Working with AutoCAD Layout View

In AutoCAD, you can treat your layout as a sheet of paper upon which you can arrange the parts of your drawing systematically, as well as add annotations and other details before creating the final output. It is always advisable to create your final print-ready drawings in a layout view. Using the layout view, you can arrange the parts of your drawing, such as the title block, the bill of materials (BOM), copyright information and annotations, easily and with the appropriate scale.

In this article, I will explain how to use the layout view in detail with a sample M10 metric nut and bolt drawing (see Figure 1). You can use your own example to follow along with the tutorial.

Figure 1. Sample nut and bolt drawing.

We will start by creating a plot-ready drawing in layout view with a detail view, a section view, dimensions, a title block and annotations.

Preparing the Layout View

To begin, open the 3D drawing in AutoCAD. Switch to layout view by clicking on the Layout1 button on the bottom-left side of the AutoCAD window. By default, you will see a layout view with a viewport. In this exercise, you will need to add your own layout before you can start adding details to it.

To add a layout, right-click on the Layout tab and select the From Template option from the contextual menu. A window will open with a list of all of the AutoCAD ready-made templates. Select the Tutorial-mMfg template (metric units) from the list and click on Open. A new ISO A1 layout template will open with a viewport shown in blue. Select the viewport and erase it. Now you have a layout view on A1-size paper; its boundaries will be 594 x 841 mm in landscape view with a title block and ruler.

Once again, right-click on the ISO A1 layout and select Drafting Standard Setup from the contextual menu. A new Drafting Standard window will open, from which you can choose your angle of projection for the drawing. In this example, Third Angle Projection has been chosen. Once you have made these changes, click on OK to close the Drafting Standard window and save your drawing.

To activate the ISO A1 layout, click on the Layout tab, then click on the From Model Space icon on the Base toolbar flyout of the Create View panel.

Figure 2. From Model Space option on the Base toolbar flyout.

You will notice that the front view of your drawing will follow the cursor. Click on a point in the layout to place this view and press the Enter key. Now you can generate the top, bottom, left, right and isometric views using this base view by clicking on the respective places in the drawing. Once you have all of your views in place, press the Enter key. The top, bottom and isometric views, along with the front view, have been created in Figure 3.

Figure 3. Front, top, bottom and isometric views of a nut and bolt drawing.

Creating the Sectional View

In order to show the cutaway or sectioned part of a geometric shape, you can use the sectional view tool. To create a sectional view, go to the Section toolbar flyout of the Create View panel and select Full from the menu. Click on the view from which you want to create your sectional view. In the example shown in Figure 3, the base view, which is in the center of the figure, has been selected. Specify a line indicating a sectional plane and click on a point in the drawing area to place the sectional view. Press the Enter key to create the final sectional view. Depending upon the initial scale of the drawing, your sectional view may or may not show proper hatch scale to indicate the sectioned part.

In order to properly adjust the scale of the sectioned hatch, select the hatches and change their scale from the Scale field on the Properties panel of the Drawing View Hatch Editor tab as shown in Figure 4.

Figure 4. Scale field in the Properties panel of the Drawing View Hatch Editor.

For this example, I have changed the hatch scale to 15 units, which makes the drawing look better and less crowded given the current layout scale.

Creating the Detail View

The parts of a drawing that are too small either for adding annotations or for viewing can be shown using a detail view. For example, in this drawing, there are threads that are too small to see or annotate. To view the thread profile and annotate it clearly, you can create its detail view. To create this view, select the Circular option from the Detail toolbar flyout of the Create View panel on the Layout tab.

Figure 5. Circular option of the Detail toolbar flyout.

Click on the existing drawing view that you want to use to create a detail view. In this example, I am selecting the base view. Use the cursor to create a circle that encloses all the portions of the drawing that you want to include in the detail view. Click on a point in the layout to place this view and press the Enter key.

Changing Visual Style and Scale

If you have followed all of the steps so far, you will notice that a single scale or visual style can’t represent a drawing clearly, so you will need to change the visual style and view scale as required. The detail view in this example has a scale of 8:1, which is not very large for practical use, so you would need to modify its current scale to make it more useful. In order to change the scale of your drawing, select the view. You will see a new Drawing View tab. Select the Edit View option from this tab and change the scale in the Scale drop-down menu of the Appearance panel on the Detail View Editor tab. For example, changing the scale to 10:1 will make the detail view 10 times larger than the original view.

In some cases, you may not find your required scale in the drop-down menu. For such cases, you can change the scale from the command line as well. To change the scale from the command line, click on the Scale option on the command line and enter a scale in your drawing. Press the Enter key twice to accept the changes and exit the Edit View tab.

Figure 6. Scale option on the command line in the VIEWEDIT command.

You can also change the visual style of the drawing view. To change the visual style, select the view, then click on the Edit View option as you did when you changed the scale earlier. In the Appearance panel of the Drawing View Editor tab, change the view to “Shaded with visible lines” in the Visual Style toolbar flyout as shown in Figure 7. Similarly, you can change the visual style of the detail view to “Visible lines” to hide hidden parts of the geometry.

Figure 7. Changing the visual style from the Visual Style toolbar flyout.

After making all of these changes, this is how the example drawing looked:

Figure 8. Views created after changing scale and visual styles of selected views.

Adding Text and Annotations

In the examples above, there are some text entities that are added by default in the drawing, such as the scale of the detail view and section geometry callouts. The text in both of these cases is very small, making it hard to see on the current A1 paper size.

To adjust the text size, type SCALETEXT into the command line and press the Enter key. Select Text Entities from the layout view for which you want to increase the text size and press the Enter key again. Press the Enter key to keep the default justification of text and then enter the scale in the next prompt. In this example, I have used a text scale of 5. Press the Enter key again to exit the SCALETEXT command.

Now you can add dimensions to different parts of your drawing directly in the layout view. One of the benefits of adding dimensions in the layout view is that the dimensions associated with the geometry are maintained. In simple terms, if you change the size of the geometry in the model space, then its corresponding paper space dimension will automatically change. After adding dimensions and other annotations, the final layout view is shown in Figure 9.

Figure 9. Final print-ready layout view.

Do you have any questions related to this article? Let us know in the comments below.