Name: Sketch with Confidence: Tips & Tricks to Master Sketches in SOLIDWORKS
Uploaded: 2026-01-29T19:00:07.495Z
Duration: 29 min 37 s
Description: Sketch with Confidence: Tips & Tricks to Master Sketches in SOLIDWORKS

Transcript for "Sketch with Confidence: Tips & Tricks to Master Sketches in SOLIDWORKS": Hi, everyone, and welcome to today's webinar. My name is Baily. I'm a senior application specialist here at GoEngineer. I work mainly with SolidWorks CAD and SolidWorks Data Management Solutions, so PDM and Manage, and three d experience in the cloud. I'm located in Toronto, Canada, and my email is at the bottom right there. If you have any questions or comments after the webinar, feel free to shoot me an email. I'll pull my email up at the end of the webinar as well. So today we're gonna be looking at sketching with confidence, These will be tips and tricks to master sketches in SOLIDWORKS. Sketches are obviously a very important part of CAD modeling, and they're essentially the foundation of three d models. Most or all of the three d models that we're creating on a daily basis are going to start with a sketch, so we wanna make sure that we're sketching efficiently and creating high quality sketches. We'll talk about sketch practices, so sketching with the right approach. Sketch settings, these would be customizing settings to optimize the way that we work in SOLIDWORKS, and then sketching tips and tricks that we can utilize to sketch efficiently. So we'll start with sketch practices, and these are basically best practices that might not only apply to sketches, but often apply to SOLIDWORKS in general. When we are designing any of our parts, we wanna keep in mind design intent. We want to make sure that we are designing with manufacturing and manufacturability in mind, as well as designing in a way that's going to allow us to make changes down the line without causing any issues. We want to use primary planes, so our primary planes are much more rigid and less modifiable than any other planes or faces that you would create, and because of that, we have less dependencies, which means that there's less room for error. We wanna fully define our sketches if possible where possible. This is going to, again, allow us to come in later and be able to make changes that won't cause the sketch to break, but this sketch will actually react in a way that we intend it to. Then all of this is kind of to keep everything simple. Our work as designers is challenging enough. We wanna keep it simple so that when we come back to make changes, when someone else comes back to look at our CAD model or make changes in our CAD model, that everything is easy understand and navigate. The second thing is our sketch settings. These are options and settings that we can toggle on and off, and things that we can customize, like UI customization that we can do in SolidWorks. This isn't just specific to sketches, but we can use an s key, which has a shortcut bar for commands that we can customize, and mouse gestures, which is similar, but it's just accessed instead of the s key through the right mouse button. So we can customize our our shortcut bar to include any commands that we want. Again, it's in context of our sketches in this case, but we'll also have sketch shortcut toolbars for our parts assemblies and drawings, and then the same thing with our mouse gestures. So, mouse gestures, would hold down the right mouse button and move into the direction of the command that we want. Some system options that that are good to look at are, first off, auto rotate view normal to sketch plane on sketch creation and sketch edit. This is when you create a new sketch or edit a sketch that the view is automatically gonna rotate normal to that sketch plane. Scale sketch on first dimension creation, so if we created a new sketch and we added an entity, and maybe it was 50 millimeters long, and then we added a a dimension to it that was 250 millimeters. In this case, it's gonna auto scale our view instead of making us have to zoom all the way out. We've got enable on screen numeric input on entity creation and create dimensions only when value is entered. In combination, these are gonna help us, number one, as we're creating sketch entities, we're gonna be able to input a dimension, and then that second checkbox is that dimension that we get that that we input is actually going to be used to constrain constrain that sketch entity, the dimension is actually going be added to our sketch. And we can preview sketch dimensions when they're selected. This will make it easier to add dimensions or just look at dimensions, so we can use this actually instead of Smart Dimension in some cases where we click on our sketch entity, we preview the dimension, and there we can actually go to change that dimension. Another one that's typically on by default that we might want to disable sometimes depending on what we're doing is snap to model geometry. When this is enabled, if there is a three d model in the background, as we're sketching, when we get close to edges or the vertices of that three d model, our sketch entities are going to start to snap to that. That could get annoying in some cases. Most of the cases it's good, but it could get annoying, so in some cases you can disable this as you need to. And then we've got a few sketch toggles I want to look at. Shaded sketch contours, so this is going to, as you close a sketch, it's going to shade that closed sketch so that you can tell that it's closed. Instant two d is something that's going to allow us to quickly and very visually modify dimensions in our sketches, and then dynamic mirror entities, instead of mirroring sketch entities after we create them, this will mirror them as they are created. So let's take a look at what that looks like in SolidWorks. So here, I'm just gonna create a new hard document. The first thing I want to look at here is if I right click on the upper menu and click customize, here's where we're going to be able to add and customize our shortcut bars. So here it's in my part one. We're looking at our sketch one today, and our mouse gestures. So