AUTODESK FUSION 360 Designing a RC Car Body

Transcription

1 AUTODESK FUSION 360 Designing a RC Car Body Abstract This project explores how to use the sculpting tools available in Autodesk Fusion 360 Ultimate to design the body of a RC car. John Helfen john.helfen@autodesk.com

2 Table of Contents Designing a RC car Body for the H-Cell 2.0 Kit... 2 Prerequisites... 2 Preparation... 2 Repositioning Parts... 2 Moving a part in the model... 2 Sculpting the Body... 3 Entering the Sculpt Workspace... 3 Creating a Sculpted Form... 4 Sculpting the Box Form... 6 Adding Symmetry from the Model... 7 Removing Symmetry from the Model... 7 Changing the Appearance of the Form... 8 Creasing the Bottom Edge of the Form... 9 Edit Form Tool Sculpt the Form with Edit Form Tool Adding Details to the Form Creating a Hood Scoop Inserting Edges Welding Vertices Shelling (hollowing) the Body Cut Openings for Wheels and Bumper... 20

3 Designing a RC car Body for the H-Cell 2.0 Kit Prerequisites Create a free Autodesk ID from ultimate (used to access and use Fusion 360 Ultimate) Install Autodesk Fusion360 Ultimate from ultimate Preparation Uploading required files Watch a video explaining how to upload required files to Fusion. Repositioning Parts After getting the Fusion and the files set up you may find that parts in the provided digital model are not in the same location as their physical counter parts on the car chassis. For example, the controller box, battery, and possibly other parts may have been moved for a number of design reasons. It will be important to reposition parts to match the car configuration to ensure the body will not interfere with other parts on the chassis. Moving a part in the model Parts can be moved by selecting (left click) a face on the model, and then right click and select the Move command from the marking menu. While in the Move command parts can easily be added or removed from the selection set by clicking a new part to add it or click a selected part again to remove it.

4 After activating the Move command a manipulator appears in the graphics window that will allow you to move or rotate the selected part(s) in any direction depending on which part of the manipulator is selected. The images above display the step required to move the control box to a new location. Note: The steps above show moving the control box bodies, but this this process will need to be repeated for each part that has been moved. Watch a video explaining how to move parts. Sculpting the Body Up to this point all parts have been created or manipulated in the Model workspace, as indicated by icon (labeled MODEL) on the left side of the toolbar. Entering the Sculpt Workspace To create the body of the car you will use the Sculpt workspace. Click on the purple sphere (ball) found in the CREATE tab of the toolbar to place Fusion in the Sculpt workspace and dim the other parts of the model. The workspace icon on the left of the toolbar will show SCULPT.

5 After entering the sculpt workspace you will see a purple sphere in the timeline at the bottom of the screen. Once a new form has been created, the purple sphere can be double clicked to return to editing this form. The form that will be created can be thought of as a block of digital clay that can be formed, or sculpted, into a RC car body. Watch a video explaining how to enter the Sculpt workspace. Creating a Sculpted Form There are many different primitive shapes which can be created, but a box will be a good starting point for the body. Selecting a shape from the CREATE tab of the toolbar will begin the process of creating the first form, called a T-Spline body. T-Spline Bodies are made of vertices (points), edges (lines), and faces that define the shape of the body. These vertices, edges, and faces will be moved, in a similar way to how parts were moved in the previous step, to change the shape of the form. When creating a form several actions will need to be taken to create the form. A face, or plane, will need to be selected as the construction location and the shape of the form must be defined. Start creating a box form by clicking on the Box command on the CREATE tab of the toolbar. After doing this the box dialog and the origin planes will appear on the screen. Note: The origin planes are a fixed location in space that can be used to construct geometry. As the cursor is moved around the screen each of the origin planes will highlight based on where the cursor is located. Hover the mouse below the car and you will see the plane parallel to the deck highlight. Left click to select the highlighted plane. The grid should appear as shown in the image on the right above. Use the ViewCube to rotate the model to view the car from the top and change the rectangle type in the dialog box from Center to 2 Point as shown in the image to the right. This will make it easier to define the rectangle that will define the form. Left click on the upper left area in front of the tire and above the bumper to place the first corner of the rectangle, then left click just

6 behind the bottom right wheel to create a rectangle that will roughly encompass the chassis. Note: This rectangle does not need to be placed or sized perfectly as it will be changed when the form is sculpted with edit form tool in the coming steps. After clicking to place the second point of the rectangle a preview of the default shape will appear. By clicking on the Home icon, which appears when the cursor is hovered over the ViewCube, will change the viewpoint so you can better see the form being created.

