Model Based Definition (MBD)

El cuadro de diálogo contextual Cotas se utiliza para editar las cotas de boceto y operaciones, así como para añadir tolerancias. Al hacer doble clic en una cota de un boceto o en una cota MBD del área gráfica, se accede a este cuadro de diálogo. Consulte Edición de cotas MBD.

• Haga clic en el ícono de tolerancia () para añadir una tolerancia a la cota.

• Una vez establecida la tolerancia, haga clic en la flecha desplegable () para definir los parámetros de tolerancia:

  

  • Precisión: utilice el menú desplegable para seleccionar la precisión de una unidad, ya sea Precisión del área de trabajo u otro valor de precisión de la lista desplegable. Introduzca de 0 a 6 decimales.

    

  • Tipo de tolerancia: seleccione un tipo de tolerancia de la lista desplegable. Las opciones son Por defecto, Sin tolerancia, Simétrica, Desviación, Límites, Mínimo, Máximo y Básico.

    Las tolerancias de diámetro de taladro y boceto también ofrecen las opciones Ajuste, Ajustar con tolerancia y Ajustar (solo tolerancia). Consulte la operación Taladro para obtener más información.

    With Default selected, tolerances are based on Default tolerances. See Onshape default tolerances library and Default tolerances library for further information.

    

    • Desviación: disponible para el tipo de tolerancia Simétrico. Introduzca un valor de desviación.

    • Superior: disponible para los tipos de tolerancia Desviación y Límite. Introduzca el valor de tolerancia superior.

    • Inferior: disponible para los tipos de tolerancia Desviación y Límite. Introduzca el valor de tolerancia inferior.

    • Estándar: disponible para el tipo tolerancia Ajuste, Ajustar con tolerancia y Ajustar (solo tolerancia). Seleccione la norma ANSI o ISO en la lista desplegable.

    • Tipo de ajuste: disponible para el tipo tolerancia Ajuste, Ajustar con tolerancia y Ajustar (solo tolerancia). Seleccione Definido por el usuario, Holgura, Transición o Interferencia de la lista desplegable.
    • Clase de taladro: disponible para los tipos de tolerancia Ajuste, Ajustar con tolerancia y Ajustar (solo tolerancia). Seleccione una opción Clase de taladro de la lista desplegable.
    • Clase de eje: disponible para los tipos de tolerancia Ajuste, Ajustar con tolerancia y Ajustar (solo tolerancia) cuando se selecciona la norma ISO. Seleccione una clase de eje de la lista desplegable.

• Haga clic en el ícono de marca de verificación () para aceptar los valores introducidos en el cuadro de diálogo contextual.

• Haga clic en el ícono x () para salir del cuadro de diálogo contextual sin ningún cambio.

• Haga clic y arrastre junto al controlador del cuadro de diálogo () para moverlo a una nueva ubicación en la pantalla. Suelte el mouse para colocarlo en su nueva ubicación.

Las siguientes cotas de boceto pueden utilizar tolerancias:

• Distancia entre dos líneas

• Distancia entre dos puntos

• Distancia entre la geometría de boceto y el plano

• Distancia diagonal

• Diámetro

• Ángulo

• Distancia directa

• Distancia lineal

• Radio

Las siguientes cotas de boceto no pueden utilizar tolerancias:

• Distancia de línea única

• Longitud de arco

• Cotas de la línea central

Consulte Cotas de herramienta de boceto para obtener más información.

1. Dibuje la entidad de boceto e introduzca cualquier valor en las entradas de valores sobre la marcha.

2. Haga doble clic en la cota (primera imagen de abajo). Se abre el cuadro de diálogo contextual Cota (segunda imagen de abajo):

   

3. To add a tolerance to the dimension, click the Tolerance options icon (; first image below), and then click the dropdown arrow (; second image below):

   

4. Introduzca los valores de Precisión y Tipo de tolerancia, con los valores especificados:

   

5. Haga clic en la marca de verificación () para aceptar la nueva cota de boceto.

   

Las siguientes opciones de operación pueden usar tolerancias:

• Extrusión

  • Sólido/Superficie/Delgado - Profundidad

  • Sólido/Superficie/Delgado - Distancia de equidistancia

  • Sólido/Superficie/Delgado - Segunda posición final - Distancia de equidistancia

  • Delgado - Espesor 1

  • Delgado - Espesor 2

  • Delgado - Plano medio - Espesor

• Hacer revolución

  • Sólido/Superficie/Delgado - Una dirección/Simétrico/Dos direcciones - Ángulo de revolución

