How to Surface Model a Shoe Horn in Fusion 360 (for 3D Printing)

by the end of this video you'll know how to surface model a shoehorn in fusion 360 hey there it's Kevin Kennedy and welcome to the product design online YouTube channel where I demo all things fusion 360 if you're new here be sure to hit that red subscribe button and go ahead and comment below and let me know what you plan on using fusion 360 for if you're not familiar a shoehorn is a curved instrument that's used to ease your heel into a shoe and they're particularly helpful when you're trying to put on dress shoes or loafers as they help you slip the shoe on without stepping on or creasing that back heel now I used to have a shoehorn but it always seems to go missing so I decided it would be fun to model one so I can 3d print a new one so to get started you'll want to enter the patch workspace I'll simply select the workspace drop down list and then select the patch option you could use the loft command in the model workspace but because this is a fairly thin object with some curvature to it I decided it would be easier to use the loft command in the patch workspace the loft command in the patch workspace allows you to create thin surfaces with no real thickness and we can thicken the surface at the end the benefit of this is that we don't have to worry about a closed profile shape getting messed up or causing any errors while working with the loft command so to start off I'm going to draw up the spline that we'll use as the lofts centerline I'll hit the keyboard shortcut letter s as in Sierra to call the sketch shortcuts box I'll type out fit point spline and I'll click on the fit point spline option to activate the spline command then I'm going to select the Y Z origin plane as the plane to start the sketch on shoehorns come in all different shapes and sizes so I'm just going to draw a simple spline curve and then I'll dimension it to the size that I want and of course you can use whatever dimensions you desire I'll start off by clicking on the origin point for the first point of the spline then I'm going to click a second point a little bit higher and for the third and final point I'll click on the x-axis and I'll simply click the enter key on the keyboard to confirm the results and to escape the spline command the first dimension I want to add is the overall dimension of the shoehorn I'm going to hit the keyboard shortcut letter D as in Delta to activate the sketch dimension tool then I'll simply click on the first point of the spline and the last point of the spline the dimension input will appear after I click to set the dimension in place I'm going to type out 13 centimeters for the length and I'll hit the enter key with the dimension tool still active I'm going to add a second dimension I'll click on the first point and then the second point and this time I'm going to drag my mouse straight up so I can add a distance for the length between each point I'll type out 50 millimeters and click the enter key lastly I want to add a dimension of 16 millimeters to the height of the spline I'll click the first point and the second point but this time I'll drag the dimension tool to the left which will let me plug in a height or the dimension of 16 millimeters we now have the spline that we'll use for the lofts centerline since we're done with this sketch I'll go ahead and hit the stop sketch button in the toolbar at this point I want to create a curved shape for the front of the shoehorn now I want to ensure that it's drawn at the beginning of the spline so I'll want to create a construction plane that's attached to the splines starting point I'll select the construct drop-down list and I'll select the plane along path then I'll select b-spline as the path and I can either type out zero for the distance or I can drag the blue directional arrow to make sure that the plane is at the starting point of the spline finally I'll click OK to confirm the location now we're going to need another plane at the other end of the spline for the second profile so I'll right-click and select repeat plane along path I'll select b-spline once again and then I'll drag the blue directional arrow until the construction plane is at the endpoint of the spline and of course then I'll click okay let's go ahead and draw the front curve of the shoehorn I'll select create sketch in the toolbar and then select the construction plane at the front of the spline so create this curve shape I'm going to use the three-point arc from the sketch drop-down list I'll select the arc flyout folder and then I'll select the three-point arc I'm just going to draw the arc out above the origin point and then I'll dimension the arc and constrain it into place I'll click once to the left to place the first point and I'll click a second time to place the second point of the art and I'll click a third time to place the third point which defines the arcs curvature next I'll constrain this art to the origin point or this first point of the spline that way the profile in the paths are connected which is required for the loft command I'll select the midpoint constraint from the sketch palette or if you're using the new UI preview you'll need to select the midpoint constraint up here in the toolbar to apply the constraint I'll select the art and then select the origin point and you'll see that the midpoint of the art is snapped to the point and this triangle signifies a midpoint constraint once again I'll hit the keyboard shortcut letter D as in Delta to activate the dimension tool for this dimension I'll select both endpoints of the arc and type out 50 millimeters with the dimension tool still active I'll select the first point and the origin point and drag my mouse cursor to the left this will let me add a dimension for the height and I'll type out ten millimeters for the height to fully constrain this sketch I'll repeat these steps on the other side with the dimension tool still active I'll select the other end point of the arc and the origin point I'll drag my mouse cursor to the right and this will let me add a dimension for the height and I'll type out ten millimeters now this first sketch profile is now done so I'll select the stop sketch button in the toolbar I'll hit the Home icon next to the view cube to take a look at this model from the home position before we use the patch workspace loft command we'll need to draw the second profile at the end of the center line because the loft command requires a minimum of two profiles one thing that I want to point out real quick you'll notice that the first construction plane disappeared and that's because by default fusion 360 assumes that after you finish a sketch you're