7 When creating sculpted forms best practice is to limit the number of length, width, and height sections to the smallest number as possible, as more edges can add unnecessary complexity. Additional edges can be added as needed during the sculpting process. Set the length and width faces to 4 and the height faces to 3. After doing so, the form should have a slightly more rectangular shape. Click OK in the dialog box to complete the creation of the Box T-Spline form. Watch a video explaining how to create a Sculpt form. Sculpting the Box Form After creating the box, you will now start to modify the form. Within the sculpt workspace there are two activities which will be very important for this project; adding and removing symmetry and moving vertices, edges, and faces.

8 Adding Symmetry from the Model During the design process symmetry is important because it will dramatically limit the amount of work required to sculpt the body. Symmetry allow changes on one side of the symmetry line to be reflected automatically to the opposite side. Symmetry can easily be added and removed as needed throughout the sculpting process. In this project, Mirror Internal and Clear Symmetry will be used to speed the process of sculpting the car body form. Click the Symmetry button on the toolbar to define symmetry for the model. Once the command is launched two faces which are symmetric to each other must be selected. Select any two faces that share a centerline through the middle of the form. The results of editing two vertices of the form with and without symmetry are shown below. Watch a video explaining how to add and remove symmetry from the model. Removing Symmetry from the Model If needed Symmetry can easily be removed from the form by clicking the arrow below the Symmetry button on the toolbar and select Clear Symmetry. With the Clear Symmetry dialog box open click on a surface on the form and click OK in the dialog box to remove the symmetry. Note: A form surface must be selected because it is possible to have unique symmetry defined on each form in a sculpt workspace.

9 Changing the Appearance of the Form The body must be sculpted around the chassis and other internal components. To help with this, the appearance of the form can be changed by applying transparent appearance. An Appearance defines the look of the material, like glossy, paint or textured, but does not affect the physical material properties like weight. It is also possible to apply a physical material, but it is not required for this project. Ensure no other commands are active, by pressing the escape (ESC) key on the keyboard, then right-click and select Appearance from the menu. The top half of the dialog displays appearances that are or have been used in the current design. Note: Right-clicking in the white area of the In This Design section allows removal of unused appearances. To apply an appearance to a part, scroll through the Library at the bottom of the dialog to locate Glass (Clear). It can be found in the Glass folder, under the Smooth category. Left Click and drag the glass material over the part and release the mouse button to apply the appearance. In the image below you can see the form is now transparent and allows the internal components to show through. Watch a video explaining how to change the appearance of the body.

10 Creasing the Bottom Edge of the Form Use the ViewCube to rotate the model to a side view and you can see that the form is rounded on both the top and bottom. The first step in forming the body is to crease the edges at the bottom of the model. This will make manufacturing of the body easier. While looking at a side view, double-click one of the edges that is closest to the bottom of the model. Double-click, as opposed to single clicking, will select this edge and all other edges connected to the selected edge. The selection will stop when it runs into a point where it has multiple paths that could be taken, in this case near the corners. With the edge selected, right-click and select the Crease command from the menu. This will pull the edge down so it is even with the bottom of the model and bring up a dialog box showing 4 items selected. While the crease command is still active, you will want to crease all the outside bottom edges. Rotate the viewpoint and continue selecting all the outside bottom edges as shown in the images below. Click the OK button to apply these changes.