  • Delgado - Espesor 1

  • Delgado - Espesor 2

  • Delgado - Plano medio - Espesor

• Redondeo

  • Radio

• Chaflán

  • Distancia (Distancia igual)

  • Distancia 1, Distancia 2 (Dos distancias)

  • Distancia y ángulo (Distancia, Ángulo)

• Taladro

  • Diámetro (Simple/Escariado/Avellanado)

  • Distancia (Profundidad: Simple/Escariado/Avellanado)

  • Diameter (Counterbore/Countersink diameter)

  • Distancia (Profundidad de escariado)

  • Ángulo (Ángulo de avellanado)

  • Distance (Tapped depth)

  • Distance (Tap drill diameter)

1. Cree una operación que acepte una tolerancia (Extrusión en este ejemplo).

2. Haga clic en el ícono de opciones de tolerancia () situado a la derecha del parámetro:

   

3. Click the dropdown arrow () to the left of the parameter:

   

4. Introduzca los valores de Precisión y Tipo de tolerancia, con los valores especificados:

   

5. Enter any other Feature settings and click the checkmark () to accept the Feature.

6. Asegúrese de que la Tabla de inspección () esté abierta para ver el valor de cota de la operación con la tolerancia:

   

La eliminación de la tolerancia de una operación no elimina la cota del modelo, ya que sigue siendo una cota válida.

Tolerance options can be used in conjunction with configurations.

1. Click the Tolerance options icon () to make the configuration's option value tolerant:

   

2. Click the dropdown arrow icon () to the left of the parameter in order to set the tolerance Precision and Type.

   

See Configurations for more information.

Tolerance options are automatically used in conjunction with the Compare mechanism. When comparing 2 history entries, select the Feature to compare (Extrude 1 in the example below). Comparisons between differing Tolerance options in the entries are outlined in yellow:

Extrude: Depth tolerance options compared between two history entries

See Compare for more information.

Images below are from iOS. The workflow is the same for both iOS and Android.

Sketch dimension tolerances:

1. Double-tap the dimension on-screen.

2. Click on the Tolerance options button at the lower right corner of the Android Dimension context dialog to set the dimension as tolerant:

   

3. In the Tolerance options dialog, enter the Precision and/or Tolerance type and click the checkmark to accept the options:

   

Feature dimension tolerance:

Feature dimensions can be set and edited in the same way as on the desktop platform:

Tolerance options for the Extrude: Depth value

Tolerances can only be viewed on the desktop platform, not Android, since the Inspection table is available only on desktop.

Currently on iOS and Android you cannot set a tolerance Precision and Type for a Hole feature's Depth parameter if its Termination is Up to Entity or Up to next. Additionally, on iOS you cannot set a tolerance Precision and Type for a Hole feature's Diameter parameter. Use a Desktop platform or Android device (in the case of Diameter) to set tolerances for these parameters.

1. Open the Inspection panel () to display the MBD dimensions in the graphics areas (left image below).

2. Double-click on the driving dimension that is associated with a sketch (right image below):

   

   The Dimension context dialog opens with context placed on the dimension value. Simultaneously, the Sketch dialog opens:

   

3. Using the keyboard, enter a numeric value or use the up/down arrows to increment the value in the Dimension context dialog. As this value is adjusted, the sketch is updated dynamically.

   If entering a value numerically, press the tab key to see the sketch value update.

   

4. Press Enter on the keyboard or click the checkmark () in the Dimension context dialog to close this dialog:

   

5. Press the checkmark () in the Sketch dialog to accept the new sketch value.

   

   The edited sketch dimension that adjusts the model's dimension

1. Open the Inspection panel () to display the MBD dimensions in the graphics areas (left image below).

2. Double-click on the driving dimension that is associated with a feature (right image below):

   

   The Dimension context dialog opens with context placed on the dimension value. Simultaneously, the associated Feature dialog opens (Extrude in this example):

   

3. Using the keyboard, enter a numeric value or use the up/down arrows to increment the value in the Dimension context dialog. As this value is adjusted, both the model and the value in the Feature dialog are updated dynamically.

   If entering a value numerically, press the tab key to see the value update in the Feature dialog.

   

4. Press Enter on the keyboard or click the checkmark () in the Dimension context dialog to close this dialog:

   

5. Press Enter on the keyboard again or click the Feature dialog checkmark () to close this dialog:

   

   The edited feature dimension that adjusts the model's dimension

To delete an annotation:

1. Select the annotation in the graphics area:

   

2. Press the Delete key.

3. The annotation is deleted from the graphics area and Inspection table.

   If the annotation is a sketch or feature dimension:

   1. The dimension's Tolerance options values are deleted.

   2. The Tolerance options icon () is deselected.

   3. The dimension value in the sketch or Feature dialog is not deleted.

Annotations cannot be deleted if:

• The annotation is derived.

