Annotations¶
Notes, hole callouts, center marks, centerlines, datum feature symbols, feature control frames, surface finish symbols and weld symbols, all on the Annotation tab. Most are attached to an edge of a view, so they move with the view and follow the model when it changes. For dimensions, see Dimensions; for balloons and tables, see Balloons and Tables.
Datum Feature and Feature Control Frame share the Tolerance button, and Surface Finish and Weld Symbol the Symbol button. Each button shows the command used last; hover over it, or click its arrow, for the other.
img/drawings/annotations-sheet.png
A part's views with a note, a hole callout, center marks, a datum feature symbol, a feature control frame and a surface finish symbol.
While a tool is on, the edge, end or center under the pointer is highlighted, and the status bar says the next step. Press Esc to end the tool. Every tool but Note needs a model on the drawing. Add a view first with Model View.
Note¶
Adds text to the sheet, with or without a leader.
- Click Note.
- Click where the note goes. For a note with a leader, first select the edge it points to, then click where the note goes.
- Type the text in the Note dialog and click OK.
The note is added and selected, and its page opens. The tool ends after each note. Canceling the dialog, or leaving it empty, adds no note.
The Note dialog has the text box and, to insert at the caret:
- Symbols: drafting symbols such as ⌀, °, ±, ⌴, ⌵ and the GD&T symbols, in the sheet font.
- Text: nX (a count prefix, such as 2X), TYP, (REF) (puts the selected text, or all of it, in parentheses), THRU, EQ SP, New Line, and ABC, which converts the text to capitals.
- Properties: Insert Property… inserts a field of the drawing or its model, such as
{PartNumber}, which fills itself in. See Title Block for the fields. - Preview: the text as it will read.
A note placed inside a view moves with the view; one placed outside the views stays where it is on the sheet. A note with a leader stays where it is on the sheet; its leader follows the edge.
Selecting a note opens its Note page:
- Text
- The note's text, on one or more lines. Fields such as
{PartNumber}are filled in from the model. - Align
- How the lines are aligned: Align left, Center or Align right.
The page also has Text Format. To edit the text in the dialog again, double-click the note.
Hole Callout¶
Adds a callout with the size of a hole or thread, taken from its feature.
- Click Hole Callout.
- Select the edge of a hole or a thread.
- Click where the callout goes.
- Select the next hole, or press Esc to end.
A hole made with the Hole feature gets that feature's callout, with the number of holes, such as 4X, when it has several, patterned copies included. A thread gets its thread's callout. Any other circle gets its diameter. An edge that is not on a hole or a thread is not accepted.
Selecting a callout opens its Hole Callout page. It shows the callout as the model gives it, and:
- Text
- The callout text.
<>stands for the hole's callout. Add lines, such as TYP, below it. Leave it empty to show the callout alone.
The page also has Text Format.
Double-click the callout, or right-click it > Edit Text…, to edit the text in the Hole Callout Text dialog. Each
line of the callout is a row of its own, <1>, <2> and so on, to change or delete, and <N> is the number of
holes. <> Callout and
Hole callouts are also added by Model Items.
Center Mark¶
Adds a center mark to a circle or arc.
- Click Center Mark.
- Select a circle or an arc. The center mark is added.
- Select the next one, or press Esc to end.
Views draw center marks on their circles by themselves when their Center marks option is on. See View Properties.
Selecting a center mark, one added by hand or one a view draws, opens the Center Mark page:
- Mark size
- The size of the mark's cross on paper. Leave it empty for the standard size for its circle.
Standard Length puts the mark's centerlines back to their standard length. To lengthen or shorten a centerline, select the mark and drag the grip at its end.
Centerline¶
Adds a centerline between two straight edges.
- Click Centerline.
- Select a straight edge.
- Select the second edge, in the same view. The centerline is added.
- Select the next pair, or press Esc to end.
Selecting a centerline, one added by hand or one a view draws, opens the Centerline page. Drag the grips at its ends to set how far it extends past the part. Standard Length puts it back.
Deleting a center mark or centerline a view draws removes it from that view. To bring the deleted ones back, click Restore Deleted Marks on the view's page.
Datum Feature¶
Adds a datum feature symbol to an edge.
- Click Datum Feature.
- Select the feature's edge.
- Click where the symbol goes.
- Select the next feature's edge, or press Esc to end.
The symbol is a filled triangle on the edge and a leader to the datum's letter, boxed. Each new symbol gets the next letter no datum on the drawing has: A, then B, and so on.
