Drawing Dimensions

Shortcut: d

The Dimension tool for drawings work much like the Dimension tool for sketches. Activate the tool (click the icon or use the d shortcut), then:

1. Click a highlighted drawing entity (circle, arc, circle center, line, centermark, point, or thread).
2. Click a second highlighted drawing entity.
3. Click to place the dimension in the drawing.

You can edit a dimension after placement by clicking and dragging a grip point. As you move the cursor, drawing entities highlight to indicate you can dimension to them.

Linear dimensions on circular parts

It is possible to automatically add a diameter symbol to a linear dimension if the lines selected are on the same edge representing an arc or circle on its edge. This works in projected views only.

The image below shows a projected side view of a cylinder part. Select the top corner snap point. Then select the bottom corner snap point. This results in a normal linear dimension, as shown below left. However, if you first select the top edge, and then select the bottom edge, this results in the same linear dimension, but with the diameter symbol applied (shown below right).

You can use the Line-to-line tool to automatically add a diameter symbol in the same way as with the Dimension tool. The line-to-line tool works on both projected and section views.

Wall thickness of concentric circles and arcs

You can automatically dimension the wall thickness of two concentric circles or arcs. After selecting the Dimension tool, click each circle or arc and drag to place the dimension. The tool automatically dimensions the linear distance between the two circles or arcs:

Below are entity-specific dimension tools. For each tool, only specific entity types are highlighted as you move the cursor.

Place a note or dimensions on a chamfered edge.

1. Click .
2. Click the chamfered edge and an adjacent edge.
3. Move the cursor away from the edges to preview the dimension.
4. Click to place the note or dimensions.

To alter the style of the chamfer dimension (note or dimension), select the preferred style in the Properties panel, Dimensions tab, Chamfer section. For more information, see Properties.

To include a prefix for the chamfer dimension, double-click the dimension to open the dialog:

Adjust the chamfer dimension formatting as explained in Dimension.

Shortcut: ctrl+m

Place a minimum or maximum dimension directly to any combination of arcs, circles and any other geometry type, excluding curves.

1. Click .
2. Select a combination of one arc/circle and any other geometry type, excluding curves.
3. Drag to move the dimension text to desired location.
4. Click to place the dimension.

Despite clicking on the circle itself, the min-max dimension tool gives you the maximum or minimum dimension depending on where you click the entity; for example, the maximum distance, shown above as 1.420, was acquired by clicking on the top of the top circle and the bottom of the bottom circle

Measure the distance between two points. Create horizontal, vertical, and rotated linear dimensions.

You must select two points. You cannot select a line.

1. Click .
2. Hover over the drawing view to activate the snap points.
3. Click when you see an appropriate snap point.
4. Click when you see the second appropriate snap point.
5. Drag to place the dimension box.

To dimension 2 points on a hole thread:

1. Add a side view of the hole with the thread feature in the drawing.

2. Right-click on the view and select Show > Hidden lines from the context menu.

3. Select the first point on a thread line.

4. Select the second point on a thread line.

5. Drag to position the dimension box.

6. Click to place the dimension box.

Measure the distance between a point and a line. Create horizontal, vertical, and rotated linear dimensions.

You must select one point and one line.

1. Click .
2. Hover over the drawing view to activate the snap points.
3. Click when you see an appropriate snap point.
4. Click when you see the appropriate line highlighted.
5. Drag to place the dimension box.

To dimension a point and a line on a hole thread:

1. Add a side view of the hole with the thread feature in the drawing.

2. Right-click on the view and select Show > Hidden lines from the context menu.

3. Select a point on the thread line.

4. Select a thread line.

5. Drag to position the dimension box.

6. Click to place the dimension box.

Create dimensions between parallel lines.

You must select 2 lines.

1. Click .
2. Hover over the drawing view to activate the snap points.
3. Click the first line highlight.
4. Click the second line highlight. Note that only parallel lines will highlight for selection.
5. Drag to place the dimension box.

To dimension 2 lines on a hole thread:

1. Add a side view of the hole with the thread feature in the drawing.

2. Right-click on the view and select Show > Hidden lines from the context menu.

3. Select the first thread line.

4. Select the second thread line.

5. Drag to position the dimension box.

6. Click to place the dimension box.

It is possible to automatically add a diameter symbol to a linear dimension if the lines selected are on the same edge representing an arc or circle on its edge. See Linear dimensions on circular parts.

