Modeling an Airframe Tutorial

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1 EAA SOLIDWORKS University p 1/11 Difficulty: Intermediate Time: 1 hour As an Intermediate Tutorial, it is assumed that you have completed the Quick Start Tutorial and know how to sketch in 2D and 3D. If you struggle to recall how to do basic functions, please review the Tips Sheet. The guides you through the creation of a tubular airframe in SOLIDWORKS. The objective of the lesson is to teach you how to use the tools to design an aircraft frame. Time limits prevent us from completing this airframe, but you should learn the skills to model an airframe. You will create this part and drawing: This lesson includes: Creating a 3D Sketches Using the Weldment feature to add structural members Trimming structural members Creating a drawing and adding a cut list Bill of Materials (BoM)

2 EAA SOLIDWORKS University p 2/11 Creating a 3D Sketch for the Airframe In this lesson we will use the weldment feature to create an airframe. Weldments are structural members defined by a cross section picked from a library and a sketch line to define its length. This sketch line can be from multiple 2D sketches, or a single 3D sketch. By using two layout sketches (side and plan elevations), you can control the 3D sketch easily and any future changes will be reflected in your airframe. The layout sketches capture the design intent and the dimensions of the finished frame. 1. Open a New Part, verify Units are inches, and Save As Airframe (Top Menu / File / Save As). 2. Sketch and dimension the side elevation sketch. Select the Sketch toolbar, click Sketch, and select the Right plane. A sketch opens on the Right plane. Select Line. Start from the center, click, and move the mouse to the right to extend the line. You will see that the line is horizontal by the icon as you extend the line. Click again to finish the line. It does not need to be 189 inches. You will add dimension in the next step. Click the Esc key to stop drawing lines. 3. Select the Smart Dimension, select the line, enter 189 for linear dimension in the Modify dialog box, and select the green checkmark to accept. 4. Add a 28.5-inch vertical line from the origin. You will know the line is vertical from the icon. 5. Add four more lines as shown below to complete the outline of the side elevation. Notice that the inch line is longer that the 28.5-inch line. You will need to angle the bottom inch line down before creating the inch line or you will have difficulty breaking the parallel relationship of the top and bottom line. Also, notice the the dimension for the vertical line near the 11.5-inch line is the dimension between those lines. Exit Sketch when you are done in preparation for starting a new sketch in the next step.

3 EAA SOLIDWORKS University p 3/11 6. Draw a Rectangle that is inches wide on the Top Plane and connect it to your other sketch. Select View Orientation and Top Plane. Select the Sketch Toolbar, Sketch, and Top plane under the Design Tree. Select the Center Rectangle tool to begin drawing the rectangle. Set the width dimension to inches and click the green checkmark to accept. Press the Esc key a couple times to make sure that you are no longer in Smart Dimension. 7. Create a coincident relationship and attach the rectangle to the endpoints of the inch segment of Sketch1. Select the midpoint of either inch-side of the rectangle by hovering over it and clicking on it when it appears. Hold down the Ctrl key and click on the point at the corresponding end of the inch segment of Sketch1. Select Coincident under Add Relations in the Property Manager. Select the green checkmark to accept. 8. In the Top Plane View Orientation (Sketch2 rectangle should appear at bottom of the sketch and Sketch1 should appear as a line extending from the top of the rectangle). Sketch a line that starts at the top left corner of the rectangle line, and angles slightly toward Sketch1. Click to create an endpoint, but continue sketching lines in step Move pencil cursor to the right and cross over Sketch1 to create a second line that is parallel to the inch rectangle side. Click to create an endpoint that makes that line approximately inches. Press the Esc key to stop sketching lines. Dimension this line to Create a Coincident Relationship between the Midpoint of that line and the line from Sketch1 that it crosses. Create a smart dimension of 20 inches between the end of Sketch1 and the inch line. You may have to drag that line closer to the inch line to make the smart dimension work. 10. Draw a line that connects the endpoint of that line with the right corner of the rectangle line you worked on in step 10.

