Figure 4­47 Sketch for the revolved feature and linear diameter dimensioning

Ordinate Dimensioning
The ordinate dimensions are used to dimension a sketch with respect to a
specified datum. Depending on the requirement of the design, the datum can be
an entity in the sketch or the origin. The ordinate dimensions are of two types,
horizontal and vertical. The methods of creating these types of ordinate
dimensions are discussed next.
Horizontal Ordinate Dimensioning
CommandManager: Sketch > Smart Dimension flyout > Horizontal Ordinate
Dimension SOLIDWORKS menus: Tools > Dimensions > Horizontal Ordinate
Toolbar: Dimensions/Relations > Horizontal Ordinate Dimension The
horizontal ordinate dimensions are used to dimension the horizontal
distances of the selected entities from the specified datum, refer to Figure 4­
48. Note that when you apply the ordinate dimensions, the Modify dialog
box will not be displayed to modify dimension values. After placing all
ordinate dimensions, you need to exit the ordinate dimensioning tool and
then double­click on the dimensions to modify their values.

To apply a horizontal ordinate dimension, choose the Horizontal Ordinate

Dimension tool from the Sketch CommandManager; you will be prompted to
select an edge or a vertex. Note that the first entity selected is taken as the datum
entity from where the remaining entities will be measured. Select the first entity
and place the dimension above or below it. You will notice that the dimension
shows the value 0. Refer to the dimension of the left vertical line in Figure 4­48.

After placing the first dimension, you will be prompted again to select an edge
or a vertex. Select the edge that you need to dimension with respect to the first
selected edge as datum. As soon as you select the edge, a horizontal dimension
between the datum and the entity will be placed. Similarly, place other
dimensions to apply multiple horizontal ordinate dimensions, refer to Figure 4­
48.
Figure 4­48 Horizontal ordinate dimensions
Vertical Ordinate Dimensioning
CommandManager: Sketch > Smart Dimension flyout> Vertical Ordinate
Dimension SOLIDWORKS menus: Tools > Dimensions > Vertical Ordinate
Toolbar: Dimensions/Relations > Vertical Ordinate Dimension The vertical
ordinate dimensions are used to dimension the vertical distances of the
selected entities from the specified datum, see Figure 4­49. To add a vertical
ordinate dimension, choose the Vertical Ordinate Dimension tool from the
Sketch CommandManager; you will be prompted to select an edge or a
vertex. As mentioned earlier, the first entity that you select is taken as the
datum entity from where the remaining entities are measured. Select the
first entity and place the dimension on its right or left. You will notice that
the dimension shows the value 0. Refer to the dimension of the bottom
horizontal line in Figure 4­49. Next, select the edge that you need to
dimension with respect to the first selected edge as datum. As soon as you
select the edge, a vertical dimension will be placed between the datum and
this entity. Similarly, place other dimensions to create multiple vertical
ordinate dimensions, refer to Figure 4­49.

Figure 4­49 Vertical ordinate dimensions

Path Length Dimension
CommandManager: Sketch > Smart Dimension flyout> Path Length
Dimension SOLIDWORKS menus: Tools > Dimensions > Path Length
Dimension Toolbar: Dimensions/Relations > Path Length Dimension The Path
Length Dimension tool is used to dimension a chain of sketch entities which
are coincident. You can set the dimension as a driving dimension, so that
when you drag the entities, the shape of the path changes but its length
remains same.

