Demo File
Dimension Sketches Demo File
Note: The file is not empty. Fusion 360 hub doesn’t show sketches on preview. Click the blue download button, select download .f3d and then enter your email. Within a minute or two you will receive an email to download the demo file.
Learn About Constraints
How to Manually Add Sketch Constraints in Fusion 360
HOW and WHY to Fully Constrain Your Sketches
7 Tips that Will Make You a Dimension Expert
1. Change Diameter or Radius
The first pro tip is that you can change each radius dimension types to a diameter, or vise-versa.
Simply right-click on a radius dimension that was applied (by default) to the arc. Then, click on the option that says “toggle Diameter”. You’ll then see the arc has the diameter applied.
Fusion 360 will automatically double the radius value, leaving you with the same dimension.
Of course, to switch from a diameter dimension to a radius dimension you’ll simply need to follow the same steps to select the “toggle Radius” option.
2. Hide or Show Sketch Dimensions
The second pro tip is that you can hide or show your sketch dimensions. To hide your sketch dimensions simply click the corresponding “dimensions” checkbox in the Sketch Palette. If the “dimensions” option is unchecked, then your dimensions will be hidden. Of course, if the box is checked then your sketch dimensions will be visible.
The ability to hide dimensions can come in handy if you’re trying to work solely with constraints or to finetune details of busy sketch geometry.
You’ll also notice just below the dimension option that you can toggle sketch constraints on and off as well.
3. Driving vs Driven Dimensions
The third pro tip is that you can create driven dimensions.
“Driving” dimensions are dimensions that “drive” the shape or size of the sketch geometry based on the values inputted.
Contrary, you can create “Driven” dimensions, which are dimensions used simply for reference purposes. In other words, they won’t alter the sketch geometry, but they themselves will be updated as you change the “driving” dimensions.
Notice that “driven” dimensions have parentheses around them.
An important thing to note with driven dimensions is that sometimes you’ll be warned that they will be automatically applied. For example, if you remember earlier in this lesson (demo file and tutorial above), we added equal constraints to the small circles so we only needed to dimension the one on the left-hand side.
You may find that you want to apply a driven dimension to the circle on the right-hand side so you’re reminded that the circle has the same dimension. However, this is by no means something that is required or necessary.
While trying to add a “driving” dimension Fusion 360 will warn you if the dimension must be “driven” instead. When the warning message pops up, simply click the “OK” button to add the driven dimension.
4. Dimensions are Numbered
The fourth pro tip is that dimensions are automatically numbered. Notice as you hover over a dimension that the dimension has a number applied to it. This dimension number can be used in the input field of other dimensions.
Note: there is a number right after the letter “d”
For example, if you click on a line and then type out the letter “d” and the number value of another dimension, then that other dimension will be applied (the same numerical value). Because the dimension is derived from another dimension you will see the function symbol before this newly created dimension.
5. Dimensions Can Include Equations
The fifth pro tip is that you can create equations within the dimension input field. You can type out any legitimate equation within the input field.
For example, if you double-click on a dimension you can type out the following equation in the input field: (2+3+5)*(4+6)*1
Notice when you hit the “enter” key on your keyboard that the equation equals 100.
Obviously, there’s no reason to enter equations if you know the final value should be 100mm. However, equations can be extremely helpful if you only know other dimensions of the model. Simply type out a relevant equation and let Fusion 360 do the math for you!
It’s also important to note that if you receive any red text while typing out an equation then that means something in your equation is not valid
6. Dimensions Can be User Parameters
The sixth pro tip is that you can use any user parameter values within the input fields. Doing so will make your model more dynamic. See the tutorial videos below tip #7 for examples and step-by-step walkthroughs.
Anytime you update a user parameter, the dimension will be updated accordingly. The user parameter can be reused in multiple dimension fields, making your dimensioning efforts more efficient.
7. Rename Your Sketch Dimensions
The seventh pro tip is that you can rename sketch dimensions. To rename sketch dimensions you’ll need to open the change parameters dialog.
Select “Change Parameters” in the toolbar (Sigma icon). Then, toggle open the file name folder, and the sketch folder. You’ll then see that all the dimensions within your file have automatically been added to the list. From there, you can edit the dimension name, typing out a text string instead of its default number.
