Autodesk Fusion 360: Drawings - Skippy's Random Ramblings

Autodesk Fusion 360: DrawingsOverviewThis drawings functionality allows you to create 2D drawings from your Fusion 360 designs and supportscore drawing tools, which give the ability to generate PDF and DWG documentation of your Fusion 360model. When you create a drawing, it is created as a derived document of a Fusion 360 model, and itshows up in the Data Panel as a unique derived item in the active project.Launch VideoLearning Objectives About Fusion 360 Drawings Create a Drawing of a model Create Views Create & Edit Annotations Drawing Settings and Preferences Output the DrawingIntroduction to Drawing ViewsA drawing view is an object that contains a 2D projection of a 3D model.When you create a drawing from the Fusion 360 modeling environment, the system automaticallylaunches a new tab of the Drawing workspace and generates a 2D projection of the components youselect. The drawing view generated is referred to as a base view. Once you place the base view in thedrawing, you can generate orthogonal and isometric projected views from it.Projected views inherit the properties of the base view by default. When you change the properties ofthe base view, the projected view properties also change. However if you override a property of aprojected view, that property stops following the changes you make to the base view.Note: When creating a drawing, the system picks up settings such as the projection angle, annotationformat, and the drawing border and title block from Preferences.1

Autodesk Fusion 360: DrawingsCreate a Drawing: In this section you will open the design file for the Utility Knife and learn how tocreate a new drawing of the assembly.Step 1 – Open the Data PanelIn this module we will be using the 08 DrawingsUtility Knife file to complete the exercise. If youhaven’t set up a new project and uploaded thenecessary designs, please follow the steps in theIntroduction module.1. Click on the icon in the upper left to openthe Data Panel.2. The Data Panel will slide openStep 2 – Open the design1. At the top left of the Data Panel, select theproject where you uploaded 08 DrawingsUtility Knife.2. Double-click on the design called08 Drawings Utility Knife to open thedesign in Fusion 360.3. When the design has opened in yourmodeling window, click on the ‘x’ icon toclose the Data Panel.Step 3 – Initiate a new Drawing1. Click on the File dropdown menu from thetop menu bar.2. Select New Drawing from Design from thefile menu dropdown.2

Autodesk Fusion 360: DrawingsStep 4 – Choose Assembly1. Select Full Assembly from the dialog andclick OK to initiate the drawing.2. Notice that a new tab is automaticallygenerated in Fusion 360 of the Drawingworkspace.Note: If you un-check “Full Assembly” from theNew Drawing dialog, you have additional controlsto pick any set of components to create a drawingfrom if the full assembly is not what you arelooking to document.Step 4 – Commit a Base View1. Move your cursor around the screen andsee the Base View preview is attached tothe cursor.2. Click on the top left quadrant of the sheetto place the view3. Click OK to commit the view.Note: Notice that after the view is committed, theshaded preview matures into a 2D line drawing ofthe view.About Projected Views & View OptionsProjected views maintain a parent-child relationship with the base view it was generated from. Theyinherit their properties from the parent base view. If necessary, you can override them after you createthe projected view.The projection angle defines the method employed to generate projected views.3

Autodesk Fusion 360: DrawingsFirst Angle ProjectionWhen you use first angle projection, projected views placed to the right of a base view depict theappearance when viewing it from the left. Projected views placed below the base view depict theappearance from above. The ISO drafting standard specifies that drawings use first angle projection.Third Angle ProjectionWhen you use third angle projection, projected views placed to the right of a base view depict theappearance when viewing it from the right. Projected views placed below the base view depict theappearance from below. The ANSI drafting standard specifies that drawings use third angle projection.4

Autodesk Fusion 360: DrawingsFinish the layout: Now that you have created a Base View of the model assembly, you will learn tocreate projected views and edit their properties to create a complete drawing layout.Step 1 – Initiate the Projected Viewcommand1. Click Views Projected View.2. Select the existing Base View asthe parent view that theprojected views will be createdfrom and associated to.Step 2 – Place the views1. Drag the cursor to the right ofthe base view, and notice thatthe projected view is previewedbased on this alignment.2. Select to the right of theexisting base view to place aprojected view.3. Select to the bottom of theexisting base view to place asecond projected view.4. Press Enter to finish the taskNote: Projected views inherit all itsproperties from the parent. When theproperties of the parent view change,the corresponding properties on theprojected view also change.Step 3 – Move the right view1. Click anywhere inside theselection boundary of the rightprojected view to activate it.2. Click the center grip to drag theview.3. Move the view to a newlocation at the far right of thelayout.5

Autodesk Fusion 360: DrawingsStep 4 – Move the bottom view1. Click anywhere inside theselection boundary of thebottom projected view toactivate it.2. Click the center grip to drag theview.3. Move the view to a newlocation at the left bottom ofthe layout.6

Autodesk Fusion 360: DrawingsStep 5 – Create an isometric base view1. Click Views Base View.2. Click to place the view in thecenter of the sheet layout.3. Set the Orientation to NEIsometric.4. Click OK to commit the viewView PropertiesHidden Lines – Select On or Off from the drop-down list to display hidden lines within the selected baseview. The Hidden-line representation suppresses or exposes lines, edges and other objects that arelocated behind other three-dimensional objects. This view property can be particularly helpful whentrying to visually communicate the inner workings or dimensions of a complex assembly or part.Hidden Lines OFF7Hidden Lines ON

