 In this tutorial, we will create the manufacturing drawing for the coupling arm in Solid Edge. First, click the Solid Edge application button and from the new menu, select Isometric Draft. Click View Wizard on the ribbon bar and select the coupling arm part. From the command bar, select a scale of 1 to 1 and click to place the view. Continue to place the top view, side view and an isometric view of the part. If a drawing view is placed out of the sheet borders, click and drag the view inside the sheet. With the isometric view still selected, change its shading from the command bar, then right-click the view and select Update View to display the shading on the view. Now, to create an auxiliary view, start the command from the ribbon and select the top inclined edge and place the view. Next, select the auxiliary view and drag the view handles to crop the view, then right-click and select Update to finish the cropping. Next, right-click the auxiliary view again and break its alignment with the principal view. Mood the view to a desired location by dragging. Now, start the Retrieve Dimension command and click the orthogonal views to extract the dimension added during model creation. To place additional dimensions, use the Smart Dimension and the Distance Between commands. Drag overlapping dimensions using the handles on the dimensions. Drag handles on linear dimensions to adjust the extension line gaps. Keep the Alt key pressed and create jogs on overlapping or closely placed dimensions. You can use handles on the dimensions to flip arrow sides if they do not fit in the default space. To create dimensions aligned to an inclined edge, start the Distance Between command and pick the Use Dimension Access option from the command bar. Specify an axis to place the parallel dimension. Next, create center marks by dragging a window around the circles and choosing to use a dimension access again. Add a suffix to an existing dimension by selecting it and adding a suffix from the command bar. Apply this format to other existing dimensions using the Copy Attributes command from the ribbon bar. Next, create a detail view by starting the command and drawing a circle around the desired area of the main view. Drag the detail view circle to dynamically update the detail view. Transfer a dimension from the parent view to the detail view by dragging the dimension handle. Next, right-click the detail view and select Properties. Check on the box for the view borders and click OK to display borders for the detail view. To add notes to the drawing, start the Technical Requirements command. Add notes in the dialog box and observe that they are numbered automatically. Next, add a call-out to the drawing views and add a reference to the note you made in a previous step. You can also modify the sequence of the notes in the Technical Requirements dialog. Notice that the numbering is updated automatically. Now, add a datum frame to one of the faces of the slot in the principal drawing view. To add a feature control frame, start the command from the ribbon bar. In the dialog that appears, select the desired control feature symbol. For example, Parallelism, type in the value, click to add the divider symbol, and pick the datum from the reference list. Watch the preview of the feature control frame build up with each click and finally place the feature control frame attached to the required face. The manufacturing drawing for the coupling arm part is now complete. In this tutorial you learned how to create principal, isometric, auxiliary, and detailed drawing views. How to shade, crop, and align drawing views. How to automatically retrieve model dimensions and place smart dimensions on the drawing views. How to add center marks and tweak dimensions using the handles. How to use the Alt key to create jog dimensions. How to copy dimension attributes in a single operation. How to add call outs and smart notes to drawings. And how to add datums and feature control frames to convey manufacturing intent.