How to 3D Model a Screwdriver in Fusion 360 - Learn Autodesk Fusion 360 in 30 Days: Day #14

hey there it's Kevin Kennedy and welcome to day number 14 of the learn fusion 360 in 30 days by the end of this tutorial you'll be able to 3d model your very own screwdriver which of course could be 3d printed and actually used we'll take a look at how to create components driven off of previous components and we'll cover the three-point arc sketch feature we're going to start off by modeling the handle of the screwdriver as one component and then we'll create a second component for the shank of the screwdriver so create a new component I'll select new component from the assemble drop-down list and I'll double check that empty component is selected before we hit okay we'll follow rule number two of fusion 360 which is to always name your bodies and components I'll type in handle for the name make sure activate is selected so we can start working on the component right away and I'll click OK and the new component dialog box now let's start to create the handle by using the cylinder tool from the create drop-down list after selecting cylinder I'll click on the front face click on the center origin drag out with my mouse and then I'll type in 28 millimeters for the width I'll hit the tab key to lock the dimension in place and I'll click with my mouse to snap the circle in place then I'll make the length 100 millimetres and click OK to exit the cylinder feature and before we do anything else I'll rename the body cylinder by double-clicking on it in the fusion 360 browser and I'll type out cylinder I'll also click on the Save icon type out slot head screwdriver for the name and I'll click the blue Save button at this point we could leave a basic cylinder shape for the handle but it would work better and be more ergonomic if we cut some grooves in it to do this I'll look at the handle from the backside then I'll hit the keyboard shortcut letter C for Center circle and I'll click on the back face of the handle what I want to do here is draw a circle extrude cut it and then I'll pattern the cut feature around the handle so I'll just click on the left side here at the edge of the handle where the centre circle function will snap into place and I'll make this circle six millimeters now I'll hit the keyboard shortcut letter e for extrude and we'll extrude cut this 75 millimeters and then I'll click OK to exit the extrude command I'll activate the circular pattern feature located in the pattern folder under the create drop-down menu you'll see that after we activate the pattern feature we can select the pattern type I'll select features as the pattern type and then I'll select the extrude feature in the timeline below for the axis I'll select the center axis of our handle and remember if you ever can't select the axis here in the canvas because it's blocked by a body you can select the axis in the fusion 360 browser now we want this pattern to go all the way around the handle so I'll make sure full is selected as the type and then we'll set 6 for the quantity or the number of times to pattern looking at the model we can see a faint preview of the pattern but let's go ahead and click OK to see the results now one thing to note here we could have used the sketch circular pattern and pattern the circle around before we extruded it but I recommend using the pattern feature under the create drop-down list when possible as it will perform much better in fusion 360 especially when dealing with larger and more complex patterns and assemblies now the main reason is because the sketch tool is trying to render all of the geometry whereas if you look at the sketch of our pattern feature it's simply rendering the one circle and the pattern feature is mimicking the extrude cut at this point I want to add a nice Filat or rounded edge to the back of the handle I'll select the keyboard shortcut letter F to activate the fill it command I'll select all six of the outside edges and ten millimeters for the distance and of course you can always type in more or less here it really just depends on how much you want the back of the handle to be rounded over well click OK to exit the Phillip command now I want to add a rounded divot to the front of the screwdriver to our thumb and forefinger have a nice and organized to rest I'll right-click on the Y Z plane in the fusion 360 browser and I'll select create sketch we're going to use this center plane because we're going to draw an ellipse and then we'll we'll revolve it around the cylinder I'll select the ellipse tool from the sketch drop-down list and I'll click just above the handle now I'm not sure exactly how far down and once ago so I'll just go down six millimeters and I'll go to the right about 21 millimeters as we can always go back and change the dimensions now I'll select the revolve tool from the create drop-down list I'll select the ellipse we just created as the profile and once again we'll select the center axis of our handle I'll make sure that my operation is set to cut and I'll click OK to see the results now looking at this divot I may decide that I want to go down a bit further if so I'll double click on a sketch in the timeline to edit the ellipse and I'll change the height here to 8 millimeters I'll hit stop sketch and take a look at the new results all righty so our handle is coming along nicely so far the last thing we'll want to do is add some nice Phillips or rounded edges to it and then we'll proceed on to make the shank and tip of the screwdriver I'll hit the keyboard shortcut letter F to activate the Phillip command and I'll select the front circle of the screwdriver I'll add a Filat of 1.5 millimeters and click OK I'll hit letter F again and I'll select these circles on each end of our divot and I'll make these one millimeter and click OK lastly we'll go ahead and add some nice rounded edges to our grips here clicking letter F to activate the fill command I'll select all six of the grip edges and then I'll punch in two-and-a-half millimeters for the Filat distance I'll click okay and then I'll right-click on the edge here and I'll select repeat fill it I'll select all six of these corresponding edges I'll make this edge round it off with one millimeter and then I'll click okay now the last thing we'll want to do with our handle before we're done with the component is to add a hole for a screwdriver shank