The benefit to this is that it can be easier to remember instead of keeping track of all of the numbers, should you want to call your current dimensions by a name.
After changing a dimension’s name you will notice that the dimension name appears instead of “dx” (x = dimension number).
User Parameters Tutorials (Dynamic Models)
Tutorial Transcript:
By the end of this video, you’ll know how to use the sketch dimension tool in Fusion 360.
The sketch dimension tool can be activated from the sketch dropdown list, where you’ll find it at the very bottom of the list. It can also be activated with the keyboard shortcut letter “D,” as in Delta. You can activate it from the right-click sketch menu in the sketch flyout folder… and lastly, from the marking-menu by right-clicking, selecting the sketch menu at the bottom, and then by dragging your mouse directly to the left.
It’s important to note that the sketch dimension tool should not be confused with the measure tool, which you’ll see in the toolbar or in the inspect dropdown list. The measure tool is solely for inspecting the dimensions of your model…not adding dimensions.
To follow along with this tutorial, you’ll want to grab the free demo file on my website. To check it out go to ProductDesignOnline.com/6…that’s ProductDesignOnline.com/6 and that URL will automatically redirect to the page with the demo file and some additional resources.
I’ll now hit the keyboard shortcut letter “D,” as in Delta to activate the sketch dimension tool. You’ll follow the same workflow every time you need to create a new dimension.
First, simply click on the sketch geometry that you would like to dimension. I’ll click on the bottom line. Then, as I drag my mouse cursor away from the line, you’ll notice the sketch dimension appears. To place the dimension you’ll need to click with your mouse, which then immediately opens the dimension input field. At this point, I can either type out a numerical value or I can simply click the enter key if the dimension is already set to the desired value. You can also type out equations and a few other things in the dimension input fields, so be sure to stick around to the end where I’ll demo 7 sketch dimension tricks that will make you a pro at adding dimensions.
For now, I’m going to hit the enter key on my keyboard to place the dimension.
If you want to move your dimensions around, at any time, you’ll simply need to click anywhere on the dimension line and then you can drag the dimension around. Notice how the dimension value follows my mouse cursor around as I move from side to side… giving you the ability to place the value in a better location, which comes in handy when you have dimensions running into each other.
After creating a dimension the sketch dimension tool will remain active, which is indicated by the sketch dimension icon next to the cursor. This lets you quickly create another dimension without having to re-activate the command each time. Otherwise, you can hit the escape key on your keyboard to clear out the command.
For the first dimension example, I simply clicked on the bottom line. However, another common use case of adding sketch dimensions would be selecting two points and then dimensioning the distance between the two points. I’m going to click on this left-middle corner of the geometry and then I’ll click on the corner where the circle meets the horizontal line.
Watch what happens as I drag my mouse cursor around. You’ll notice there are three different ways that I could dimension the distance between these two points. I could do the width, height, or the angle. For now, I’ll simply drag straight up and I’ll click to create the distance between these two points. I’m going to type out 15mm and then I’ll hit the enter key on my keyboard.
Now you may have noticed that the line on the right side updated as well. This is because of the constraints that are currently applied to this sketch…which leads me to one of the most important practices when creating sketch dimensions.
In general, as you dimension sketch geometry, you want to consider how you can dimension your sketches with the fewest amount of dimensions as possible. In order to do this, you’ll have to apply constraints to your sketches, so it’s very important that you understand how to constrain your sketches. Click that info icon in the upper right-hand corner to watch a video on sketch constraints. I’ll also add the video to the resource page for this tutorial.
Let’s now quickly take a look at an example of this. Notice how there are two small circles on this sketch, that appear to be the same size. If I wanted to ensure that the sketches were always the same size then the best practice would not be to dimension each circle as the same dimension. I would actually want to first add the equal constraint to the circles and then dimension one of them.
I’m going to hold down the shift key on my keyboard and then I’ll select the small circle on the left…and I’ll select the small circle on the right. Once they’re both selected I’ll select the “equal” constraint icon in the sketch palette… or if you’re on the new UI then you can select the equal constrain up here in the toolbar.