11 Watch a video showing how to crease edges on a form. Edit Form Tool With bottom edge creased in the previous step, the sculpting of the form can continue. Sculpting a form is accomplished through the Edit Form tool. By right-clicking on the screen and selecting Edit Form, a dialog box with a series of tools is displayed. This dialog box includes many options, but the selection filter is most important to the sculpting process. The selection filters tell the Fusion what specific type of geometry you want to edit and helps make selecting that geometry easier.

12 Below are a series of images showing multiple vertices, edges and faces selected with their corresponding options enabled in the dialog. The selection filters are highlighted yellow in the image to the right to make them easier to locate. Sculpt the Form with Edit Form Tool As mentioned earlier, each car design may be slightly different based on where components have been place. While the instructions will show specific steps; this section of the document will inevitably be different for each person. Use the following steps as a guide to form the body to the desired shape. Rotate the model to view it from the side then right-click and select Edit Form from the marking menu. Set the selection filter to vertex and all vertex points will appear on the model. The images below are a series of before (on the left) and after (on the right) shots that show the effect of moving geometry on the form. The selection of each set of vertices is done by left clicking and dragging a box around the vertex point that are to be modified. Throughout the process it will be important to remember where internal components in relation to the body. The view of the model can and should be rotated to evaluate whether the body is interfering with internal components. Note: The sculpting process can take a few minutes or as long as needed to generate the level of detail and fine tuning required to shape the form. There is no Right amount of time or detail. It is up to you as the design to determine the level of detail required to reach the desired shape.

13 While editing geometry Fusion is set to move geometry in set increments, by default 0.25 inches. At times it may be helpful to adjust this increments based on the work being done. This can be done using the Navigation bar at the bottom of the screen. On the toolbar, click the Grid and Snaps setting, second button from the right, and select set Increments. Change the linear increments value to the desired amount and click OK to apply the changes. Results of the changes above are shown in the image below.

14 Rotate the model into and perspective view looking at the car from the front driver side angle. In the next series of images the edge selection filter will be used to make additional changes. Remember that during this process switching between different selection filters and view of the model is very common.

15 After making a few changes it is a good practice to rotate the model and look at it from different perspectives to see the effects of the changes. To the right is an image looking at the model from the front and it appears the wheels are not covered and a slight bump has developed near the roof. These can be resolved by using the vertex and edge selection filters and changing the position of the some geometry.

16 The image above shows the front of the body after several additional edits including: Pulling the front middle edge forward Moving the edge in front of the wheel back closer to the tire Pulling the vertex located above and behind the wheel out to the side and toward the back After further editing, an unlimited number of complex forms can be created and many iteration made be created before determining the correct form for the design. Below shows what the form could become with more editing. In the next section you will learn how to add a hood scoop. The process for creating a hood scoop can be used to create other details like fins or a spoiler as well. Watch a video explaining how to use the Edit Form Tool.

17 Adding Details to the Form Creating a Hood Scoop In the beginning the project it was mentioned that the fewer face sections started with the better because complexity can always be added as needed. As details like the hood scoop are added additional edges will need to be inserted and vertices welded together to have better control over the form. Inserting Edges To have better control over the width of the hood scoop without greatly affecting the overall form shape, new edges will be inserted. Double-click on either of the highlight edges shown in the image, remember double clicking and edge will attempt to select all edges that make a loop around the form, unless the loop reaches a point where multiple paths could be taken. Note: When Symmetry is on, Double-clicking one edge will automatically select the corresponding loop edge on the opposite side of the model. In the image above the blue line was double-clicked and the yellow line was automatically selected because of Symmetry being turned on. With the edge loops selected, right click and select Insert Edge. Doing this will present a preview of the edge to be inserted and the Insert Location value will show It is important to note that in the case of inserting an edge the 0.50 value is not an inch value, but instead a percentage (50%) of the distance from the selected edge to the next edge. If the previewed edge is on the wrong side of the selected line; changing the Insert Location value to a negative will move the edge to the other side of the selected loop edge. For this edge insert the value will be set to 0.25, but it is also important to understand this

