Retrieve model annotations in a drawing

What's New: 2023.2, 2027, 2027.2

You can retrieve 3D annotations from the model for a selected drawing view. The retrieve workflow for part views is slightly different from assembly views.

Part Views

Access

Ways to access the Retrieve Model Annotations are:

• While placing a base view, in the Drawing View dialog Recovery Options tab, select All Model Dimensions.
• With no view selected, right-click and select Retrieve Model Annotations in the marking menu.
• With a view selected, right-click and select Retrieve Model Annotations in the context menu.
• On the ribbon, click Annotate tab Retrieve panel Retrieve Model Annotations .
• On the Ribbon, Tools tab Applications Options Drawing tab. In the Defaults group, select Retrieve all model dimensions on view placement. Note, this does not retrieve 3D annotations.

While placing a base view

1. Click the Base View command.
2. Click the Recovery Options tab.
3. Select All Model Dimensions. Note, this does not access 3DA.
4. When all other options are satisfied, click OK. All model annotations populate the base view.

In the Ribbon

1. Click the Annotate tab and in the Retrieve panel click Retrieve Model Annotations.

2. In the Retrieve dialog, click Select View (lower left) if it is not active.

3. Select the drawing view that will have the retrieved model annotations. This is the Source model for the annotations being retrieved.

4. The Sketch and Feature Dimensions tab is selected. In the Select Source group, Select Features is selected by default. All available feature defining dimensions display.

   Note: To exclude dimensions already retrieved in other views, clear the Include dimensions already recovered check box. It is unselected by default.

5. To retrieve dimensions do one of the following:

   1. From the displayed dimensions, select the ones you want retrieved for the view.
   2. Click Apply to continue to use the Retrieve command to retrieve 3D annotations or work with another view.

6. To select 3D annotations do the following:

   1. Select the 3D Annotations tab, all available 3D annotations display.
   2. Click Select Source again. The dialog controls enable.
   3. In the dialog, for Design View, click the dropdown button and select the design view that has the annotation you want to display. The annotations preview.
   4. Under Annotation Filters, deselect any annotation types that are not needed in the view. They are removed from the display.
   5. Click Apply to continue to use the Retrieve command to retrieve more annotations or work with another view.
   6. Click OK to end the command.
   Note: To clear the selection and start anew, click Select Source twice.

   To select specific feature dimensions:

   1. In the Sketch and Feature Dimensions tab, click Select Source, the dimensions are hidden and the feature selector is active.
   2. In the view, select a feature to preview its dimensions.
   3. Click Select Source again and select the feature dimensions you want to retrieve for the view.
   4. Click Applyto continue to use the Retrieve command to retrieve 3D annotations or work with another view. Click OK to end the command.

Assembly Views

1. On the ribbon, click Annotate tab Retrieve panel Retrieve Model Annotations.

   Note: Alternatively, right-click the drawing view that will display the model annotations and select Retrieve Model Annotations...

   The Sketch and Feature Dimension tab is selected. In the Select Source group, Select Parts is selected by default. No dimensions preview.

2. Select View is active, click the drawing view that will have the retrieved annotations.

3. Choose either Select Features or Select Parts to display available annotations.

4. Click Select Source and select the part or feature to retrieve dimensions from and all applicable sketch, feature, and part dimensions preview.

5. Click Select Source again and begin selecting the dimensions you want retrieved.

6. When finished click Apply to retrieve the selected dimensions and continue using the Retrieve command to display 3D annotations in the same view or work with another view.

7. To retrieve specific feature dimensions, click Select Features, then Select Source .

8. In the view, select the feature to display its dimensions.

9. Click Select Source again and begin selecting the feature dimensions you want to retrieve.

10. Click Apply to end the selection, display the dimensions, and continue using the Retrieve command.

11. Click OK to end the command.

3D Annotations

1. If Select View is active, click the drawing view that will have the retrieved annotations.
2. Click the 3D Annotations tab.
3. Click Select Source and, in the view, select the component having the 3D annotations you want to display. Available annotations preview.
4. Click Select Source again and, if desired, use the Annotation Filters to adjust which annotations preview for selection. Select the 3D annotations you want displayed in the view.
5. Click Apply to retrieve the selected annotations and continue working with the command or Click OK to end the command. You can cancel at any time.

Automatically retrieve dimensions when you create views

1. Click File Options to access the Application Options dialog box.
2. On the Drawing tab, select the Retrieve all model dimensions on view placement option.

Exclude already-recovered dimensions

1. To exclude dimensions already displayed in other views, clear the Include dimensions already recovered check box. This is the default setting and prevents the same dimension from appearing in multiple drawing views unintentionally.
2. To include all available model dimensions regardless of whether they have already been recovered, select the Include dimensions already recovered check box.

Remove retrieved annotations from a view

1. Select each annotation to remove.
2. Press Delete or right-click, and then select Delete from the menu.

Add model dimensions to views containing derived part features

1. Right-click a view with a derived part, and select Retrieve Model Annotations....

2. On the Sketch and Feature Dimensions tab, Click Select Source, in the view, select the derived body.

3. Do one of the following:

   1. Click Select Feature and select the derived part feature having dimensions you want in the view.
   2. Click Select Parts and, in the view, select the derived part. The dimensions display.

4. Select the dimensions to keep in the drawing view. Selected dimensions are highlighted.

5. Click Apply to retrieve 3D annotations or OK to end the command.

6. Select the 3D Annotations tab.

7. Click Select Source and in the view select the derived part with the annotations you want to use in the view.

8. Click Select Source again and then select the annotations to display in the view.

9. Click Apply to continue working with the Retrieve command or OK to end the command.