HOW and WHY to Fully Constrain Your Sketches - Learn Autodesk Fusion 360 in 30 Days: Day #17

hey there it's Kevin Kennedy and welcome to day number 17 of learned fusion 360 in 30 days by the end of this tutorial you'll have a solid understanding of how to use dimensions and constraints to fully constrain your sketches you'll learn a few dimension tricks and I'll explain in demo why it's important to fully constrain your sketches let me start off by stating that fusion 360 does not require sketches to be fully constrained but it's a good practice to always fully constrain your sketches which we'll cover in just a minute but first it's important to note that the way you define or constrain your sketches will differ per each design this is why it's important that you come up with a strategy for how your sketch entities relate to one another at the beginning of each model now this strategy is often referred to as the sketches design intent personally I recommend sketching out your design on pencil and paper before you start sketching anything out in fusion 360 doing so will help you think about how the sketch should be constrained before you even get too caught up in the computer now for this demo I went to draw this square washer plate which is essentially a square with a hole cut out of the middle while looking at this sketch I can ask myself what do I know about this object without knowing any of the dimensions I see that all four sides appear to be equal I see that the lines are perpendicular at the corners and the lines opposite of each other appear to be parallel and it appears that the center of this circle is located directly in the middle of the washer plate so let's start off by creating a new component from the assemble drop-down list and I'll title it square washer and click OK now let's create a sketch for this washer plate so we can walk through the steps of constraining and dimensioning it I'll hit the keyboard shortcut letter R for rectangle and I'll select the top plane now before we click on anything if you look in this sketch palette you'll see that we can switch from a two point rectangle to a three point rectangle or a center rectangle for this washer plate we'll want to use the center rectangle because the center rectangle will already have a nice center point for us to reference for the circle cut out this is why as you continue to learn fusion 360 it's important that you understand what all of the sketch tools do the more you know you'll become more efficient and it will help you eliminate unnecessary steps so I'll select the center rectangle icon and I'm just going to click away from the origin out in space here and I'll drag out with my mouse and click at a random distance and just so you can see the difference I'm going to select a two point rectangle and draw that out right next to our center rectangle and I'll hit the Escape key to clear all commands now let's look at both of these rectangles so you'll notice a few things here as I mentioned in day number 16 you'll see that fusion 360 will automatically apply some constraints when using these predefined sketch entities now using the two-point rectangle tool applied vertical slash horizontal constraints to all four lines now here's a little tip for you if a constraint is automatically applied and you can't seem to remember what it stands for then simply click on the glyph or icon and you'll see in the lower right hand corner it states the type of constraint you'll see this one says horizontal and if I click on this one for the right line it states that it's a vertical constraint now looking at the center rectangle we created you'll see that it automatically created some different constraints for us it created some parallel constraints a coincident constraint or the lines meet in the middle and a perpendicular constraint in the corner now that you see the difference here I'm going to delete the two-point rectangle by selecting over the entire object and then I'll hit the Delete key on my keyboard as we go a bit further you'll understand why we ended up going with the sender rectangle now we'll once it fully constrained or define the center rectangle before we go ahead and turn it into a three-dimensional object that way we have 100% control of the sketch if we go to update the size of the sketch or change anything with the square washer plate so in this current state you'll notice that the lines of the rectangle are blue which means that they're not fully constrained and we can still move them around now if I click and drag on these lines you'll see that I can move them up and down side to side or I can drag points and change the overall size of the rectangle so our goal here is to figure out how to turn all of these lines from blue to black because black sketch entities signify that they are fully constrained and they can't be moved unless we update the dimension or the constraint that is driving the sketch again doing this will give us full control of the sketch so if we update the size we can keep the shape that we originally intended now the rule of thumb is to always use constraints first and then dimension your sketches second and there are a few different reasons for this first the fewer amount of dimensions we have the easier it will be to update the size of our model should we need to second the fewer dimensions we use the fewer amount of problems will likely run into such as accidentally over defining our sketch which means that the dimension cannot be altered because it's already driven by other dimensions and/or sketch constraints so if we look back at our original sketch notes we'll see that it appears that all four sides are equal therefore using the equal sketch constraint we can force all four lines of our rectangle to always be equal so holding down the shift-key i'm going to select the left line and the top line of the square and i'm going to click on the equal constraint in the sketch palette now the reason I only applied the equal constraint to the left and top line is because they already have parallel constraints if I reactivate the equal constraint and select the other two lines you'll see that it won't let us add the equal constraint to all four lines because it would over constrain the geometry making those constraints unnecessary now you'll notice that the lines of our rectangle still aren't fully constrained because they're still