched symbols can contain 2D geometry, bitmap images, static text, prompted text boxes, or properties fields that update automatically.
To make the sketched symbols available in new drawings, save them in a template that you use to create drawings.
The templates provided with Autodesk Inventor contain one or more standard title block formats that you can modify and use. You can also sketch custom title blocks, and save them as drawing resources. Title blocks can contain 2D geometry, bitmap images, static text, prompted text boxes, or properties fields that update automatically.
To use the custom title blocks in all your new drawings, save them in a template that you use to create drawings.
Custom borders can contain 2D geometry, bitmap images, static text, prompted text boxes, or properties fields that update automatically. To use a custom border in new drawings, save it in a template that you use to create drawings.
All drawing borders have four points at the sheet corners that cannot be deleted. These points move when the sheet is resized. If you constrain the custom border geometry to these points, it adapts to any sheet size.
To place dimensions attached to the geometry on the sketches, select Promote Dimensions to Sketch in the Import Destination dialog box when opening an AutoCAD file. AutoCAD line styles are maintained.
On the Sketch tab, use the commands to add sketched elements to a drawing. Drawing sketches are associated with the drawing sheet, but if a drawing view is selected, the sketch is associated with the view.
To add sketch geometry to an existing sketch, right-click a sketch in the browser, and then select Edit.
You can view or change line attributes for new or edited sketch geometry.
Tip: On the ribbon, click to display the Sketch Properties toolbar.
You can hide one or more sketch elements in a drawing sketch without making the entire sketch invisible by setting the Sketch Only attribute.
Geometry with the Sketch Only attribute set is hidden when you exit from sketch mode and is no longer visible on the face of the drawing.
If you wish to restore the visibility of the hidden sketch elements:
The browser for each drawing or drawing template contains a Sketched Symbols folder in the Drawing Resources folder. When you create custom symbols, they are added to Sketched Symbols available to use in the drawing.
A sketched symbol can contain geometry, text, or imported bitmap images.
If you prefer, right-click the Sketched Symbols folder in the browser and select Define New Symbol.
A draft sketch is a special drawing view that contains no representation of a model. When you open an AutoCAD file as an Autodesk Inventor drawing, a new file is created with a sheet that contains a draft sketch. Geometry from the AutoCAD file is placed in the draft sketch.
You can scale a draft sketch and give it a label. If you later copy data from a draft sketch to another sketch, the copied geometry is shown with a 1:1 scale in the sketch.
You can add a draft sketch even if you do not have AutoCAD data:
You can showand from a model in a drawing view of the model. You cannot edit a model sketch in the drawing.
Only sketches that are parallel to the view can be displayed.
Click Fill/Hatch Sketch Region to hatch or color fill an enclosed boundary in a drawing sketch.
When you edit attributes of a hatch fill, all edits are kept as object overrides.
Adds hatch or color fill to an enclosed boundary in a drawing sketch.
And then select a closed sketch profile in the graphic window
| ||Hatch switches the hatch fill on. Enables the Hatch options|
| ||Color Fill switches the color fill on. Enables the Color option.|
|Pattern||Selects the hatch pattern to use. |
Select Other to add a hatch pattern to the Pattern list. Then add the hatch pattern using the
|Angle||Rotates the hatch pattern by the specified angle. Enter the desired angle.|
|Sets the distance between lines in the hatch. |
A scale of 1 uses the original distance specified in the hatch pattern. A scale of 0.5 results in line spacing that is one half of the original distance.
Shifts the hatch pattern to offset it slightly from the original hatch pattern position. Enter the distance for the shift.
Displays a preview of the hatch pattern definition.
Sets the hatch line weight.
Creates a copy of the specified hatch pattern perpendicular to the first hatch pattern.
Sets the color of the fill for the selected sketched profile. Click to open the Color dialog box and select the color.
Changes the line type, line weight, and color for selected edge, feature or part to the value specified in the style or for the current document, overrides values set in the style.
Manages properties for view edges, symbols, feature and component selection priorities, trails, user-defined symbols, and sketch geometry.
Right-click on the edge of an object, and then select Properties from the menu.
Available only when the Select command on the Quick Access toolbar is set to either Feature Priority or Part Priority. Select the check box to show properties specified as By Layer. Clear the check box to set Line Type, Line Weight, or Color independently.
