Oh oh. Well, a quick and easy way to model just about anything that is cut from length. Unlike an assembly file where each individual length of material would be its own part. Well, let's use multiple bodies within a single part file, allowing for faster creation and greater control of the entire frame's shape and size. We're going to walk you through the steps required to go from a blank document to a fully complete trailer chassis, using Wellman's as the primary modeling tool. The starting point for any element is a sketch, and this sketch is a stick out line of where your length of material will eventually lie. Let's begin by creating a new part file. I'm starting a sketch on the top plane. We will place the center rectangle about the origin, and then add in a horizontal midpoint line centered on the lower edge of the rectangle. Sketch a centerline vertically upwards from the origin and place this outside of the rectangle boundary. Sketch a small vertical line over the top of this centerline, ensuring it lies fully outside of the rectangle boundary. This will become the tow bar. Add in an angled sketch line. Snap to the midpoint of the tow bar, and snap to the left hand side of the rectangle. Finally, sketch in a horizontal line directly across the middle of the rectangle, snapping to each midpoint. We then need to add the dimensions. Select Smart Dimension from the sketch tab. The height of the rectangle is 2.5m. The width of the lower midpoint line should be two meters, with a 300mm offset from the outside of the rectangle. This can be positioned on either the right or left hand side of the rectangle. 750mm between the angled bracing and the top of the rectangle. And 500mm for the length of the tow bar, with a 150mm offset from the top of the rectangle to the underside of the tow bar line. If you pause this point, you can see all of the required information for the sketch. When you're done, exit the sketch. To access the wildman features. You will need to enable the weld tab. Right click on any of the existing tabs and make sure weld is ticked. Choose Structural member. Pick ISO for the standard. C channel for the type. And 120 by 12 for the size. Click on the left hand side of the rectangle and the profile will appear down the sketch line's length. This profile can then be rotated, mirrored, and positioned using the options towards the bottom of the properties dialog. On the left hand side of the screen, to position this first structural member, use the Locate Profile button to snap to the top left hand sketch point within the C channel profile sketch. If you require multiple structural members that are the same profile type and size, this can be achieved by using a new group rather than creating a new feature. Choose new group and position the corresponding profile on the right hand side of the rectangle. You will need to rotate the profile through 180 degrees, and then locate again using the Locate Profile button, snapping this time to the top right hand corner of the sketch point within the C channel profile. Choose new Group again and position the central bracing. The profile will need rotating through 270 degrees and positioning using the Locate Profile button. Snapping to the center. Sketch point of the profile. We'll go into adding some more structural members. This time they will be rectangular, so we need to add in a new structural member feature. To structural member, pick ISO for the standard rectangular tube for the type and 70 by 40 by five for the size. Position this profile along the back. Bracing the tow bar and the angled bracing. Each of these will require a new group and be positioned using the Locate Profile option. The angled bracing needs to be trimmed back where it meets the side rail. This can be done using the Trim Extend tool found on the Wildlands Time. Select the body to be trimmed, which in our case will be the angled bracing, and then select the inside face of the side rail. As the trimming boundary, the angled bracing is split into, allowing you to discard the smaller piece of material. As with any SOLIDWORKS model, making the most symmetry will speed up the design process. Here we're going to mirror the angled bracing about the right plane. Choose the mirror feature from the features tab and select the right plane. In the Mirror Face Plane dialog box. Make sure that you're mirroring bodies rather than features. There is a specific selection box for this. Click on the bracing to populate the selection box. Green tick. When you're done. We'd like multiples of the back bracing to be equally positioned along the length of the chassis, rather than modeling each bracing individually. We will use a pattern. Choose the linear pattern feature from the main features tab in the first selection box. Select one of the edges that runs the length of the side rail. This sets the direction for the pattern. Scroll down to the selection box named bodies and tick this off. With this selection active. Choose the back bracing. You should now see a preview on screen, but the spacing and instances are not yet set to the values we need. Toggle the radio button under direction one to up to reference. Some new options become available. The first is a selection box. Choose the end face of the side rail at the opposite end to the back. Bracing. Toggle the next radio button to selected reference. A new selection box will appear in here. Select the side face of the back bracing. Choose number of instances for the next button down and set the value to four. What we have achieved here is uniform spacing along the length of the side rail. If the side rail changes in length, the bracing will automatically move to you. Currently there is no material specified. So next we need to apply one. Right click on the material from the feature manager and choose Plane Carbon Steel. This changes the appearance and the weight of the part, using what is a really quick way of adding in cut from length geometry. But one of the other main benefits is that it automatically creates a cut list in the feature manager. On the left hand side you will see the Cutlass folder. Expand this to see the cut list items. Right click on any cut list item and choose properties to view all of its information. We would like to create a 2D drawing of our frame. But before we do this, we need to save the file. Choose save and give your file a name. I'm going to call mine chassis. Once saved, choose make drawing from part from the file menu. When prompted for a template, choose A3 and C landscape. From the view palette on the right hand side. Drag and drop a right hand view onto the paper space. As you move your cursor, you should see that the other projections become available. Move your cursor upwards to position a top view and then left click. If you then move your cursor out at an angle and isometric view will appear to break the 45 degree alignment. Hold control on your keyboard before placing. The views look a bit too small, so we will change the sheet scale. Hit the upward arrow in the bottom right hand corner of the screen and choose User Defined. Then set the scale to 1 to 25 and hit okay. The cut list information from the parts can be inserted into the 2D drawing, and this is done by choosing World Cut List from the table. Drop down on the annotations tab, selecting a view and then hitting the green tick. You should then find that the table is on your cursor and can be positioned on the drawing. The item numbers from the cut list can be shown on the drawing view too. And this is done by selecting a view and choosing auto balloon from the annotations tab. Finally, let's add in a few key dimensions to the model, capturing the width and the length. Use the Smart Dimension tool from the annotations tab. This is the same dimension tool that we used in the sketch environment. Currently the frame length is 2.5m. If we make an adjustment in the part file, this change is instantly seen in the 2D drawing. Toggle back to the part file using the window menu. Click on the first sketch in the feature Manager and change the 2.5m dimension to 2.75m. Toggle back to the drawing again using the window menu. Notice the updated dimensions on the drawing views and the changes to the list length. If your dimensions or lists haven't updated, try hitting the traffic light icon in the top middle of the screen. This prompts a rebuild. This is just a small example of some of the functionality available within SOLIDWORKS world, but if you would like any more information, make sure to get in touch and we will be happy to help.