Selecting a datum feature symbol opens the Datum Feature page:
- Letter
- The datum's letter, such as
A. Typed letters are made capitals.
The page also has Text Format.
Feature Control Frame¶
Adds a geometric tolerance frame, with or without a leader to an edge.
- Click Feature Control Frame. The Feature Control Frame dialog opens.
- Set what the frame says (below) and click OK.
- Select the feature's edge for a leader, or click away from the part for a frame with no leader.
- Click where the frame goes. The tool ends, and the frame's page opens.
The dialog, and the Frame section of the frame's page, have:
- Characteristic
- The geometric characteristic: Straightness, Flatness, Circularity, Cylindricity, Profile of line, Profile of surface, Angularity, Perpendicularity, Parallelism, Position (the default), Concentricity, Symmetry, Circular runout or Total runout.
- Tolerance
- The tolerance value. Required.
- Diameter zone (⌀)
- Shows ⌀ before the tolerance, for a cylindrical tolerance zone. On by default.
- Material condition
- None, M (maximum material) or L (least material), shown circled after the tolerance.
- Datums
- Up to three datum references, separated by commas, each with its material condition if any:
A, B(M), C.
A frame with no leader placed on a view moves with the view.
Selecting a frame opens the Feature Control Frame page, to change what it says, with Text Format.
Surface Finish¶
Adds a surface finish symbol to an edge.
- Click Surface Finish, on the Symbol button.
- Select the face's edge.
- Click where the symbol goes.
The symbol is added with a leader to the edge, the tool ends, and its Surface Finish page opens to set what it says:
- Kind
- Any process, Material removal required (the default, a bar across the symbol) or Material removal prohibited (a circle in it).
- Roughness
- Written under the symbol's line, such as
Ra 3.2(the default). - Process
- The production method, such as
GROUND, written over the line. - Lay
- The lay's direction symbol:
=,⟂,X,M,C,RorP. - All around
- Adds a circle at the symbol's corner.
The page also has Text Format.
Weld Symbol¶
Adds a weld symbol to a joint's edge.
- Click Weld Symbol, on the Symbol button.
- Select the joint's edge.
- Click where the reference line starts.
The symbol is added with its arrow on the edge, the tool ends, and its Weld Symbol page opens to set what it says:
- Kind
- Fillet (the default), Square groove, V groove, Bevel groove, U groove, J groove, Plug or slot, Spot or Seam.
- Side
- Where the weld is: Arrow side, Other side or Both sides.
- Size
- The weld size. 6 by default.
- Length
- The weld length, or length and pitch for an intermittent weld, such as
50-100. - All around
- Adds the all-around circle.
- Field weld
- Adds the field weld flag.
- Tail
- A process or reference written in the tail, such as
GMAW. Empty, the symbol has no tail.
The page also has Text Format.
Selecting and Editing Annotations¶
Click an annotation to select it. Its page opens in the property panel. Every change shows on the sheet as you make it. Click OK to keep the changes as one undo step, or Cancel to put the annotation back as it was. While the page is open, Ctrl+Z takes back its changes one at a time. Press Esc to clear the selection.
Double-click a note or hole callout to edit its text in the dialog. Double-click any other annotation to open its page.
Text Format¶
The pages of notes, hole callouts, datum feature symbols, feature control frames, surface finish and weld symbols end with:
- Height
- The text height on paper. Leave it empty for the height in Document Properties > Annotations. See Drafting Standard.
- Layer
- The layer the annotation is on. Shown when the drawing has layers. See Layers.
Moving Annotations¶
Drag an annotation to move it. A note outside the views snaps its box's corners, the middles of its sides or its middle to the ends and centers of the model under them. A selected note shows its box dashed.
A selected note, hole callout, datum feature symbol or feature control frame with a leader has a grip at the leader's tip. Drag it onto another edge or point to attach the leader there. A hole callout's tip goes only onto the edge of a hole or a thread, and it then shows that hole's callout. A note's leader can go to any view; the others stay in their own view.
Deleting Annotations¶
Select an annotation and press Del, or right-click it > Delete. Deleting a view deletes the annotations attached to it too.
An annotation whose edge is gone from the model is dangling. It shows in red on the sheet, with what it showed last, and the design tree lists it under its sheet with (Dangling). Delete it, or add it again.
The Annotation Menu¶
Right-click an annotation:
| Item | Does |
|---|---|
| Edit Text… | Edits the text in the dialog. For notes, dimensions and hole callouts. |
| Properties… | Opens the annotation's page |
| Delete | Deletes the annotation. |