4 EAA SOLIDWORKS University p 4/ Create a Centerline by reusing an existing line with the Convert Entities tool. Select the 189-inch line from Sketch1. In Sketch mode, click on the line, select Convert Entities and click the green checkmark in the dialog to accept. To make it appear as a Centerline, right-click on the line and select the Line to For Centerline tool. 12. Create a circle at the end of the aircraft centerline of Sketch2 on the Top Plane with a diameter of inches and make it For Construction. 13. Add a line from the inch line to the aircraft centerline, following the angled dashed yellow line, press the Esc key to terminate it, and dimension it to 0.15 inches from the end of the aircraft centerline and click the green checkmark to accept this line. Exit Sketch and Save. Creating a 3D Wireframe The next step is to create a 3D wireframe, which is done with a 3D sketch. To make it easier to locate the wireframe elements, we will add reference planes at the points of fuselage transition. The front plane sits at the front of the aircraft, we need to add planes where the frame changes direction. 1. Show the Front Plane (if hidden) by clicking on the plane in the Design Tree and select the eye icon. 2. On the Features toolbar, select Plane from the Reference Geometry dropdown. 3. The first reference is the Front plane and the second is a point on Sketch1 opposite the inch rectangle. Under Parameters, it should say Front Plane under First Reference, Parallel icon should be selected, for Second Reference, Coincident icon should be selected, and if the blue arrow on the new plane is pointing to the Front plane, check the box for Flip Normal under Options. Click the green checkmark to accept. 4. Repeat the process from step 3 to insert another plane parallel to the Front plane at the inch line. 5. Create the 3D wireframe. You have the top sketch drawn and will need to create rectangles on each of the planes. Switch to the Sketch toolbar. Click the down arrow under the Sketch tool and select 3D Sketch. Select the Convert Entities button and select the green checkmark to accept.

5 EAA SOLIDWORKS University p 5/11 6. Select the Front plane and with the plane selected, chose the Center Rectangle tool. Hover over the midpoint of the vertical line from Sketch1, click on the midpoint and drag the rectangle so that it overlaps the inch line of the rectangle on Sketch2 and the top point of the line from Sketch1 to draw a rectangle on the Front plane. Select the green checkmark to accept. 7. Create a Coincident Relationship between the top line of the center rectangle from step 6 and the top point of the vertical line from Sketch1, and select the green checkmark to accept. Do the same with each of the bottom corners of the center rectangle and the corresponding end points from the inch side from the Sketch2 rectangle. 8. Create rectangles on Planes 1 and 2. Remember to click on the correct plane before drawing each rectangle. To set the height for the rectangle on Plane 2, hover over the top line until the Midpoint shows up, click on it and then click on the top line of Sketch1 and create a Coincident relationship. 9. Before you draw wireframe lines to connect the rectangles, you may want to hide Sketch1 and Sketch2 by clicking on them in the Design Tree and selecting the eye icon. 10. With the Line tool under 3D Sketch, connect each vertex of each rectangle corner with the corresponding vertex from the other two rectangles. After the wireframe is complete, select the green checkmark to accept the sketch. Add Structural Members The fuselage structural members are made up of weldments. These are structural extrusions with length and orientation defined by 2D and 3D sketches.

6 EAA SOLIDWORKS University p 6/11 1. Open the Weldments tool bar by right-mouse clicking on any toolbar tab and select Weldments from the context menu. If the 3D Sketch icon is active, click on it to stop sketching and then select the Structural Member icon. 2. In the Property Manager, set Selections to Standard: ansi inch, Type: pipe, and Size: 1.5 sch Begin applying the pipe properties to the sketch by selecting a line from the sketch and ensure Apply corner treatment is unchecked. Continue selecting lines to apply the pipe properties until lines no longer accept the pipe properties. 4. Select the New Group button, and select a line without pipe properties applied and select connected lines until they will no longer accept pipe properties. Repeat this process until all lines have pipe properties applied. Add Frames & Bracing With the main longerons in place, we now have to add the intermediate frames and bracing structure. 1. If Sketch1 is hidden, select it in the Design Tree and select the eye icon to make it visible. Then, click on it again and select the Edit Sketch icon. 2. Orient the sketch to the Right Plane view, select the Line tool on the Sketch toolbar and begin drawing vertical frame members. Dimension the distance between the first two sets of parallel vertical bracing at 19-inches and then sketch diagonal cross members. Notice the distance between the last two vertical member is not dimensioned. That is already defined by the inch dimension. 3. Add frame and bracing dimensioned at 26-inches apart along the rest of Sketch1. Exit Sketch.

7 EAA SOLIDWORKS University p 7/11 4. Create a Plane parallel to the Front plane at the closest frame and bracing. Select Reference Geometry and Plane, then select the Front Plane as the first reference, and the top point of the closest vertical frame member from Sketch1. 5. To use the new plane as a reference, for the 3D Sketch, move it up in the Design Tree. Click on it, continue holding your left mouse button down and drag it to just before 3DSketch1 on the Design Tree. 6. Right click on the pipe in the design tree and hide it so you can see the sketch wireframe more clearly. 7. Click on 3DSketch1 and select the Edit Sketch icon in the context menu. 8. Click on the Shaded Sketch Contours button in the Sketch toolbar so you can see the wireframe more clearly. 9. Draw a Center Rectangle on the new plane and create Coincident relationships between the rectangle corner points and the relevant lines on the airframe. Add a line connecting the bottom corner of the front rectangle frame to the top corner of the first intermediate rectangle frame. You could continue adding planes, rectangles, vertical frames and cross braces, but in the interest of time, we will move on to editing the pipe to add the newly sketched wireframes. Exit Sketch. 10. Click on the pipe feature in the Design Tree and show it. Then, click on it again in the Design Tree and click the Edit Feature icon. 11. In the Property Manager, select New Group, and add the lines of the intermediate rectangle frame. Click the green checkmark to accept. 12. Add a new Weldment Structural Member with Selections set to Standard: ansi inch, Type: pipe, and Size: 1.0 sch 40. Select the cross member brace you just created, and click the green checkmark to accept.