blue so if you're ever wondering why they aren't fully constrained you can simply click on any lines or points and drag them around if I click and hold on the center point of the rectangle you'll see that I can drag it around now we can use the coincident constraint to snap the center of the rectangle to the center origin I'll activate the coincident constraint click on the center origin and then I'll click on the middle of the rectangle and you'll notice the rectangle will snap to the center origin now you should also notice that the center construction lines and the center point of the rectangle are now black or fully constrained so if I click-and-drag at the center point I can no longer move this rectangle around but we can still change the size of the rectangle by dragging the blue lines which aren't fully defined yet now one thing to know I normally would have started the center rectangle sketch off the origin point but for this demo I wanted to show you what happens when you don't with that said I would always recommend starting your first sketch of each file at the center origin unless you have a good reason not to now let's go ahead and fully constrain the lines that are still blue to do this we'll have to add a dimension to one of the sides so I'll hit letter D on the keyboard for dimension and if I click on the top line drag up with my mouse and type in 100 millimeters and click enter you'll see that now our sketch is 100% black or fully constrained and I can't change the size or move any of these lines by dragging them around now the only way I can change the size is by changing this one dimension that we just added now let's go ahead and add our circle cut out in the middle I'll activate the center circle sketch tool with the keyboard shortcut letter C I'll click on the center origin point type in 50 millimeters for the dimension and I'll click with my mouse again to snap the circle into place now you'll see that our circle is also represented as fully constrained with black lines because the dimension we added and the fact that we drew it on the center point which automatically added a coincident constraint now to delete a constraint that is automatically applied all you have to do is click on it and hit the Delete key if I click on the middle of the circle you'll see that there are four different coincident constraints and if I hover over the glyph of each one you'll be able to see what it relates to I'll select the second constraint and then I'll hit the Delete key and now you'll see that the circle is blue because I can move it around so I'll go ahead and reapply a coincident constraint by activating coincident in this sketch palette I'll click on the center origin now let's go ahead and extrude our square washer up by hitting the keyboard shortcut letter e for extrude I'll select the sketch and type in five millimeters for the thickness and click OK at this point I want to show you a few dimension tips I'll double click on the sketch in the timeline to reopen it and if I hover over the dimensions you'll notice that it gives the dimension number so we have d1 : 100 millimeters where the number 1 represents the dimension number so if we hover over the circle dimension you'll see that the dimension number is number 2 and these numbers are created based on the order in which you dimension entities now one cool thing about dimensions is that we can use functions in the dimension field to make them a bit more robust so if I knew that I always wanted this inner circle cut out to be half the size of my overall square I could apply a function to always be half of the squares dimension to do this I'll click on the circle dimension and I'll type out d1 to reference the first dimension or the dimension of the outer rectangle I'll type a forward slash to represent that I want to divide and then I'll type out number two because I wanted to always be cut in half or half of the rectangle now if I click enter you'll see it says FX for function and it shows the diameter of 50 millimeters now if I were to update the original dimension to 150 millimeters you'll see that the circle dimension updates as well so now it's automatically been changed to 75 millimeters so once again this is why it's super important to think through your designs before you start sketching anything out on the computer I'll also point out that you have to use functions like this with caution you don't necessarily want to reference dimensions all the time especially in larger models or sketches as it can get quite hard to remember what each function or dimension actually represents now to summarize what we did here we added constraints first so we only had to add two dimensions to fully define and constrain our sketch which allows us to easily go back and simply change one dimension if we decided our square washer needs to be smaller or larger if we take a look at this other file I've gone ahead and created the same washer but I didn't follow these best practices and you'll notice if I double-click to open up the sketch the sketch is not fully constrained or defined now if I go to update the dimension you'll see that it totally throws off the whole entire shape and I'd have to also manually update the other dimensions here now it may not seem like that big of a deal because this square washer is a fairly simple object but as you can imagine as you start to 3d model more complex objects especially ones that contain multiple sketches it can really suck up a lot of time and cause a lot of problems if you don't plan ahead and fully constrain your sketches based on your original design intent now the last thing here be sure to check out the comment section below where I'm gonna post three helpful tips that you should always follow when working with sketches thanks for watching if you have any questions at all about this tutorial for 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: 45,732

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, learn fusion 360 or die trying, how to fully constrain sketches in fusion 360, fusion 360 fully constrain sketch, fusion 360 dimensions, fusion 360 dimension constraints, fusion 360 constraints explained

Id: C11L136U0vQ

Length: 15min 1sec (901 seconds)

Published: Thu Aug 23 2018

Reddit Comments

[u/productdesignonline]

Be sure to watch to the end where I show how to use functions in conjunction with the dimension tool ;)