You’ll see that each circle now has an equal constraint next to it. I’ll now hit the keyboard shortcut letter “D,” as in Delta, to activate the dimension tool. Then, I’ll click on the left circle and I’ll click once again to set the dimension.
I’ll type out 10mm for the circle’s dimension. Now pay close attention to what happens to the circle on the right as I hit the “enter” key on my keyboard to place this dimension. You’ll notice the circle on the right updated to 10mm as well, because of the “equal” constraints.
To summarize why this is so important, imagine being able to change only a handful of dimensions to update dimensions all across your model versus updating a dimension for every single piece of sketch geometry in your model.
As you can imagine, more complex sketches could start to get out of control, and it would be hard to keep track of all the dimensions, which is why it’s crucial that you attempt to use sketch constraints first and then apply the fewest amount of dimensions possible, which “drive” the sketch.
At this point, we’ve taken a look at how to dimension the diameter of circles and linear lines. Let’s now take a look at how to dimension angles between lines.
With the dimension tool still active, I’ll select the left vertical line and then I’ll select the adjacent line. As I drag my mouse cursor out you’ll notice that it creates a degree input field for the angle. Notice how I can dimension this angle in four different directions, based on the lines of this sketch geometry.
I’m going to click on the inside of this obtuse angle to make it a bit larger. I’ll type out 145 degrees and then I’ll hit the “enter” key on my keyboard. This time you may have noticed that the right side did not automatically update, and that’s because there are no constraints applied that are forcing that to happen. So again, I can’t emphasize enough the importance of adding constraints before dimensioning. You can add constraints after dimensions, but you’ll find it more efficient to add them all at the beginning.
Next, let’s take a look at defining the radius of an arc. I’ll make sure the sketch dimension tool is still active and then I’ll click on the arc at the top of this sketch. After I click to place this dimension and hit the “enter” key to set the radius, you’ll notice there is the letter “R” in front of the numerical value.
The letter “R” stands for “Radius,” whereas, the letter “D” for the small circle below stands for the “Diameter” of the circle. Arcs will always default to be dimensioned by their radius, along with sketch fillets. Contrary, circles will always be dimensioned by their diameter. Keep this in mind as you create sketch dimensions… it can be easy to type out the diameter when you’re really applying the radius or vice-versa.
Now that you know how to apply a variety of sketch dimensions, it’s important to note that all of these dimension types are parametric, meaning you can change the dimensions at any time. To edit a dimension simply double-click on the dimension to open it back up. Then, type out a new value before hitting the “enter” key on your keyboard.
I’ll double-click on the dimension for the small circle. I’ll type out 12mm for the new value and then I’ll hit the “enter” key on my keyboard. You can update dimensions at any time as you work on your model, letting your model adapt to changes in your requirements.
Now that you’re familiar with the sketch dimension basics, let’s take a look at 7 tricks that will make you a pro at creating sketch dimensions in Fusion 360. Before we get started, I’ll quickly point out that I’ve added all of these on the resource page for this tutorial so you can bookmark the page and quickly reference them later on.
If you remember earlier, I pointed out the arc had a radius dimension by default and the circle had a diameter dimension by default. For pro tip #1 I’ll show you how you can change each dimension type to one or the other.
I’ll right-click on the radius dimension that was applied to the arc. Then, I’ll click on the option that says “toggle Diameter”. You’ll now see the arc as the diameter applied and Fusion 360 automatically doubled the radius value, leaving us with the same dimension.
Of course, to switch from a diameter dimension to a radius dimension you’ll simply need to follow the same steps to select the “toggle Radius” option.
Pro tip #2 is that you can hide or show your sketch dimensions. To hide your sketch dimensions simply click the checkbox in the Sketch palette. If it’s unchecked then your dimensions will be hidden…and of course, if the box is checked then your sketch dimensions will be visible.
The ability to hide dimensions can come in handy if you’re trying to work solely with constraints or to finetune details of busy sketch geometry.
You’ll also notice just below the dimension option that you can toggle sketch constraints on and off as well.
Pro tip #3 is that you can create Driven Dimensions. Up to this point in the tutorial, we’ve been creating “Driving” dimensions, meaning they drive the shape or size of the sketch geometry based on the values we input.