I'll hit the keyboard shortcut letter H for hole and I'll click on the front face of our handle now the hole should have snapped to the center origin you'll see if I drag this hole around it will snap right into that Center origin point we wonder hold to go half way into the handle and the whole dialog box I'll make the length 50 millimeters I'll make the width of the hole seven millimeters and then I'll change the drill points of flat okay to exit the whole command and we are now officially done with the handle of our screwdriver at this point we'll want to create a new component for the shank of our screwdriver but first we'll want to activate the top level component so our new component is nested within it to activate it I'll click on the little circle to the right of our file name and once activated I'll select new component from the assemble drop-down list and I'll rename this one shank and click OK now you'll see in the fusion 360 browser that the shank and handle components are nested underneath the screwdriver assembly I'll make sure that the shank component is active before we start doing any work and then I'll select the face of our hole this way if we change the whole dimension later on our sheykh dimension will update accordingly just like we talked about in day number 13 I'll hit letter e for extrude and then I'll make the distance 150 millimeters and click okay now let's click on the circle next to the handle component to reactivate it and we'll take a look at our hole size I'll double click on the whole feature and change the width to 10 millimeters and then click OK then I'll reactivate our assembly and you'll see that the width of our shank did update accordingly as we expected I'll go ahead and click undo to revert back to the original size now all we have to do is create our screwdriver tip which will create a new component for this time I'll use another method I'll right-click on the top assembly and select new component I'll double click on the component in the browser and type in tip for the name I'll select the front face of the shank and click letter e on the keyboard for extrude and I'll punch in ten millimeters for the distance I'll make sure new body is selected and then I'll click OK and before I forget I'll find the body in the browser and rename it to slot head tip now we're going to create the slot or flathead tip by cutting out the cylinder from the side I'll right-click on the Y Z plane and select create sketch then I'll activate the three-point arc from the sketch drop down list for the first point I'll select the front edge here where it snaps in place I'll select the top line where it snaps in place and then I'm just going to put the third point where it creates that nice art of the flat head now at this point will went to fully define our sketch so we don't mess it up if we change dimensions and any of our other components I'll hit letter D to activate the dimension tool I'll click on the end of the three-point arc here I'll click on the center origin of our tip and I'll make this 0.5 millimeters and then hit the Escape key to exit now you may have noticed that the other end point moved down so I'll select this end point of the arc and holding down shift I'll select the corner of the cylinder now I'll click on the horizontal constraint icon this way it's always in line with the thickness of the tip even if we change our dimensions now in order to extrude cut the shape we'll have to close off our profile so we can hit letter L for line and then draw a horizontal line and we can also draw a vertical line connecting the endpoints once again before we cut this we'll also want to make sure that all of our lines are black indicating that they are fully constrained using D on the keyboard for dimension I'll select the horizontal line and I'll make this nine millimeters then you'll notice that the arc is still blue because we can dimension the radius of it so we'll click on the arc and then hit enter and you'll see after that our profile is fully constrained as it has black lines all the way around I'll hit letter e for extrude select the profile and I'll change the direction here two two sides will need to change the operation to cut and for the extent of each side will select all now the reason we're selecting all is again for the purposes of our dimensions if we decided to make this shaft thicker then our cut here will update accordingly and we won't have to go back and manually edit this extrude feature I'll click OK to exit the extrude command and now we'll want to select mirror from the create menu well change the pattern type to features and we'll select the extrude in the timeline for the mid plane I'll select the XZ plane in the browser and then I'll click OK to take a look at the results now we're essentially done with our slot head screwdriver we can reactivate the top level component to take a look at it and of course we can always select a component hit letter a for appearances and we can drag and drop the appearances onto each component you thanks for watching if you have any questions at all about this tutorial or any fusion 360 questions in general then be sure to comment them below hit that thumbs up icon if you learn something in this video and click Subscribe - followed by that little bell icon to be notified of more fusion 360 tutorials

Channel: Product Design Online

Views: 51,763

Keywords: fusion 360, autodesk fusion 360, kevin kennedy fusion 360, product design online, fusion 360 tutorials, fusion tutorials, fusion 360 30 days, learn fusion 360 in 30 days, lars christensen fusion 360, fusion 360 beginners, fusion 360 kevin kennedy, autodesk fusion 30 days, #larslive, learn fusion 360 or die trying, 3D model a screwdriver, how to 3d model a screwdriver, screwdriver fusion 360, flat head screwdriver fusion 360, fusion 360 screwdriver tutorial, screwdriver f360

Id: 29kCwkapes4

Length: 14min 46sec (886 seconds)

Published: Tue Aug 14 2018

Reddit Comments

[u/ITinSeattle]

Appreciate these videos. Thanks.

[u/ArtofMelC]

Thanks for sharing Kevin. First time viewing your tutorials and I really like the pacing and content. Looking forward to following the full 30 days and improving my Fusion 360 knowledge.

[u/productdesignonline]

Day #14 was just posted! Anyone else got a 3D printer?? Let me know if you 3D print this! Cheers, Kevin

[u/Slowmac123]

This might help me. I just started f360