CONCEPT OF A FULLY DEFINED SKETCH

IT IS IMPORTANT FOR YOU TO
UNDERSTAND THE CONCEPT OF FULLY
DEFINED SKETCHES. WHILE CREATING A
MODEL, YOU FIRST NEED TO DRAW THE
SKETCH OF THE BASE FEATURE AND
THEN PROCEED FURTHER TO CREATE
OTHER FEATURES. AFTER CREATING
THE SKETCHES, YOU NEED TO ADD THE
REQUIRED RELATIONS AND DIMENSIONS
TO CONSTRAIN THE SKETCH WITH
RESPECT TO THE SURROUNDINGS.
AFTER ADDING THE REQUIRED
RELATIONS AND DIMENSIONS, THE
SKETCH MAY EXIST IN ANY OF THE SIX
STATES DISCUSSED NEXT:
Fully Defined
A fully defined sketch is the one in which all entities of the sketch and their
positions are completely defined by the relations or dimensions, or both. In a
fully defined sketch, all degrees of freedom of a sketch are constrained.
Therefore, the sketched entities cannot move or change their size and location
unexpectedly. If a sketch is not fully defined, it can change its size or position at
any time during the design because all degrees of freedom are not constrained.
All entities in a fully defined sketch are displayed in black.
Overdefined
An overdefined sketch is the one in which some of the dimensions, relations, or
both are conflicting or the dimensions or relations have exceeded the required
number. An overdefined sketch is displayed in yellow. It is recommended not to
proceed further to create the feature with an overdefined sketch. When a sketch
is overdefined, you need to delete the extra and conflicting relations or
dimensions. An overdefined sketch can be changed to fully defined or
underdefined sketch by deleting the conflicting relations or dimensions. You will
learn more about deleting the overdefining relations or dimensions later in this
chapter.
Underdefined
An underdefined sketch is the one in which some of the dimensions or relations
are not defined and the degree of freedom of the sketch is not fully constrained.
In these types of sketches, the entities may move or change their size
unexpectedly. As a result, the sketched entities of the underdefined sketch are
displayed in blue. When you add relations and dimensions, the color of the
entities in the sketch changes to black, indicating that the sketch is fully defined.
If the entire sketch is displayed in black and only some of the entities are
displayed in blue, it means that the entities in blue require some more
dimensions or relations.

Tip 1. In SOLIDWORKS, it is not necessary to fully dimension or define the

sketches before using them to create the features of a model. However, it is
recommended that you define the sketches fully before you proceed further to
create the feature.

2. If you always want to use fully defined sketches before proceeding further, you
can do so by choosing Tools > Options from the SOLIDWORKS menus to
display the System Options ­ General dialog box. Select the Sketch option from
the area on the left. Next, select the Use fully defined sketches check box and
choose OK from this dialog box.

Note This chapter onward, you will work with fully defined sketches. Therefore,
follow the above mentioned procedure to use the fully defined sketches.
Dangling
In a dangling sketch, the dimensions or relations applied to an entity lose their
reference because of deletion of the entity from which they were referenced.
These entities are displayed in brown. You need to delete the dangling entities,
dimensions, or relations that conflict.
No Solution Found
In the no solution found state, the sketch is not solved with the current
constraints. Therefore, you need to delete the conflicting dimensions or relations
and add other dimensions or relations. In such cases, the sketched entity,
dimension, or relation will be displayed in yellow.
Invalid Solution Found
In the invalid solution found state, the sketch is solved but it will result in invalid
geometry such as a zero length line, zero radius arc, or self­intersecting spline.
The sketch entities in this state are displayed in yellow.

Sketch Dimension or Relation Status In SOLIDWORKS,

while applying the dimensions and relations to the
sketches, sometimes you apply the ones that are not
compatible with the geometry of the sketched entities or
they make the dimensioned entity overdefined. In
addition to the fully defined state, the sketch dimensions
or relations may have any of the following states:
Dangling Satisfied Overdefining Not Solved Driven
Dangling
A dangling dimension or relation is the one that cannot be resolved because the
entity to which it was referenced is deleted. The dangling dimension appears in
golden brown.
Satisfied
A satisfied dimension is the one that is completely defined and is displayed in
black.
Overdefining
An overdefining dimension or relation overdefines one or more entities in a
sketch. This type of dimensioning appears in yellow.
Not Solved
The not solved dimension or relation cannot determine the position of the
sketched entities. The not solved dimension appears in yellow.
Driven
In a sketch, the driven dimension’s value is driven by other dimensions that
solve the sketch. The driven dimension appears in gray.

