Creating 2D Views From 3D Models in AutoCAD, Part 2

Section views and model documentation are a breeze if you start with AutoCAD solid models.

We continue here with making 2D view from 3D models after
part 1 of this 2-part series.

Using AutoCAD’s Section Plane, you can section 3D models by a user-defined cutting plane. This works with solids, surfaces, meshes, regions and point clouds.

You have multiple options for setting the sectioning object’s location and orientation.

Select a Face—AutoCAD aligns the section plane to the plane of the selected face.

Draw section—you define the section by selecting multiple points building a section line with jogs.

Orthographic—to align the section object to an orthographic orientation relative to the UCS. Use the View Cube as a reference.

After creating the sectioning object, you can adjust its position by moving it with the Move Gizmo that appears after you select it. Use the direction grip to flip the sectioned part. Find Rotate in the right-click menu.

With the sectioning object in location and orientated correctly, use Generate Section to create a block of the sectioned geometry.

In the dialog, select 2D Section/Elevation to create a 2D representation of the sectioned geometry. You can either include all visible objects or select the objects for inclusion.

As with Flatshot, you insert the results for a block or export to a new drawing.

Use Section Settings to control the display of the sectioning object and the geometry created by the Generate Section feature. This includes the intersection boundary (outline), hatching for cut objects, background objects and tangency lines.

Model Documentation

Use the model documentation features of AutoCAD to create 2D drawings from 3D models. This is the same as you would find in 3D modeling applications like Autodesk Inventor and Fusion 360.

Like with SOLVIEW, the first view you place is the base view. You can initiate VIEWBASE from model space or a paper space layout. The first step is setting the source—either objects from Model Space or a selected Inventor File. If you started from model space, you then need to set the destination layout. Finish the process by selecting the insertion point.

As a bonus, you can create associative 2D views from linked Autodesk Inventor models. If the Inventor model changes, the views in AutoCAD update to match the changes. This means you can design in Inventor but document the design in AutoCAD.

When selecting objects from model space, consider using the right-click Entire Model option to select all visible objects.

Prior to picking the view’s location, use the command line (or right-click menu) options to reselect the objects and to adjust the view’s orientation and scale. By default, AutoCAD uses the front view. But you can change this to any of the predefined views or to the current model space orientation.

You cannot edit the view’s geometry—what you see is what you get. This is because it stays associative to the 3D model. If the model changes, the views update automatically. However, AutoCAD places the objects on a predefined set of layers, meaning you can change properties by changing the layers.

Although the view border is visible, it does not print, regardless of the layer it is on. With the view border selected, use the square grip to reposition the view on the sheet and the triangular grip to adjust the scale.

If you are using AutoCAD Mechanical, you can make further changes to the view from the contextual Drawing View ribbon tab. If you are using vanilla AutoCAD or one of the nonmechanical flavors, you need to use the right-click menu options.

Start with Edit View.

While editing the view, you can use Model Space Selection to switch into model space and adjust the objects selected for the view. Use the Scale Drop-down to adjust the view scale.

The view is in one of four display styles: Visible Lines, Visible and Hidden Lines, Shaded with Visible Lines and Shaded with Visible and Hidden Lines.

Use Edge Visibility options to manage the visibility of interference and tangent lines. Interference edges occur when solids intersect with each other. Technically, there is not an edge, although our eyes perceive one.

From the base view, create projected views from it. The projected views derive from the base view, not the 3D model. The command is VIEWPROJ. Alternatively, you can select the base view and start Projected from the ribbon or right-click menu.

The projection type depends on the position of the view. You can create both orthographic and isometric views from a base view. The command stays active until you exit it, meaning you can place multiple views.

By default, the projected views inherit the settings (including the scale) from the base view and update if you change the base view settings. If needed, you can override the settings.

With the views created, add notes, dimensions and other annotations. AutoCAD does its best to update the associative dimensions and annotations with changes to the model.

You can move isometric views anywhere on the layout. When you move an orthogonal projected view, it stays aligned to its parent view.

Press Shift to break the alignment and place the view anywhere on the layout. You can also use Shift to restore the alignment with the parent.

You can create section views and detail views from any existing drawing view, whether base or projected.

Section views are created like projected views with the extra step of defining the section line.

After creating the view, add constraints to keep the section line constrained to the view geometry. Then if the model changes, the section line (and view) will update to match.

Create section views of several types. The default Full section cuts completely through the objects, revealing all internal features and details. With Half sections, the cutting plane passes halfway through the objects, leaving one-half in an orthographic view and the other half sectioned. Use Aligned to align the view perpendicular to the first or last section line.

In addition to the settings found on projected views, you can also change the section depth, toggle the display of the hatching and adjust the section label identifier.

The section depth sets the depth of the section view. The default Full section cuts completely through the model. A Slice is a paper-thin cut that removes all geometry beyond the section line. Use Distance to set the depth of the section.

A Detail view is a view magnifying a selected part of the view. Create the view with a circular or rectangular shape. Regardless of the shape, the first step is to pick the center point and then sett the size of the boundary. Details views can be placed anywhere on the layout and are not constrained by the parent.

With detail views, you can change the model edge. The model edge is the edges of the detail view, where its boundary intersects with the parent view. It visually separates the magnified part of the view.

AutoCAD supplies different model edge appearances. The default Smooth creates a continuous shape around the detail view, typically as a collection of arcs and splines. Smooth with Border is like Smooth but it inserts a circular or rectangular border around the detail view matching the boundary. Use Smooth with Border and Connection Line to include a line connecting the detail view to the boundary in the parent view. Finally, Jagged displays the model edges that have jagged lines without a border.

As with section views, consider adding constraints to keep the detail view constrained to the parent view.

As you can see, AutoCAD provides multiple methods of creating 2D views from 3D objects, even if the 3D objects did not originate in AutoCAD. Creating 2D views is useful when you need to create documentation of the 3D model and use AutoCAD’s strengths to detail and annotate the design. 2D views can also provide a simpler view, making it easier to understand the design.