done using that plane for the time being if you would like to you can change this and your preferences otherwise if all you need to do is use it later on in the model you can simply turn it on by hitting the corresponding light bulb in the fusion 360 browser let's create a sketch on the second construction plane I'll right-click on the sketch plane and I'll select create sketch for this profile I'm going to simply draw a straight line I'll select the line tool from the sketch drop-down list then I'll click twice to draw a line above the splines endpoint once again I'll select the midpoint sketch constraint from the sketch palette and I'll click the line and the endpoint of the spline I'll hit the keyboard shortcut letter D and I'll add a dimension by selecting the line for this dimension I'll type out 30 millimeters and then I'll select stop sketch in the toolbar we now have the framework finish for the loft command so I'll activate the loft command by selecting it from the create drop-down list for the first profile I'll select the arc and for the second profile I'll select the straight line that we just created you'll see that the loft command is already connecting the two profiles so we'll need to add our spline as the center line I'll select center line as the guide type because this rails option would be used if our path wasn't directly down the center then I'll select the plus symbol in the rail section of the dialog box and I'll select the spline in the canvas window now before hitting okay I'll change the operation to new component so we can move all the bodies that we create to be nested under this component and I'll go ahead and click OK if I toggle open the component in the bodies folder in the fusion 360 browser you'll see that the surface body icon is next to the body name you can also tell that we have a surface body because the face is yellow instead of gray because surface bodies technically have no real thickness to them we'll need to use the thicken command to make this an object that we can actually print out I'll select the thicken command near the bottom of the create drop-down list then I'll select the face if it isn't automatically selected and I'll type out a dimension of three millimeters for the thickness followed by hitting the OK button in the dialog box one of the last things we need to do to our model is round over the corners so the shoehorn can actually be used I'll hit the keyboard shortcut letter f as in Foxtrot to activate the Phillip command then I'll simply select the front two corners of the shoehorn and I'll type out 12 millimeters for the Filat radius one of the nice things about the Phillip command is that it was recently updated to allow you to create multiple fill 'its with a different specified radius to do so I'll click the plus symbol to add a new selection and this time I'll select the back two edges of the model type out sixteen millimeters for the fill it radius after selecting the back edges and then I'll click OK in the fill it dialog box we'll also want to add a fill it to the edge of the shoehorn so I'll right-click to select a repeat fill it now the reason I'm making this a different Philip command is because if I click the edge now it will select all the way around the object whereas before it wouldn't let us do that because the other Philip commands would affect it I'll make sure both the top and the bottom edges are selected and I'll type out a dimension of 1.5 millimeters before clicking okay in the fillit dialog box now the last thing that I want to do to the shoehorn is add a hole near the top so a string can be added all head up to the construct drop-down list and this time I'll select plane tangent to face that point this type of construction plane lets us create a plane using the face of some geometry while using the point to dictate the direction that the plane faces I'll select this top face of the shoehorn and then for the point I'll select one of these two end points of the fill it radius and then I'll click OK I can now create a center circle by selecting C as in Charlie for the center circle command I'll select the construction plane that I just created and I'll click on the y-axis to place the circle as I drag out my mouse you'll notice that I can type out the dimension I'll type out five millimeters followed by the tab key to lock the dimension in place then I'll click to set the circle lastly I'll hit the Escape key to exit the circle command I'll right-click to select the sketch option in the marking menu and then straight to the left I will select the sketch dimension tool I'm just going to add a dimension from the center point of the circle to the end point and I'll make this 10 millimeters all we have left is to cut out the hole so I'll hit the letter e as an echo to call the extrude command I'll select the circle I'll drag the directional arrow down which changes the operation to cut and then I'll change the extent to all and I'll click OK in the dialogue box I selected the all option in case I was to go back and change the thickness of this model later on then the whole cutout will always remain cut out and I won't have to worry about updating it the last thing I'll do is toggle open the bodies folder in the fusion 360 browser and I'll drag the body down so it's nested under the component I'll also go ahead and do this with the sketch folder as well so everything is nested neatly under this same component which helps if I want to make copies or if I wanted to insert this into another design to 3d print this model all you'll need to do is simply right click on the component and click save as STL then from the save as STL dialog box you can select your slicing software which will output the file directly to it or you can save the file to your local machine if you have access to a 3d printer and you're going to print this out then go ahead and let me know in the comments below I'd love to hear what type of printer you have and what type of settings you use and of course if you have a photo of the finished object go ahead and link to that below thanks for watching if you have any questions at all about this tutorial or fusion 360 questions in general then be sure to comment them below hit that thumbs 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Channel: Product Design Online

Views: 28,215

Keywords: 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, fusion 360 surface modeling, fusion 360 surface modeling tutorial, fusion 360 surface pro, fusion 360 shoe horn, fusion 360 3d printing nerd, fusion 360 3d printing for beginners, 3d printing, 3d print, 3d printer, 3d software

Id: cTaMbTTz5PQ

Length: 15min 22sec (922 seconds)

Published: Fri Feb 08 2019