Specifies how a line or type of curve is displayed. Set to By Layer to inherit the line type specified for the layer.
Specifies the thickness of the line type. Set to By Layer to inherit the line weight specified for the layer.
Available only in a drawing sketch. Changes the scale of the selected line type. Enter scale size in the text box.
Sets the line color for the line type. Set to By Layer to inherit the color specified for the layer.
Use the Format Text dialog box to set the attributes for a drawing or sketch text.
Specifies the text style to apply to the text. Click the arrow and select from the list of available text styles.
Specifies the paragraph attributes for selected text.
Justification positions the text within the text box.
Base Line Justification is available when Single Line Text is selected and when creating sketch text.
Text box allows constraining and dimensioning to text. Available only for sketch text.
Fit text sizes the text to fit the designated space, such as a text box. Available only for sketch text.
% Stretch specifies the text width. Enter 100 to display the text as designed, enter 50 to decrease the width of the text by 50%.
Single line text removes all line breaks from multiline text. Available only for sketch text.
Spacing sets the line spacing to Single, Double, 1.5 Lines, Multiple, or Exactly.
Value specifies the value for line spacing, when you set line spacing to Exactly or Multiple.
Specifies the font attributes for the text.
|Specifies the text font. Click the arrow and select from the list of available fonts.|
|Font Size||Sets the height of the text in sheet units (inches or millimeters). Enter the size or click the arrow and select a size from the list.|
|Style||Sets the style. Click Bold, Italic, or Underline to apply the style to the text.|
|Stack strings in drawing texts to create diagonal or horizontal stacked fractions, and superscript or subscript strings. The option is available only if a string in a correct stacking format is selected in the edit field. Examples of correct stacking format: |
|Color||Specifies the text color. Click the Color command, and then select a color from the Color dialog box. In the Color dialog box, select the By Layer check box to set the color specified by the text layer. Clear the check box to select a color. The color command shows the selected color or layer color.|
Sets the angle of the text. Rotates the text around the insertion point. For example, if text is top and left-justified, the text rotates around the top left corner. Click the arrow to select the rotation orientation or enter the angle of rotation in the edit box.
For drawing notes, you can rotate to any angle. Enter the angle or click the arrow to select predefined angles or a recently used angle.
When retrieving model properties, the model source depends on the sketch type:
Sheet or Draft View sketch
Top-level model of the first view on the sheet. If the first base view on the sheet is deleted, the next base view on the sheet becomes the data source for properties.
Top-level model of the view.
Specifies property types from the drawing, the source model, and the custom property source file (for external and model custom properties) specified on the Drawings tab of the Document Settings dialog box. Available when creating or editing sketch text (in Sheet, View, or Draft View sketches), symbol text, title block and border text.
Specifies a property associated with the selected Type. Available when creating or editing all drawing text, including text properties in notes, leader text, sketch text, symbol text, title block, and border text.
Specifies the precision for numerical properties displayed in the text. Select the desired precision from the list.
Add Text Parameter inserts the parameter selected in Type and Property to the text. Available when creating or editing drawing text, including sketch text, symbol text, note text, leader text, title block, and border text. Not available for Prompted Entry type.
Selects a named parameter and inserts its value into the text at the insertion point. Parameter options are available only when adding or editing text in general drawing notes and dimension text.
Specifies the model file that contains the parameter. If the drawing contains views of more than one model, click the arrow, and select the file from the list. If the drawing contains derived parts, the donor parts are also included in this list.
Selects the type of parameter to show in the Parameter list. Click the arrow and select from the list.
Specifies the parameter to insert into the text. Click the arrow and select from the list. The parameters in the list change, depending on the Source you selected.
Specifies the precision for numerical parameters displayed in the text. Select the desired precision from the list.
Add Parameter adds the selected parameter from the selected component to the text.
Inserts a symbol into the text at the insertion point. Click the arrow and select the symbol from the palette. The top three symbols are diameter, degree and plus-minus, and they use the active font. All other symbols use the AIGDT font. In drawings, the available symbols are determined by the active drafting standard.
At the bottom of the symbol list, the Windows Character Map command accesses characters not available as standard keyboard characters. In the Character Map, click a character, and then click Select and then click Copy. In the Format Text pane, right-click and select Paste.
Zooms in or out on the text and symbols in the edit box. Click the up arrow to zoom in, click the down arrow to zoom out.