Measure the interior angle between the two legs and the exterior angle formed by two lines.

1. Click .
2. Click two lines.
3. Move the cursor between the lines to preview the inner angle dimension.

Line-to-line angular dimensions have a drag-able grip on the dimension arc for changing the angle to be measured:

Drag the grip point across one of the infinite lines through the ends of the selected edges/points to change the measured value to the supplementary or vertical angle of the angle where the text was first placed.

Dimensions can be created not only for the angle, but also for its conjugate/reflex and supplementary angles. The example below displays two sketch lines in blue. The angle of 116.4°, its conjugate/reflex angle of 243.6°, and the supplementary angles of 63.6°, are all dimensioned.

Measure an angle by selecting 3 points, including a vertex and two points on the legs:

1. Click .
2. Click the vertex.
3. Click a point on each leg on the perimeter of the arc.

Angular dimensions have a drag-able grip on the dimension arc for changing the angle to be measured.

Drag that grip point across one of the infinite lines through the ends of the selected edges/points to change the measured value.

On 3-point angular dimensions it changes from the initial angle to the outside angle (360 minus initial angle).

Before drag (below):

After drag (below):

Shortcut: Shift+r

Measure the radial dimension of a circle, arc, or circular arc centermark.

1. Click .
2. Select the arc, circle, or centermark.
3. Move the cursor and click to place the dimension.

You have the ability to foreshorten a dimension line on an arc when the center point is at an inconvenient distance from the arc on the drawing. In this case, select the dimension, right-click and select Foreshorten. A jogged line appears, drag to the desired location and click to set the endpoint.To undo the foreshortened line, select the line, right-click and select Remove foreshorten.

You can also add a Radial dimension to circles that are on either side of other geometry. For instance, the top and bottom circles below have two ellipses between them. The four sketches are lofted, and then a top view is placed in a Drawing. Radial dimensions are then added to both circles. If the circle is obscured, as is the case in the bottom circle in this example, a guide line is overlaid on top, as you add the dimension, ensuring the visibility of the circle.

Shortcut: Shift+d

Measure the diameter of a circle, arc or circular arc centermark, including silhouette edges.

1. Click .
2. Select the arc, circle, or centermark.
3. Move the cursor and click to place the dimension. A diameter symbol is included in the placement.

Placing a diameter dimension on a detail view or crop view of an arc or circle displays a foreshortened diameter dimension, as shown below.

To convert the foreshortened diameter dimension format to a direct dimension, right-click on the diameter and select Display as direct diameter (below left). This replaces the foreshortened dimension with a direct dimension (below right). This option is a toggle, so you can switch between the dimension styles at any time.

To flip the foreshortened diameter dimension to the opposite side of the extension line, hover your cursor over the grip point. When you see the flip arrow attached to the cursor, left-click the mouse. Left-click again to flip it back to the original side of the extension line:

To create a foreshortened diameter dimension for a non-cylindrical feature, select a centerline and the corner, point, or axis of choice. Selecting the foreshortened dimension highlights the reference point or edge and centerline.

You can also add a Diameter dimension to circles that are on either side of other geometry. For instance, the top and bottom circles below have two ellipses between them. The four sketches are lofted, and then a top view is placed in a Drawing. Diameter dimensions are then added to both circles. If the circle is obscured, as is the case in the bottom circle in this example, a guide line is overlaid on top, as you add the dimension, ensuring the visibility of the circle.

Create ordinate dimensions (X, Y pairs) for a feature measured from a datum. Ordinate dimensions created as a group move together when one is moved.

1. Click .
2. Click the point to serve as the datum (0, 0). Points may include edges and lines, arc, and centermarks as well as manually placed centermarks.

If the orientation of the ordinate dimension is not correct, move the mouse around the datum point until the 0,0, dimension is in the correct orientation, then click to set its location on the drawing.

3. Click each point in one direction (Y, for example) to associate with that datum point.
4. Press Escape to exit the tool.

   At this point, one Ordinate dimension group is created.

5. Click .
6. Click the point to serve as the datum (0,0).
7. Click each point in the other direction (X, for example) to associate with that datum point. This datum is able to be the same as the first datum chosen.
8. Press Escape to exit the tool.

   At this point, a second Ordinate dimension group is created.