here we can see what our mouse gestures currently look like, and we can add and and take away different commands. And the first thing I'm gonna do today is I'm going to create a sketch here on my top plane. Using my right mouse button to access my mouse gestures, I'm going to create a rectangle. I'm not going add a dimension just yet. Again, I'm going use my mouse gesture here and go up to my smart dimension. Here, I'm going to add a dimension of 100 millimeters. Notice that it automatically scaled the view, I didn't need to zoom out. It automatically just scaled it. It all happened at once. If I come out of my smart dimension and actually just click on one of my edges here, we're gonna see the preview of the dimension, and I can use that preview also to add the dimension. So just a quick way we can add dimensions. And because I also have my shortcut bar set up, if I click my s key here, I can directly extrude this profile just using my s key. So I'm gonna extrude that just 10 millimeters. Now I'm gonna click on the top face of my geometry right now and and create a new sketch. So now I'm going to use the s key to add a center line, and I'm using the s key instead of mouse gestures because I have a few more options with my s key. And as I hover over one of the edges here, it's gonna actually snap to the model geometry, so that's one of the options that we had enabled. And now if I enable dynamic mirror entities and I select the line about which to mirror and create a line, as I add new sketch entities, they're gonna be created on the other side as well. And once I close this off, we're gonna see that because I have shaded sketch contours enabled, that closed sketch is shaded now. With instant two d enabled, I can click on one of my dimensions and grab the handle at the end, and then I can just change it by dragging it and change it more on an integer basis here, And here I've quickly changed my dimension. So I'm just going to exit out of my sketch, and we're going to jump back to presentation. So now we're going to look at some sketch tips and tricks that we can use as we're sketching. Some are for sketch definitions, so we can use these tips to add dimensions, use equations and dimensions, modify sketch relations. We're going to use some of them for advanced dimensioning, so dense dimension types and angle types, as well as different ways that we can modify our dimensions, creating efficiency when we're sketching, different ways we can select sketch entities, switching between sketch entities as we're sketching, copying sketches to different planes, and incorporating some of the three d part geometry that's in our model. And some extra control that we have, we can automatically fully define our sketches, we can solve our sketch conflicts using a good tool called Sketch Expert, We can import pictures and then some tips with three d sketching as well. So again, we're gonna come back to SOLIDWORKS here, and I'm gonna create a new part again here, and we're just gonna start fresh. And we're gonna start by clicking on the top plane, creating a new sketch. Notice that it auto rotated because we have that setting still on. I'm going to start creating a line, so I'm gonna use my mouse gesture and go to align. We're gonna just make a vertical line. And next, we wanna create an arc, but here, instead of switching to the arc tool, I can just hover over that endpoint, and then it's gonna activate the arc tool. So I'm gonna come back around. I'm gonna go horizontal to that endpoint, and we're gonna come all the way back and pose off our sketch. So we can add dimensions using smart dimension and preview sketch dimension. We can also add them using auto insert dimension. If I right click here, I can use auto insert dimension, and this is gonna be a quick way that we can add dimensions, but it's not gonna be as flexible as using smart dimension. I'm gonna add a few dimensions here, and now I've constrained I fully defined my sketch. It automatically created a bunch of relations. I'm just gonna delete this tangency relation, and now that it's not that it's not constrained, now if I just click on that coincident point, I can add the tangency relation directly from the coincident point rather than selecting both of the lines. So that's just a quick way we can do that, and we can also reverse the tangency of this arc, so I can just do reverse endpoint tangency, and we can just quickly reverse that if we want a different effect there. So now I'm gonna go ahead and add a slot, which I have as part of my which I have a shortcut to on my shortcut bar. We're just gonna add a vertical slot here. I wanna set my dimensions for this slot. First of all, I'm gonna use the the arc here. I'm gonna select set the dimension of the arc. I'm gonna double click on this dimension instead so that I can access the dialogue, and here I can actually create an equation. So if I hit equals, I have the option to use certain mathematical functions or file properties in my equation. In this case, I actually wanna use one of my dimensions, and this dimension, in this case, is on this sketch, but it can be on another sketch as well. You'll notice that says d one at sketch one, and I'm going to say this dimension minus one inch. So I'm going to use that dimension, and I'm going to do a unit conversion because here I'm actually in millimeters, so it's going to do that conversion for me and that math for me. Here I can see because of that symbol there, can tell also that there's an equation that's driving that dimension. Now I'm gonna use smart dimension, and I'm I'm gonna add a dimension of the overall length of this arc. But, typically, when you would do this, it would just do the center to center point distance. In this case, I'm gonna hold shift, and because I'm holding shift, it's gonna enable this maximum to maximum distance. So this is the outer arc dimension essentially. So I can set this. In this case, we'll set it to 25 millimeters, and in the dimension dialog, I can look at the leaders tab, and here I can actually change the arc condition. So if I didn't actually want it to be max to max, instead