Contrary, you can create “Driven” dimensions, which are the dimensions used simply for reference purposes. In other words, they won’t alter the sketch geometry, but they themselves will be updated as you change the “driving” dimensions.
I’ll activate the sketch dimension tool and then I’ll click on the center-circle and I’ll click on the outer arc. Now before I click to place the dimension I’m going to right-click in order to select the “driven” option from the list. Then, I’ll click to place the driven dimension. Notice how this dimension has parentheses around it, signifying it’s a “driven” dimension.
In this example, I’ve added the driven dimension to show the distance between the circle and the arc. This way, if I add a dimension to the circle… and then if I update the circle’s dimension, the driven dimension will update accordingly showing me the current distance of the gap at any given time, without actually altering the dimension of the gap.
An important thing to note with driven dimensions is that sometimes you’ll be warned that they will be automatically applied. For example, if you remember earlier in this lesson, we added equal constraints to the small circles so we only needed to dimension the one on the left-hand side.
You may find that you want to apply a driven dimension to the circle on the right-hand side so you’re reminded that this circle has the same dimension, however, this is by no means something that is required or necessary.
Notice as I try to add a “driving” dimension that Fusion 360 warns me that the dimension will be driven instead. I’ll simply click the “OK” button to add the driven dimension to the circle on the right.
Pro tip #4 is that dimensions are automatically numbered. You’ll notice as I hover over a dimension that the dimension has a number applied to it. This dimension number can be used in the input field of other dimensions.
If I hover over the 15mm dimension on the left, you’ll see there is a number right after the letter “d”. I’ll use this as a way to create a dimension for the smaller line.
I’ll click on the small line and then I’ll type out the letter “d” and its number value, as well as the division symbol, and the number 2. This will set this dimension to be half of the 15mm dimension while ensuring that it always references this other dimension. This is why you’ll see the function symbol before this newly created dimension.
Pro tip #5 is that you can create equations within the dimension input field. We just saw an example of this on a very basic level by calling the dimension number and dividing it by 2. However, it’s important to note that we can type out any legitimate equation within the input field.
For example, if I double-click on the 100mm dimension at the bottom… I can type out the following equation in the input field (2+3+5)*(4+6)*1
Notice how when I hit enter that the equation equals 100. Now obviously there’s no reason to enter equations if you know the value should be 100mm…however, equations can be extremely helpful if you only know other dimensions of the model. Simply type out a relevant equation and let Fusion 360 do the math for you.
It’s also important to note that if you revive red text while typing out an equation then that means something in your equation is not valid.
Pro tip #6 is that you can use any user parameter values within the input fields to make your model more dynamic. I have a few other videos where I demo this with dynamic models… I’ll add those videos to the resource page for this tutorial.
For now, I’ll quickly create a user parameter value of “height” that is equal to 40mm. Then, I’ll create a new dimension on the left-hand side and I’ll type out the user parameter of “height”. As I hit “enter” on my keyboard you’ll see that the function symbol appears before the expression of the user parameter.
Anytime that I now update the user parameter, the dimension will be updated accordingly…and this user parameter can be reused in multiple dimension fields.
Lastly, pro tip #7 is that you can rename sketch dimensions. To rename sketch dimensions you’ll need to open the change parameters dialog.
I’ll select “Change Parameters” in the toolbar. Then, I’m going to toggle open the file name folder, and the sketch folder. You’ll then see that all the dimensions have automatically been added to this list. From there, you can edit the dimension name, instead of its default number.
The benefit to this is that it can be easier to remember instead of keeping track of all of the numbers, should you want to call your current dimensions by a name.
I’ll simply click on D1 or the first dimension we created, and I’ll rename this by typing out “bottomLine” in camel case. Then, I’ll click the “enter” key and I’ll close the parameters dialog box by hitting the blue “OK” button.
If I now hover over the bottom dimension you’ll notice that the dimension name now appears instead of “d1”.
To summarize this sketch dimension tutorial, you’ll want to remember that the most important takeaway is that you should always use the fewest amount of dimensions possible per each sketch. Always start by adding constraints before dimensions. Be sure to check out ProductDesignOnline.com/6 to check out constraint tutorials and other resources for this tutorial.