Working with ordinate dimensions

Right-click on an ordinate dimension access the context menu for the ordinate dimension group:

• Add to ordinate dimension group - Select to add another ordinate dimension to the existing group; click a point to act as a datum point.
• Edit - Select to open the Dimension palette for the ordinate dimension group.
• Reset ordinates - If you've moved the ordinate dimension out of its original alignment, select this option to automatically move it to its previous position.
• Clear selection - Clear all selected items.
• Zoom to fit - Zoom the drawing to fit in the view.
• Delete - Delete the selected items.

Tips

• Use the inferencing to make realigning the datum points easier. Click and drag a datum point (it doesn't matter if it's a jogged position or not) to activate inferencing guidelines.

  For example, to unjog the .963 datum point below:

  

  Click and drag until the desired inferencing guideline appears, then release to place the datum point.

  

  The bold datum point (.963 to the left, above) is the point being realigned; the red crosses (plus signs) on each datum point are alignment snap indicators

  The guidelines come in especially handy when trying to jog or unjog datum points.

• Grouped ordinate dimensions can be moved as a group or singly. Drag the middle snap point of the dimension, notice the dashed lines appear on all dimensions in the group, and drag the dimension to a new position and all members of the group move in sync:

  

  Use the outmost snap point (below, on the far right) to drag a singular dimension on its own:

  

  If you subsequently move any of the group, all are moved in their relative positions, as indicated by the dashed lines:

  

• Circular grip points at arrow bases flip the arrows to the opposite side of the dimension lines.
• Each direction must have a datum; each time you initiate the command from the toolbar, the first click establishes the datum point (0, 0).
• Each direction of dimensions (Y, for example) consists of an ordinate dimension group with a single datum. To add another value pair to that group, select an existing value in the group, right-click and select Add to ordinate dimension group. This activates the command and the next click establishes the additional dimension value:

  

  

• If the drawing is updated such that the feature an ordinate dimension refers to is removed, the ordinate dimension remains and turns red. You can safely delete the dimension (right-click and select Delete, or select and press Delete).

  

• Drag the jog point, the grab point at the point in the leader where it jogs, to reposition the jog point. When you reposition the dimension, the leader will jog at the new point. You can line up all the jog points for a series of ordinate dimensions, then when you move one dimension, the jog points of all of them will stay aligned:

  

  The red line and x, above, show the alignment of the red x jog point to the others

• To change ordinate dimension style, open the Properties panel > Dimensions tab, and select ANSI or ISO from the Dimension style dropdown. ANSI ordinate dimensions display a leading line from the ordinate dimension. ISO ordinate dimensions display additional arrows that connect the increasing ordinate values from the origin point.

  

  If you use an ANSI or ISO template when creating a new drawing, the ordinate dimension style defaults to ANSI or ISO, respectively.

• Use the Drawing styles panel to style individual ordinate dimensions.

• To replicate the ordinate dimension to another view in the drawing, see Views: Replicate annotations.

See the Hole/thread callout topic.

You can customize the appearance of a selected dimension (both driving and driven) with the Dimension palette. Selecting a dimension causes the dimension palette icon to appear.

1. With no tool selected, select the dimension.
2. The Dimension palette icon appears .
3. Hover over the icon to open the palette. (You can also double-click the dimension to open the palette).
4. Set the following options in the palette:

   

   • Above text - Enter the text or symbol to appear above the dimension value.

   And then, for each of the primary dimension units and the dual dimension units, respectively:

   • Prefix text - Enter the text to appear as a prefix to the dimension value.
   • Count type - Use the dropdown to select a count type for the dimension.
   • Precision - Select the depth of unit precision (zero to 8 decimal places).

     Precision defined on a drawing dimension may be linked to the Properties panel through this Dimension palette by selecting the tolerance with “(Drawing)” beside it. Whenever the Properties panel tolerance precisions are updated, any dimension with the “(Drawing)” tolerance selected will also be updated. You can choose to link these properties (and unlink them) on a dimension-by-dimension basis.

   • Dimension units - Select the units of your choice. The currently selected unit is displayed in the dropdown label:

     

     • Choose from: Millimeters, Millimeters (Drawing), Centimeters, Meters, Inches, Inches fractional, Feet and inches, Feet, or Yards. This selection overrides the units for that dimension. If you later change the drawing units, the units for the dimension are not overridden. You can change the units back to (Drawing) if you want to inherit the drawing properties again.