we'll do center to center, we can modify that afterwards. With arcs, obviously we have radius and diameter dimensions, but, we can also do a an arc length dimension. So if I use my smart dimension, click on the two endpoints of the arc and the arc itself, we're going to get an arc length dimension. Because this is already fully defined, it's going to prompt me to make it driven instead of driving, and a driven dimension is essentially a dimension for reference rather than something that is actually defining the sketch. So I'm just gonna create that as a reference dimension, and then we're also gonna add another type of dimension here. So if I right click and go to more dimensions, I'm gonna add a path length to this slot because I wanna see how how long the outer edges of this slot is. There we go, and I can create a path length dimension against again, I'm gonna get the same dialogue, but I'm gonna make it a driven dimension, so we're not gonna over define our sketch. So now I'm going to exit out of this sketch, and I'm going start a new sketch instead on the front plane. Just going to hide the previous sketch. You'll notice this little symbol next to my sketch. This is gonna tell us whether our sketch is fully defined or not. In this case, it's not fully defined, I can see that symbol there. And here, I'm just gonna start sketching a kind of a triangular shape. And I wanna add a dimension from this line to a horizontal axis, but I don't have any constructions construction lines in this model in this sketch. Without having to add construction lines, instead, I can just use Smart Dimension and click on that line, click on its edge, and we can activate some of the directional axes. So, here I'm going to add a dimension from that horizontal. I can also add dimensions just using vertices. So here I'm going to add a dimension using the three vertices of the triangle. We'll set that to 100, and I'm going to add a height dimension here as well. We'll set that to 10. And something cool that I can do with my dimensions once they've already been created is that I can drag and drop the end location of that dimension, and I can change the location of that dimension wherever where it's referencing to. So now I'm just going to use my s key actually, and we're going to add a center line here. And here, if I add a dimension so we'll smart dimension from this line to my center line. Because it's a center line or a construction line, I can add this dimension normally, or I can add a mirrored total dimension. So this is gonna be two times the dimension as if I was to either mirror it or maybe I was going to revolve it and I wanted a diameter dimension instead of a radius dimension. So we can set that to 10. We can do the same thing with angles. So I can set an angle dimension from that line. If I hold shift, I can do that kind of overall angle dimension. And again, we're gonna over define here, but instead, I'm just gonna make it driven so we're not over defining our sketch. And now I just I'm just gonna add one more line into my sketch here. So we're gonna go just from that point to our center line. And when I go to trim, I have an option to keep trimmed entities as construction geometry. This is gonna be helpful if we wanna keep that geometry as reference to use later on or to see how it was created. So I'm just gonna power trim, and I'm going to trim out that geometry. But you'll notice that it's still going to remain as construction geometry here. So I haven't entirely gotten rid of those lines. If you are in a pinch or you have a reason that you need to kind of do a quick and dirty method to fully define your sketch, you can use the fully defined sketch command. And here, it's going to quickly and automatically fully define our sketch. So it's gonna add the the dimensions and relations that are needed. This might not be they're probably not gonna be how you would do it, so recommend fully defining the sketch yourself, but this is just a quick and dirty command that you can use. And then some options for selection. So if you've used box select, you may not have noticed, but if you go left to right using a box select, it's only gonna select things that are fully contained. So I need to actually fully contain an entity in order to select it, and I can use that to select and delete. Yes, we're going to delete. If I go right to left, it's going to select things that are either fully or they can just be partially contained. Here, I only selected the edges of these lines, but it included it in the selections. I'm going to use that to delete those, and one other thing I can do is I can use just control A. In a lot of software, we've seen that. We can just use control A and delete using that method. So some good selection tools that we can use. Now I'm going to create a sketch on the right plane, and here I'm just gonna add a polygon. So we know we have our line, circle, and rectangle, kind of the classic entities that we would add, but we also have other options like an ellipse, parabola, conic shape, obviously, the slot we've used today in a polygon. So here, I'm gonna create a polygon. I'm gonna locate it at the origin. We're going to use some smart dimensions and use this new tip that we just learned about clicking the line, clicking the endpoint to create a dimension to that vertical axis, and we'll set a length. So if you can set this to 25, and now we fully constrained, fully defined our sketch. We can use this sketch entity to copy and paste onto other planes as well. So here I'm just going to take that right plane, I'm going to create two new planes that are offset from that right plane, and I'm gonna just click on that sketch, control c, and paste it, control v, to my other planes. And now I can come in. We can see that they're not fully defined, and that's because when you copy and paste a sketch, you need to set the location. So here, I'm gonna set the origin. I'm actually just gonna change some of these dimensions for each of these sketches. Right. And we're gonna just do that one more time. So let's change this to 90 and this 20. And we gotta make sure that we snap it