Home / Creo Parametric / Applying Shrinkage by Dimension

Applying Shrinkage by Dimension

You can specify one shrinkage ratio for all model dimensions, or
specify unique ratios for individual model dimensions.
• Dimensions with shrinkage ratios
applied appear magenta in the
graphics window.
• Select individual feature
dimensions to add shrinkage
ratios to.
• Select a feature to add shrinkage
ratios to all of its dimensions.

Applying Shrinkage by Dimension 2
Figure 2 – Shrinkage Ratio Applied
to All Dimensions
Applying Shrinkage by Dimension

Applying Shrinkage by Dimension 1
Figure 1 – Model Before
Shrinkage Applied

Applying Shrinkage by Dimension 3
Figure 3 – Different Shrinkage
Ratios Applied to Specific
Dimensions
The Shrinkage by Dimension method enables you to set up one shrinkage
ratio for all model dimensions, and specify ratios for individual dimensions.
To apply shrinkage by dimension, you must specify the following items:
• Formula — Specify the formula you want to use to calculate shrinkage.
• Dimensions — Specify which dimensions to add shrinkage to.
• Shrinkage Ratio — Specifies the ratio of shrinkage you want to apply.
Within the Shrinkage By Dimension dialog box, a table displays the following
columns:
• Dimensions — Displays which dimensions have a shrinkage ratio applied.
The dimension symbol and original value are displayed in the cell.
• Ratio — Displays the shrinkage ratio for each dimension in the table.
• Final value — Displays the final dimension value once the shrinkage ratio
has been applied.
You can specify a shrinkage ratio for All Dimensions in the model. The
shrinkage ratio is in the first row of the Shrinkage Ratio table. In Figure 2, a
shrinkage ratio of 0.5 has been applied to all dimensions.
To add additional dimensions to the table, you can use the following methods:
• Insert Selected Dimensions
— Displays the dimensions for a
selected feature, enabling you to select and apply the desired shrinkage
ratio. In Figure 3, the 3 hole diameter dimension has had a shrinkage
ratio applied to it.
• Insert All Dimensions From Feature
— Enables you to select a
feature in the graphics window. All dimensions comprising that feature are
automatically added to the table. In Figure 3, all three dimensions of the
main extrude feature have had a shrinkage ratio applied.
• You can also click Add New Row and type the symbol for the dimension.
You can see what a given dimension’s symbol is by clicking Toggle
Dimensions
.
The following options are available when applying shrinkage by dimension:
• Change Dimensions of Design Part — Determines whether the shrinkage
feature is placed in the design model. Depending on the method of
reference model creation, this option may be grayed out. For example, if
the reference model was created using the Same Model, this option does
nothing, as the feature is created in the design model regardless.
Considerations when Applying Shrinkage by Dimension
When applying shrinkage by dimension, keep the following in mind:
• A negative shrinkage ratio shrinks the dimension, while a positive shrinkage
ratio expands it. For example, a positive 0.02 shrinkage ratio applied with
the 1+S formula expands all the model dimensions by 2 percent, while a
negative 0.02 shrinkage ratio shrinks all the model dimensions by 2 percent.
• If the part has had shrinkage applied, dimensions display in magenta when
viewed in the design model or a drawing, as shown in Figures 2 and 3.
• If the part has not had shrinkage applied, dimensions remain displayed in
black when viewed in the design model or a drawing.
• Shrinkage by dimension values is not cumulative. For example, if you
specify 1.5 as the All Dimensions shrinkage ratio for a model with 10 as the
value of all its dimensions, and then specify a separate shrinkage ratio of
2.0 for the length dimension, then the final length is 20 (i.e. 10*2.0), not
30 (i.e. (10*1.5)*2.0). Individual shrinkage values for dimensions always
supersede the overall model shrink value.
• The configuration file option, shrinkage_value_display, determines how
dimensions are displayed when shrinkage is applied to a model. The
possible values of this configuration option are percent_shrink and
final_value. For the procedure, the value for this configuration option is
percent_shrink.
• By default, whenever a part has shrinkage information associated with it,
the nominal dimension values are displayed, followed by the shrinkage
value in parentheses. If you set the value of the configuration file option
shrinkage_value_display to percent_shrink, shrinkage is represented as
percentage of the nominal dimension. You can display the final value of the
shrunken dimensions by changing the value of the configuration file option
shrinkage_value_display to final_value.

Leave a Reply

Your email address will not be published. Required fields are marked *