     • When you choose units, you set two properties in the drawing or on a dimension - the Units property and the Fractional display property.

     • Drawing units are managed separately from Workspace units for Part Studios and assemblies
     • Feet and Inches is only available in drawings; it is not available for workspace units.
   • Suffix text - Enter the text to appear as a suffix to the dimension value.
   • Below text - Enter the text or symbol to appear below the dimension value.
   • Symbol dropdown - Select a symbol to insert from the dropdown:
     
     

     Symbol	Name	Shortcut
     °	Degree	%%d
     ⌀	Diameter	%%c
     ℄	Centerline
     ⌵	Countersink
     ↧	Depth
     ⌴	Counterbore
     □	Square
     ⌒	Arc length
     ±	Plus/Minus	%%p
     Ⓤ	Unequally disposed profile
     Ⓘ	Independency
     	Continuous feature
     	Spot face
     ▷	Translation

   • Inspection dimension - Toggle to add or remove an oval frame around the dimension to indicate this is an inspection dimension.
   • Dual dimension - Toggle to specify whether to have a single unit dimension, single unit as specified for the drawing properties, or a dual unit dimension:

     

   • Tolerance - Select None, Symmetrical, Deviation, Limits, Basic, MIN, MAX, Fit, Fit with tolerance, or Fit (Tolerance only).
     • Set the upper and lower tolerance (available for Symmetrical, Deviation, or Limits)

       

     • Optionally, to set a Deviation or Limits tolerance to plus/plus (+/+) or minus/minus (-/-), click the plus (+) or minus (-) button, as required:

       

     • Set the Fit type, Shaft class, and Hole class (available for Fit, Fit with tolerance, or Fit (Tolerance only))

       

     • Set the precision depth of the Fit tolerance units, from 0 to 8 decimal places (available for Fit with tolerance or Fit (Tolerance only))

       

   • Reset text position - Toggle to reset the text to the previous location.
   • Parentheses - Toggle to add or remove parenthesis around the dimension field.
   • Toggle hole class visibility - (Available for Fit and Fit with tolerance options) Use this to show or hide the hole class in the dimension. When shown, select one of the following options:
     • Stacked without line
     • Stacked diagonally
     • Stacked with line
   • Toggle Radius/Diameter dimension - Use this to change a radial dimension to diameter or vice versa.

You are also able to copy/paste into all text boxes, in dimensions and notes as well.

After picking two entities the dimension is drawn in a preview mode to allow final placement:

• Dragging the text around during preview allows for the text to move outside of the extension lines, and also switch between horizontal, vertical, and aligned measurement modes:

  

  

  

  

• Dragging the text away from the two chosen snap points up or down the drawing creates a horizontal dimension line:

  

• Dragging the text away from the two chosen snap points toward the side of the drawing creates a vertical dimension line:

  

• Dragging the text away in a direction perpendicular to a line through the two chosen snap points creates a dimension line parallel to the two chosen snap points:

  

• Horizontal and vertical projected snaps are also available during text placement. This allows for lining dimensions up with existing text/dimensions and other locations on the drawing:

  Hover over a marker to wake up alignment. This is available in Preview mode only. Pass over other drawing entities to wake up alignment as well, like other views’ entities.

  

When the dimension tool is selected, you can move the cursor over an edge representing a circular edge to 'wake up' the center mark. Once visible, this mark remains visible.

Upon moving the cursor over an edge, an orange circular snap point appears, with the vertical center marker:

After hover, the orange snap point disappears but the marker remains:

Change the position of dimension arrows. Use on any dimensions that display arrows or ticks.

When you select dimensions, a node displays near dimension arrows or ticks. Clicking a node flips the arrows of the dimension.

To flip dimension arrows:

1. In the graphics area, select the dimension to change.
2. Drag the value to the new position (the arrows change accordingly).

Use the right-mouse click to open a context menu on any dimension to access a list of command options for that dimension. These command options are listed below. Not all the commands listed here are available for every type of dimension.

• Edit - Opens the dimension palette to edit the dimension.

• Paste - Pastes the dimensions along with the view into the current location.

• Clear selection - Deselects the selected dimension(s).

• Zoom to fit - Zooms the entire Drawing into view.

• Delete - Deletes the selected dimension(s).