Join Jomarc Baquiran for an in-depth discussion in this video Creating components, part of Migrating from AutoCAD to Fusion 360.
- [Instructor] One of the key feature of Fusion 360 is its ability to create dynamic assemblies. If your intent is to create an assembly that will function in the real world then, the first step is to create a component and apply joints. Now, we have two ways in creating a new component. The first way is heading to assemble. Selecting new component.
Definitely, this would be an empty component. And, will not be coming from an existing body. Let's name our component as plate. The parent being out main file. Let's uncheck activate. And, because we will not be working with a sheet metal component, let's leave this unchecked. Hitting OK.
In this scenario, our intent is to model our plate component. A very important rule when working on a specific component, the component should be activated. And, to activate plate, we should select activate component. From here, we can now begin sketching. Let's hit R for rectangle, select our XY plane.
I'm going to change our rectangle to center rectangle, drop our center point at the origin, the height to be 40, hitting tab, the length to be 120, hitting enter. Next, let's create two circles here for the holes, hitting C for circle, left click here, diameter to be 10, hitting enter, hitting C once more, creating another circle, and, instead of keying a value, I will left click, hit escape, select our left circle, control, left click our right circle, right click and select equal.
Next, I will grab our line tool, create a line from the center point of the circle to the center point of this other circle, hitting escape. Let's turn this line into a construction line by hitting X and finally, reselect this line, hold control S, select our origin, right click, and select midpoint.
Inspecting. And, finally, selecting this line once more, right click, selecting horizontal. Next, grabbing our dimension, hitting D, selecting this horizontal line, drop our dimension here, left click, and key in 80, hitting enter, and hitting escape. Hit E for extrude, select this profile, change the direction to symmetric.
For measurement, let's select whole length. The distance to be 15. Operation new body and hit OK. Another very important rule is always make it the habit that your parent component or your base component should always be grounded. The plate being our base component, I will right click on our component plate, select ground.
The second way in creating a new component is to head to our main file, right click, and select new component. For organization, let's rename this. Left click and left click once more. Rename this to link, hitting enter. Notice, this new component is already active and before we start sketching, let's isolate link by right clicking, going down, and selecting isolate.
Next, let's grab our center to center slot selecting our XY plane. Let's drop our first point here. Left click. I'm going to key in 30. Left click, move our cursor, key in 10. Left click once more. Let's zoom in and hit escape. Next, selecting this horizontal construction line, control left click our origin, right click and select midpoint.
Let's make this line horizontal as well. Left click, right click and select horizontal. Let's grab our circle by hitting C. Create a circle on this endpoint. I'm going to key in 10, hit enter, hitting C once more for circle. Left click, hit escape, grab our equal constraint, select the parent, this one to be the child.
Hit D for dimension, selecting this arch. I'm going to key in 10. Dimension tool is still active. Selecting this horizontal construction line. Left click here and key in 30. Hitting enter. Hitting E for extrude. Going to home view. Making sure our mode of selection is window.
Zooming out, creating a window selection. Change the direction to symmetric. Measurement to be whole length. And, I want the thickness of this extrusion to be five. Operation new body and hit OK. Next, let's reuse our sketch. For extrusion, let's turn on the visibility of our sketch.
Hitting E for extrude. My intent here is to select this circular profile. I'm going to hold my left mouse button until a menu appears selecting profile, moving our arrow to the right. So, notice it's a cut extrusion. Let's change the operation to join. For the distance, I'm going to key in -2.5 minus 15.
Finally, hitting OK. Hitting E once more for extrude and selecting this other circular profile. Moving our arrow, changing the operation to join, keying in 2.5 plus 10, and hitting OK. Let's turn off the visibility of sketch five, activate our main file, right click and select unisolate all.
Zooming out. And, because link is ungrounded and has no joints, we can move this component by holding our left mouse button and move. Join me in the next lesson as we insert a new component into our current assembly.
- Similarities and differences between AutoCAD and Fusion 360
- Collaborating in Fusion Team and A360
- Sketch constraints
- Creating and modifying tools
- Design intent
- Assembling parts and components
- Creating 2D drawings
- Importing AutoCAD files
- Exporting a drawing to DWG