Tip In the sketching environment, the status bar of the SOLIDWORKS window is
divided into four areas. The Sketch Definition area of the status bar always
displays the status, dimension, and relation applied to the sketch. If the sketch is
underdefined, the status area will display Under Defined; if the sketch is
overdefined, the message displayed in the status area will be Over Defined; and
if the sketch is fully defined, the message displayed in the status area will be
Fully Defined.

DELETING OVERDEFINED DIMENSIONS

In solidworks, when you add a dimension that overdefines a sketch, the color of
the sketch and dimension changes and the Make dimension driven? Message
box is displayed, as shown in figure 4­50. This message box informs you that
adding this dimension will overdefine the sketch or the sketch will not be solved.
You are also prompted to specify whether you want to add the dimension as a
driven dimension. If you select the Make this dimension driven radio button
and choose Ok, then the selected dimension will become a driven dimension.
The driven dimension is displayed in gray and cannot be modified. Its value
depends on the value of the driver dimension. If you change the value of the
driver dimension, the value of the driven dimension will
be automatically changed.

Figure 4­50 The Make Dimension Driven? message box

If you select the Leave this dimension driving radio button and choose OK,
then some of the entities and dimensions in the sketch will be displayed in
yellow. Next, you need to delete the relation or dimension that is overdefining
the sketch. In SOLIDWORKS, the Over Defined button is provided in the status
bar, as shown in Figure 4­51.

Figure 4­51 The Over Defined button in the status bar

To resolve the overdefining relations or dimensions, click on the Over Defined

button displayed in the status bar; the SketchXpert PropertyManager will be
displayed, as shown in Figure 4­52. In this PropertyManager, you can choose the
Diagnose button in the Message rollout to automatically resolve possible errors
or choose the Manual Repair button to resolve errors manually. On choosing
the Diagnose button, the relations or dimensions that need to be deleted will be
displayed in the Results rollout. Also, the conflicting relations will be listed in
the More Information/Options rollout. Choose the arrows in the Results
rollout to view various solutions. On choosing the arrows, the additional relation
or dimension to be deleted will be displayed with a strike mark. Figure 4­53
shows the sketch that is overdefined because of the additional vertical dimension
100. Figure 4­54 shows the additional vertical relation struck out. To remove a
particular relation or dimension, choose the Accept button in the Results rollout;
the relation or dimension that has been struck out will be removed and the sketch
will be fully defined. Also, a message informing that the sketch can now find a
valid solution will be displayed in the SketchXpert PropertyManager. Choose
the OK button.
Figure 4­52 Partial view of the SketchXpert PropertyManager
 Figure 4­53 The overdefined sketch

Figure 4­54 The additional vertical relation struck out

Choose the Manual Repair button from the Message rollout; the relations or
dimensions that are responsible for over defining the sketch will be displayed in
the Conflicting Relations/Dimensions rollout, as shown in Figure 4­55. Select
any of the relations or dimensions that is responsible for overdefining the sketch
and choose the Delete button. If the overdefining status of the sketch is removed,
then a message stating that the sketch can now find a valid solution will be
displayed in green background in the Message rollout. If the dimensions or
relations deleted are not sufficient to find out a valid solution, the Conflicting
Relations/Dimensions rollout will still be displayed. Therefore, you need to
delete few more dimensions or relations to remove the overdefining status from
the sketch.
 Figure 4­55 The Conflicting Relations/Dimensions rollout

You need to delete the relation or dimension displayed in red to make sure that
the sketch is no longer overdefined. When the sketch is no longer overdefined,
the Message rollout in the SketchXpert PropertyManager will inform you that
The sketch can now find a valid solution. Choose OK from the SketchXpert
PropertyManager; the sketch will be displayed in black or blue, depending on
the current state of the sketch. Note that if you select the Always open this
dialog box when sketch error occurs check box in the More
Informations/Options rollout of the SketchXpert PropertyManager, the
SketchXpert PropertyManager will be displayed automatically when a sketch
is overdefined.