If you made it to the end of this tutorial then please let me and the rest of the community know by commenting below what cool project you’re currently working on in Fusion 360…and/or comment below with another dimensioning tip that you think everyone should know!
As always, I really appreciate you taking the time to watch this tutorial. If you enjoyed this tutorial please click that thumbs up icon and click on that playlist in the lower right-hand corner to watch more Fusion 360 sketch tutorials.
To be a part of the Product Design Online community, be sure to click that red subscribe button and click that little bell icon to be notified of more Fusion 360 tutorials.
A lot has changed in the menu of Fusion 360 since you made these videos.
Sometimes hard to follow for a beginner like me.
Hi Kim,
I understand that the UI changes make it more challenging. However, please note that none of the Sketch Dimension’s functionality has changed.
Finding the sketch features has been the consistent struggle that I’ve seen from viewers. The sketch tools have all moved into their own “Sketch” tab in the toolbar. The disconnect is because the Sketch tab is only visible while in an active sketch environment.
With all of the new content that I have in progress, it will be a while until I can revise these individual feature tutorials. You can learn more about the changes on this page – https://productdesignonline.com/fusion-360-tutorials/fusion-360-new-ui-vs-old-ui-august-2019-update/
Cheers,
Kevin
Hi Kevin,
I just wanted to say thank you so much for your videos. I downloaded fusion360 less than a week ago and originally started taking lessons from Fushion 360 Design Academy website, but it was a lot harder to learn from them. I almost quit using this program. Then I found out about your video over youtube and you made this program so much easier for me to use and I am not a computer person. With that being said, I hope this video stays here for a long time. Thank you so much again.
H
Hi Hiromi,
I’m glad to hear you stuck with it! One of the reasons I started creating tutorials was under the premise that more people should have access to the ability to learn CAD programs, such as Fusion 360. I don’t plan on stopping any time soon and hope your skillset continues to grow as I release more videos.
Cheers,
Kevin
Hi Kevin, I know this is the wrong section to ask this question. But I’m at the Day#3 lesson of paper clip and I’m stuck there for last hours. My sweep command only let me go though half way though of paper clip. What am I doing wrong?
Hi Hiromi,
The Paperclip lesson has a known issue with the fillets messing with the sweep command. To fix this, you’ll want to revert the sketch and apply the fillets ONE at a time. The other option would be to delete the fillet ends and use the tangent arc command to connect the straight lines. Either one should take care of the issue and allow you to complete the sweep.
Cheers,
Kevin
OMG! I did it. It worked. I guess too many constrains would mess up final result.
Hi Hiromi,
Glad to hear that it worked for you. The fillets meeting in the middle seem to mess with the Sweep command… so it’s not necessarily the constraints.
Cheers,
Kevin
Hi Kevin,
Sorry for asking questions again, I know this isn’t the right section to ask, but I cannot find coherent place to post my question on your website (let me know where you prefer me to send some question if I’m allowed to). I’m now at day #7 of handle grip. I did have a hard time to click the ditch profile (?) at 4:29 into the video clip and to click the wired shape by using L tool at 4:50, I struggled, but I managed to solve by approaching different ways. But I cannot change the color of text itself. I can select just alphabet, and they will be highlighted but when I move appearance, the entire bar will be affected. What am I doing wrong?
I really do appreciate your video. I am a ceramists and my intention is to create a model or mold model to make a plaster mold eventually. Then either I would slip cast with casting slip or simply use as press mold with clay. I was struggling during this difficult time, but decided to think it positive way and started teaching myself something new. So far I’m very excited about this possibility and once 3D printer place open, I would like to get hold of what I’ve been designing with. Thank you Kevin. Your tutorial is just amazing.
Hi Hiromi,
Once you have the faces of the text selected/highlighted you have to carefully drag and drop the appearance to within the boundaries of the highlighted section. If it goes outside the highlighted section then it will be applied to everything.
Let me know if that helps at all. Otherwise, I’d have to take a look at your file to double-check everything is set up as expected.
Glad to hear you’re making the most of the situation! There is a lot of opportunity with 3D printing and ceramics and I think you’ll find the new skillset to be very valuable in your work. Keep at it! 🙂
Cheers,
Kevin
Thank you Kevin. It just took some patience to drag out appearance at the right spot. But I found out that if the alphabets are all highlighted (not trying each alphabet one by one), “drag appearance tool and drop off” process takes easier to engae in the program, at least that’s how I felt.