8 EAA SOLIDWORKS University p 8/11 Add Rudder Post & Supports 1. Create a new 3D sketch. Select the Right Plane and draw a vertical line for the rudder post near the tapered end of the airframe. Right click on the new line and select the Collinear icon in the context menu. 2. Dimension the segment at the top of the rudder post to 5-inches and at the bottom to 3-inches. Click the green checkmark and exit the sketch. 3. Add wireframe lines to draw supports to connect the back rectangle wireframe corners to the rudder post line. Click the green checkmark and exit the sketch. 4. Add Weldment Structural Member with Selections set to Standard: ansi inch, Type: pipe, and Size: 1.5 sch 40, and apply to the rudder post. 5. Add Weldment Structural Member with Selections set to Standard: ansi inch, Type: pipe, and Size: 1.0 sch 40, and apply to the rudder post supports. Cleanup If you zoom in to the lower front corner of the airframe, you will see that the pipes are intersecting. The next step is to trim and extend the pipes to the correct sizes and end conditions. Looking at the bottom corner from the side we can see that the longeron pipe is shorter than the extent of the vertical rectangle frame pipe width. Longerons will need to be extended and then pipes will need to be trimmed. 1. Create an offset plane to account for the width of the pipe. Select Reference Geometry and Plane from the Features toolbar. The First Reference is the Front Plane. The default is offset, so edit the D1 from 0.10 to 0.95-inches and flip the offset if necessary so that the offset plane is on the outside surface of the rectangle frame pipe (blue arrow will point in direction of offset). Click the green checkmark to accept the new plane. 2. Select Insert / Weldment / Trim/Extend from the top menu to open the Trim/Extend tool Properties dialog or click on the Trim/Extend tool in the Weldments toolbar.

9 EAA SOLIDWORKS University p 9/11 6. Leave the Corner Type as End Trim, select the four longeron pipes for Bodies to be Trimmed, make sure Allow Extension is checked and the Face/plane radio button is selected, select the Trimming Boundary box and select the offset plane from step 1. The pipes will extend up to the new plane. Click the green checkmark. 7. Trim the frames and supports starting at the front. You will select frame and support pipes as Bodies to be Trimmed and select the longeron pipes as Trimming Boundary Bodies under Property Manager. Check the box for Allow Extension and select the Coped Cuts icon. Click the green checkmark. Repeat this process for all frame and support members. 8. Join the two tubes that make up each longeron. Zoom into where the longeron goes from the horizontal to angled pipe and you will see a slight gap. Open the Trim/Extend command and set the Trimming Boundary to Face and select the plane at the end of the horizontal section of the tube. Select the four angled tubes as the Bodies to be Trimmed. Click the green checkmark.

10 EAA SOLIDWORKS University p 10/11 Create a Drawing Using the skills and steps outlined before you can create a fully detailed and trimmed fuselage frame, but in the interest of time, we will move on to the final step creating a production drawing. The first thing we will do is clean up the view of the model by hiding all the planes. We can do this individually or through the mini toolbar at the top of the modelling area. 1. Select the eye icon and a drop down list appears. De-select the planes icon at the top of the list to hide all the planes in the model 2. Select File \ Make Drawing from Part in the top menu. 3. Select your drawing sheet size (click on size to preview orientation and dimensions). 4. Click on the side view orientation and drag it onto the page. Click to place it. If you move the mouse around, it will display other views and you can click to place them. Click the green checkmark to finish adding views. 5. You can move a view on the page by hovering over it, moving the mouse to the dashed box around the view, clicking and holding the mouse button grab the view, moving it to where you want it and releasing the mouse button. 6. Add a table showing all the pipes that need to be cut. Select Insert \ Tables \ Weldment Cut List from the top menu.

11 EAA SOLIDWORKS University p 11/11 7. Select a view from which to build the cut list. In this case, we will use the Isometric View. Accept the default and select the green checkmark. The table is now on your mouse and you can place it with a mouse click.

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