Autodesk Fusion 360: DrawingsTangent Edges – Select Full length, Shortened or Off from the drop-down list to display Tangent edgeswithin the selected base view. Tangent edges mark the transition between a flat surface and a roundededge, most commonly seen as filleted edges. Tangent edges can be set to Full Length, Shortened, or Off.Tangent Edges OffTangent Edges ShortenedTangent Edges Full LengthInterference Edges – Select On or Off from the drop-down list to display of Interference edges withinthe selected base view. An interference edge occurs when two faces of two componentsintersect. When Interference Edges are turned on, an edge is displayed that shows where the twocomponents meet. When selected, associated drawing views are to display both hidden and visibleedges that were previously excluded due to an interference condition (press, or interference fitconditions, threaded fasteners in tapped holes where the hole feature is modeled with the minordiameter).Interference Edges OffInterference Edges ONEdit the layout views: Now that you have created a base view and several projected views of the modelassembly, you will practice using the View Properties settings to further customize the view layouts.8

Autodesk Fusion 360: DrawingsStep 1 – Edit the isometric base view1. Double-click anywhere insidethe selection boundary of theisometric view to activate it.2. Select the Scale ratio in theView Properties dialog box tochange the scale.3. Change the Scale to: 1:14. Click OK to accept the drawingview changes.If the projected view properties arechanged, they no longer inherit thesettings of the base view.Step 2 – Edit the right projected view1. Double-click anywhere insidethe selection boundary of theright projected view to activateit.2. In the View Properties dialogbox, click Hidden Lines andselect On.3. Click Close to accept thedrawing view changes.When the projected view properties arechanged, they no longer inherit thesettings of the base view.Step 3 – Edit the bottom projected view1. Double-click anywhere insidethe selection boundary of thebottom projected view toactivate it.2. In the View Properties dialogbox, change Tangent Edges toFull Length.3. Click Close to accept thedrawing view changes.9

Autodesk Fusion 360: DrawingsBy now, your drawing should look something like this:Text and AnnotationsAt any point in the drawing creation, you can add a variety of text and annotations to the drawing andthe views to document additional detailed information. The tools for adding annotation and text to adrawing include:Dimension: LinearCreates a horizontal or vertical dimension.Dimension: AlignedCreates a linear dimension that is aligned with the origin points of the extension lines.Dimension: AngularMeasures the angle between selected geometric objects or 3 points.10

Autodesk Fusion 360: DrawingsDimension: DiameterCreates a diameter dimension for a circle or an arc.Dimension: RadiusCreates a radius dimension for a circle or an arc.TextCreates single and multi-line text.LeaderCreates a leader note.Text and Leader Notes: In this section you will learn how to create, reposition and edit text and leadernotes in the drawing.Step 1 – Create Text1. Click Annotation Text.2. Select two corners below theIsometric Base View to create a textbox.3. Type the following text into the textbox: NE Isometric View4. Select anywhere outside of the textbox to commit the action.5. Repeat process to add text belowthe to the initial base view with thetext: Front View6. Repeat process to add text belowthe right projected view with thetext: Right View7. Repeat process to add text belowthe bottom projected view with thetext: Bottom View11

Autodesk Fusion 360: DrawingsStep 2 – Create Leader Notes1. Click Annotation Leader.2. Click near the blade of the bottomview to place the start of the leader.3. Click outside the view to place theend of the leader.4. Type the following text: Steel blade5. Select anywhere outside of the textbox to commit the action.Step 3 – Reposition Leader Notes1. Click on the leader note to activate.2. Drag the leader note using the textgrip to the left so that the leader isat a 90 degree elbow.3. Press the Esc key to commit thechanges and exit the command.Step 4 – Edit Text1. Double-click on the leader note toactivate the text editor.2. Drag the to the right to formatthe text into 2 lines.3. Select anywhere outside of the textbox to commit the action.Dimensions: In this section you will learn how to create, reposition and edit a variety of dimension typesin the drawing.12

Autodesk Fusion 360: DrawingsStep 1 – Create linear dimensions1. Click Annotation LinearDimension.2. Click the two midpoints of thebottom view and a preview isdisplayed on your curser.3. Click again to place thedimension.13

Autodesk Fusion 360: DrawingsStep 2 – Create aligned dimensions1. Click Annotation AlignedDimension.2. Click the top edge and bottompoint of the cutting blade of theright view.3. Move the cursor out to the leftand see a preview of thedimension.4. Click again to place thedimension and finish thecommand.Step 3 – Create angular dimensions1. Click Annotation AngularDimension.2. Select the left curved edge ofthe front view.3. Move the cursor out to the leftand see a preview of thedimension.4. Click again to place thedimension and finish thecommand.Step 4 – Create Radial Dimensions1. Click Annotation RadialDimension.2. Select the blade slider of theright view as the circle todimension.3. Move the cursor down and tothe left and see a preview of thedimension.14