• The annotation is created in a custom feature where the parameter is made tolerant but the tolerant toggle is not made available for user input.

In either case the following message is displayed:

• Driven dimensions cannot be edited. Double-clicking on a driven dimension opens the Dimension context dialog, but values in the dialog cannot be edited.

• Derived dimensions cannot be edited. Double-clicking on a driving or driven dimension from a derived part does not open the Dimension context dialog.

• To cancel out of the Dimension context dialog, press the Esc key. If editing a feature dimension, the Dimension context dialog and Feature dialog close simultaneously. If editing a sketch dimension, only the Dimension context dialog closes. The sketch dialog must be manually closed (clicking the x icon).

• Alternatively, with both the Feature dialog and Dimension context dialog open, the value in the Feature dialog can be selected and edited, which updates both the Dimension context dialog and model dynamically. Once edited here, pressing Enter closes both the Feature dialog and the Dimension context dialog simultaneously.

• The location of the model dimension and location of its corresponding sketch dimension are not locked together. They are independent:

  

  The model's width dimension is located below the model (left) but above the sketch (right)

• In Pause regeneration mode, the model's dimension cannot be edited or deleted. However, you can still edit the feature or toggle a dimension's tolerance on or off. Changes take effect after clicking the Regenerate features and exit checkmark on the Paused regeneration banner.

• Configurations work as expected. However, the dimension in the Dimension context dialog is not surrounded by a dashed orange outline to indicate it is configured. Configured sketch dimensions cannot be edited.

Depth dimension:

Offset distance dimension (with a composite part):

Thin extrude (Thickness 1 and Depth dimensions):

Revolve (Revolve angle dimension):

Revolve (Thickness 1 and Revolve angle dimensions):

Fillet (Radius dimension):

Since default tolerances always use linear or angular dimensions, adding a dimension using the Inspection panel's Dimension tool () with a Default tolerance type always generates a linear or angular tolerance value, even if the face is a fillet. For this reason, it is recommended to apply fillet tolerances from the feature dialog, and not from the Inspection panel.

Dimensioning a fillet face: From the Fillet feature dialog (driving) and from the Inspection panel (driven)

A Chamfer is defined as a distance to angle or distance to distance between a face and an edge. The Chamfer width dimensions are specified as the distance from an edge to the virtual sharp. The display for virtual sharps is added to the dimensioned edge, including a dashed curve.

• Tolerances are not disabled When a tangent measurement is used, since they can work in certain cases, and especially when accounting for the specified tolerance.

• In situations where two chamfer measurements are used (Two distances or Distance and angle), the user does not have to create tolerances for both. Tolerances can be added to only one parameter, if required.

Equal distance Chamfer type displays 2 Distance tolerance values, which are reflected in the table, even though there is only one distance tolerance option in the dialog:

Two distances example:

Distance and angle example:

For cases where the chamfer results in a variable distance (for example, if the chamfer is applied to a cylinder face that is perpendicularly connected to another cylinder), try selecting tangent for the Measurement, to make the distance uniform along the edge:

Non-uniform chamfer using an Offset measurement displaying a Nominal value error.

Uniform chamfer using a Tangent measurement results in a Nominal value without error.

If a tolerance is placed on a hole feature, it can be displayed in the Inspection table.

Some things to keep in mind:

• Hole dimensions are only visible as rows in the Inspection table. There are no dimensions placed in the graphics area. This is done so as not to clutter the graphics area with callouts.

• Before hole dimensions are visible in the Inspection table, another callout (a datum, for example) must be placed on the part.

• Only one set of dimensions (Diameter, Distance, and/or Angle) are shown per hole feature. Patterned holes or additional holes in the same feature are not dimensioned separately.

• The custom Tip angle dimension is not currently supported and does not create a row in the Inspection table.

• Cross-highlighting works as follows:

  • Distance (Depth) is not cross-highlighted because there are no faces at either end of the hole, and edges are not currently supported for MBD.

  • Diameter, Distance (Counterbore depth), and Angle (Countersink angle) cross-highlights a single face.

Hole dimensions are visible in the Inspection table after a Datum is added to one of the part's faces.

Axis distance dimensions between center circles:

Thickness is displayed in the Inspection table as a Distance row.

Thin extrude (Thickness 1 dimension):

Thin revolve (Thickness 1 dimension):