18 may need to be slightly different for each design. The images below show the insert edge preview and results. Note: In the image above, the heavy blue line is the edge that was selected and the heavy green line is the preview of the edge to be created. To control the transition between the hood scoop and the windshield an additional edge will be inserted in the opposite direction using the edge at the bottom of the windshield as the selected insert edge loop. For this insert the value is set to 0.10 to keep the edge fairly close to the selected edge loop. With the control edges inserted, it is time to create the hood scoop. Up to this point geometry that existed on the form has simply been moved around to change the shape of the body. To create the hood scoop new faces and edges will be added to create the bump in the hood that will be shaped into the hood scoop. Start the Edit Form tool and select the highlighted faces by left clicking on one, then holding the shift key down on the keyboard and clicking the other. For this step symmetry can remain enabled, but it is important to select each of the faces or the results may be unexpected. Note: Both faces will be blue if they have been properly selected. If one of the faces is yellow it indicates the face is only selected because of the symmetry. With the faces selected, hold the ALT key down on the keyboard and drag the arrow up. Unlike what has happen in the previous steps, with the ALT key held down Fusion will keep the edges around the faces and add additional edges to create new faces and add material to the form.

19 While the faces are still selected use the arrow pointing toward the back of the car to drag both faces forward slightly to smooth the transition near the windshield and sharpen the front of the hood scoop. Click the OK button to commit the changes. Watch a video explaining how to create a hood scoop. Welding Vertices Depending on the design intent, the last step is to weld the vertex points at the back of the hood scoop to the corresponding points on the edge that was inserted in front of the windshield. From the modify menu on the toolbar select Weld Vertices. Below is an image showing the results of adding the hood scoop and a small spoiler to the body. The same steps can be used to create other details such as fins, spoilers, and lights. Watch a video explaining how to weld verticies on the hood scoop.

20 At this point the body has been developed enough for vacuum forming if the intent is to manufacture a body for the car. The form can be exported for slicing in 123D Make or cut on a CNC machine to create the buck or mold for the vacuum forming. If the intent is to use the body for marketing and promotional images, then additional actions should be taken to make the model look more realistic. The following sections will explain how to shell (hollow out) the body, cut openings for the wheels and bumper, and add decals. Shelling (hollowing) the Body With the body sculpting complete, return to the MODEL workspace by clicking the workspace button on the far left of the toolbar and selecting MODEL. In this workspace additional features can be added to complete the body. To hollow out the body, select the Shell option from the MODIFY menu on the toolbar. Select the bottom face of the model as the face to remove, set the shell value to inches, and click OK to shell the body. The images above show the face to remove and the results of the shell action.

21 Cut Openings for Wheels and Bumper In order to cut an opening for the wheels and bumpers a new sketch much be created. Right click and select sketch, then rectangle to begin the sketching process. Select the origin workplane that runs through the center of the body as seen in the image to the right. Turn on the visibility of one front and one rear wheel and the bumper for reference. These will be used to properly position the openings. Use the view cube to rotate the model to look at the car from the side. From the SKETCH menu select Project/Include then Project. Select a circular edge on each of the tires in order to project the circles to the current sketch. The purpose of this project is to simply locate the center of the wheel in order to create another circle to remove material to make room for the wheels. After projecting a circular edge from each tire, select circle from the SKETCH menu to create the shape to remove the wheel opening in the body. Use the center from the projected circle as the center of the new circle and set the diameter to 3 inches. Then use rectangles and lines to create the sketch shown below. The image on the left shows the sketch with the tire edges projected and the image on the right shows just the sketch with the bodies. Below those images is an image of just the sketch for clarity.

22 The purpose of the sketch is to create opening in the body for the wheels and bumper as well provide some ground clearance. With the sketch complete, right click, select Press/Pull then select all the profiles that were created. In the Extrude dialog box that is presented, set the Direction option to Symmetric and set the distance to 4.25 or any value that will extend the cut beyond the edges of the body. The symmetric setting will ensure that the cut is made on both sides of the car body. Note: It is critical that the visibility of all components and bodies, except the RC car shell, are turn off by clicking the lightbulb next to each item in the browser on the left side of the screen. Any items that are visible and intersect the cut operation will be removed from the design.