- tol_display Set
the tolerance display on and off
- tol_mode Set the default display for dimension
tolerances Set Datums
- maintain_limit_to_nominal Maintains the nominal
value of a dimension regardless of the changes that you make to the tolerance
values. If you set it to "yes", the system does not modify the Nominal
Value of a dimension with a Limits tolerance format when you set
the format to Limits or change the value of the upper or lower tolerance.
- Before you can create dimensional tolerances you have
to load the tolerance tables in the model. Set the tolerance standard
to ISO/DIN and retrieve the tolerance tables you need.
TIP: Retrieve often used tolerance tables
in the start part.
Geometric tolerances can be created in
Part, Assembly, and Drawing modes. To create them in Part and Assembly modes,
select Setup, Geom Tol, Specify Tol. To create them in Drawing mode, select
Create, Geom Tol, Specify Tol. In either case, the Geometric Tolerance dialog
box will appear as shown in Figure 1.
Once the Geometric Tolerance dialog box
appears, the procedures for creating a geometric tolerance are the same in Part,
Assembly, and Drawing modes. The procedures are as follows:
- Select the type of geometric tolerance to be placed.
The possible types are graphically shown on the left hand side of the Geometric
Tolerance dialog box, as shown Figure 1. In this example, the position tolerance
type has been selected.
- Select the model to be toleranced. The model may be
selected from either the Model drop down list or by selecting Select Model...
and picking the model from the screen. In Drawing mode, the list of available
models will include all the models currently in the drawing as well as the
drawing itself. For assemblies, the list of models will include the assembly
as well as the components that make up the assembly. For parts, only the part
can be selected as the model.
- The next step is to assign datum references to the
geometric tolerance. Select the Datum Refs tab from along the top of the Geometric
Tolerance dialog box and choose the datums for the primary, secondary and
tertiary references. For each reference, the material condition may also be
set. In this example, the primary datum is being set as datum "A" with a maximum
material condition (MMC) as shown in Figure 2. The secondary datum is being
set as a compound datum "B-C" with an RFS(No Symbol) material condition as
shown in Figure 3. For position and surface profile geometric tolerances,
a Composite Tolerance can be set with or without a datum reference. Figure
4 shows the composite tolerance being set with a value of 0.005 and the primary
datum (datum "A") being selected as the reference.
In order for datum planes or axes to
be selectable for use as datum references, they must have previously been
set using the Set Datum option from the GEOM TOL menu.
- The next step is to set the tolerance value for the
geometric tolerance. Select the Tol Value tab from along the top of the Geometric
Tolerance dialog box and set the Overall Tolerance as desired. The Material
Condition for the overall tolerance can also be specified. In this example,
the tolerance is being set to 0.020 at MMC, as seen in Figure 5. For straightness,
flatness, perpendicularity, and parallelism, a Per Unit Tolerance may be set.
In this example, a Per Unit Tolerance is not applicable.
- The next step is to set the Symbols, Modifiers and
a Projected Tolerance Zone. Select the Symbols tab from along the top of the
Geometric Tolerance dialog box. The options Statistical Tolerance, Diameter
Symbol, Free State, All Around Symbol, and Tangent Plane symbols may be selected
depending on the type of geometric tolerance being placed. A Profile Boundary
or a Projected Tolerance Zone may need to be established depending on the
tolerance being set. Select any desired Symbols, Modifiers, Projected Tolerance
Zone, or Profile Boundary. In this example, a Projected Tolerance Zone will
be placed below the geometric tolerance with no specified Zone Height. If
a specified Zone Height is desired, select the Zone Height option and enter
the desired height in the input field.
- The Reference Entity should then be set by first selecting
from the Type drop down list in the Model Refs portion of the dialog box and
selecting one of the available options. Once the desired Reference Entity
type is selected (i.e.. Edge, Surface, etc.), the Select Entity... option
will become depressed and the Reference Entity should be selected on the screen.
- With the geometric tolerance now fully defined, place
the geometric tolerance as desired by selecting the Placement Type from the
drop down list. The possible placement options will vary depending on the
type of geometric tolerance being placed. The list of possible options are,
Dimension, Free Note, Leaders, Tangent Ldr, Normal Ldr, and Other Gtol. For
this example, the geometric tolerance has been placed as a Free Note. The
Place Gtol... option will become depressed after selecting the Placement type.
Continue placing the geometric tolerance.
If the geometric tolerance is placed,
it does not mean that the definition of the geometric tolerance is complete.
The geometric tolerance can be placed
and actively changed until it is set. Figure 7 shows the geometric tolerance
created in this example.
8.After the geometric tolerance is placed,
there are other options:
- Select New Gtol to create a new geometric tolerance.
- Select Cancel to quit the creation of the current
geometric tolerance and exit the dialog box.
- Select OK to accept the current geometric tolerance
and exit the dialog box.
Modifying Geometric Tolerances
The modification of geometric tolerances
can be performed in Part, Assembly, or Drawing modes by selecting Modify, Geom
Tol. Once a geometric tolerance is chosen, the Geometric Tolerance dialog box
will appear with options to change the geometric tolerance type, datum references,
tolerance values, and symbols. None of the settings under Model Refs may be
modified (which include the Model, Reference Entity, and Placement values).
Also, note that if the Type of geometric tolerance is changed, datum reference
information will be removed from the existing geometric tolerance or the settings
under Datum Refs will become unavailable, depending on what information is proper
for that particular type of geometric tolerance.
1. Figure 1 displays a drawing view with a geometric
tolerance. To change any of the values of this geometric tolerance, select Modify,
GeomTol and choose the geometric tolerance.
- 2.The dialog box appears and by default, the settings
for Tol Value are available for modification. Values for Overall Tolerance
and Material Condition can be changed, as displayed in Figure 2. Notice that
any modifications made in the dialog box automatically update the model and/or
3.Modify the datum references, material
conditions, and compound/composite tolerance information by selecting Datum
Refs from the Geometric Tolerance dialog box, as seen in Figure 3.
4.Make any changes necessary with respect
to symbols, modifiers, and projected tolerance zone information by selecting
Symbols, as shown in Figure 4.
5.Once all of the desired changes are
made, select OK from the Geometric Tolerance dialog box. The modifications made
in the previous steps to the original geometric tolerance are displayed in Figure