You’re welcome! Glad to hear that it’s working for you. It can be tricky with smaller objects.
Cheers,
Kevin
Hi Kevin, I’m at the day #12 of Auger bit. Everything was smooth till loft tool. I cannot connect bottom of coil and point. The error says try changing the inputs or swapping the profiles for center lines or adjusting the continuity condition. Tool body creation failed. I think I’m having a hard time to project the bottom of coil (?) or maybe I’m not creating the right project(?). New version of fusion 360, it’s hard to figure out when you are switching sketch mode or model mode. After the creation of metal spiral (I’m out of sketch palette), you still have access to project command, which I don’t. So, I’m creating new sketch palette, is this when I’m doing something wrong? I’m so confused.
Hi Hiromi,
You’ll want to Project the bottom of the straight pipe, which was created with the pipe command. Select the bottom face and then hit the keyboard shortcut letter “P,” which will activate the Project command.
When you go to complete the loft you’ll need to make sure you select between the two projected circles/edges of the pipe, followed by selecting the point.
Cheers,
Kevin
Hi Kevin,
I think my problem was that I didn’t click bottom face, but outer and inner circle line instead to project. But what is project anyway… I can already click bottom of pipe to create offset plane to create point. Why cannot just loft between bottom of coil to point on offset plane? What the project command do? What is project anyway?
Hi Hiromi,
The Project command recreates sketch geometry on the active sketch based on your selection of existing 3D bodies. You need a sketch profile to work with the loft command, as sketch profiles are different than simply selecting the face of a model. Learn more about the Project and Intersect commands with this video – https://youtu.be/WAs144r-Xko
Cheers,
Kevin
Hi Kevin,
Thank you for answering all my questions. Your last link you send me really helped me to understand what the project command does. I do have a couple more questions to ask. Q#1, At day #16 of 4:47 into the video, why the circle moves down, instead of arc moves up? I thought whatever you click first in constrain mode is more dominant, so second one you click would match with first one you select? Q#2, To be printed in 3D machine, is everything has to be converted to BREP file before you send to the printer? (currently I don’t have any access to printer, so I don’t know how it works) Q#3, Even the simplest thing we designed in sketch and extrude or stuff we created in create mode like sphere or box under form and modified (Q#3.5 Is this the equivalent to model mode from old version of fusion 360?), when I convert to mesh mode, they will be made of tons of edges like one of those phone stand? I don’t even know why the simple phone stand has to have so many edges, or those edges are necessary to make even the simplest stuff? Thank you so much in advance.
Hi Hiromi,
1. Sketch entities will move based on all of the sketch constraints, so not necessarily the first one selected. If something else is already fully-constrained then the other object will be forced to move to it.
2. To export a file for 3D printing you’ll need to right-click on a body or Component and select “Save as STL”. That converts the solid BREP body to an STL mesh file. This video you’re referencing is essentially the opposite process. If you find a mesh file online then you’ll need to follow this process to convert it to a BREP solid body so it can be manipulated with Fusion 360’s native tools. The lines are caused by the file being a mesh file, made up of hundreds of triangles.
3. The Model workspace was renamed “Design”. You’ll also find that there are not “contextual tabs,” meaning it presents you with the relevant tools while you’re in an active environment. Sketch tools will now only be available when in a Sketch environment.
Cheers,
Kevin
Any way of stopping Fusion from automatically outputting the dimension measurements for every dimension in a sketch?
I always use my keyboard to enter dimensions and measurements instead of using the mouse to “chase” correct values, and I also frequently use math operands.
However the time I save by using keyboard is completely eaten and then some by having to manually remove every single dimension measurement for every single line drawn…
Unfortunately, there is no way to do that.
You can, however, “lock” dimensions in place once you’ve typed them out. Simply hit the “tab” key and you’ll then see a gold lock icon.
Some prefer to click to place the sketch objects (square, circle, etc) without placing dimensions. Followed by manually adding the dimensions per each line or entity. This will avoid having many dimension inputs open at the same time.
Cheers,
Kevin