and locate it. And one use case for this could be maybe you wanna create a loft, and you want the profile to be similar as it's being lofted, but it's gonna change slightly. So here we can copy and paste the sketches, and we're gonna use this in our loft. Right? So we can create somewhat interesting shape here. If you're using three d sketches, just a quick tip for three d sketching, I'm gonna create a line. As you're sketching in three d, you'll notice it's gonna show which plane you're sketching on. So currently, I'm sketching on the x y plane. And if I wanted to change the plane, can click tab, and now I'm gonna sketch on the y zed plane. Right? Tab. Tab again. Now I'll sketch on the zed x plane. So you can change the plane that you're sketching on in a three d sketch just by clicking tab. I'm just going to open one of my recent documents here, and here we can see we have I'm going to click q, and q is just going to quickly show me my sketch planes. So I'm gonna click click q, and here I can see my sketch planes. I can see this geometry that we have is kind of angled in a strange way relative to our our primary planes. And if I go to create a sketch on, let's say, my top plane, for example, I can use some of this three d geometry in this sketch. So I can use my convert entities command, and I can use either convert entities to just bring in some of those edges, and it's not gonna constrain an edge if it's not at a coincident point, so I can move around these edges, those endpoints. I can also silhouette entities, so this would be essentially from casting a a light over this part, what the shadow would look like. So it might look a little bit arbitrary relative to other views, but if I come back to my normal view here, it's gonna be the silhouette of that part. Or I can also use an intersection curve, and this I can do for maybe specific faces or maybe I wanna do it for the entire part, and this is going to show where that three d geometry intersects with the plane that I'm sketching on. So, it might not make total sense when you're looking at it right now, but if we look at our top plane, we can see that's all the points where that cube is going to intersect with it. One other thing we can do is we import a sketch picture, so if I click the s key, I'm just going to search for picture, and we can use a picture if we want to use this for maybe reference in our sketch. We want to sketch over it, maybe trace over it. We can use this for reference. We can resize it. Here it's way too big for me, so I'm going set it to 150. We can resize it. We can move it around, and we can use this for our sketch to have as a reference. One last thing I want to show is the Sketch Expert tool. So, if we have a sketch, and here we're going see what we get an error when we open the sketch because when we open this SolidWorks part because there is a warning in the sketch. When we open that sketch, we're going to see that it's over defined, so that's not good practice to leave our sketch over defined. We want to make sure to fully define it, so what we're going to need to do is remove some of our relations. In order to do that quickly, I can just click on that over defined error, and I can use the Sketch Expert tool to either manually repair it, but in this case, I'm going to use it to actually help me further and diagnose the issue and then give me some solutions. This is one option, getting rid of the horizontal relation over here. We can see that that's going to cause a very strange kind of sketch, or we can get rid of this collinear dimension. That's what I want to do. I'm going to accept that, and I can use Sketch Expert to very quickly resolve my sketch conflicts. I know that was kind of a lot of tools and a lot of different tips and tricks to show in one presentation, but hopefully you found that helpful. Obviously, now that we've seen all that stuff, go ahead, try it out. If you have any questions or if you're looking for guidance, we can help through application mentoring sessions that can be scheduled at this link. We can help through consulting services if it's a little bit more of a deeper issue. We are running tips and tricks webinars throughout the year, so each month we're going to have a different tips and tricks webinar. The next one is going to be patterning tips and tricks in late February, so feel free to check that out. Obviously, I encourage you to just keep learning, keep watching webinars, keep doing training. There's always ways that we can work more efficiently and improve the way that we're working in SOLIDWORKS. So, yeah, like I said, if you have any questions, feel free to email me benymarovskygoengineer at dot com. We can help, obviously, with this webinar. In addition to that, GoEngineer offers all sorts of solutions from engineering hardware, engineering software, so CAD, CAM, simulation, anything from implementing in support to training services and consulting services, so feel free to reach out if you have any questions, and hope you guys have a good rest of your day. Thank you. I do see there's been a bunch of questions in the chat. And, Mike, thank you very much for answering those. You've been a good help. I saw a question about so Dan, if you're still here, I know you'd asked the question about showing again how to mirror a part using that dynamic mirror entities. So I'm just going to share my screen here. Let me share my screen. I'm just pulling up kind of that same area where I did that dynamic mirror entities. And here I'm going to use my right to left box select, and here, I'm gonna select everything that's partially contained. So I'm just gonna remove all those mirrored entities already that I had already created. And I'm gonna use my mouse gestures actually, sorry. I'm gonna first, I'm gonna enable dynamic mirror entities. I'm gonna select my line to mirror about, and then I'm gonna use my mouse gesture to activate the line command. And here, I'll do it a little slower so you can see as I add each of those lines, you're gonna see on the other side, those entities are gonna be mirrored dynamically. So I don't need to create them and then mirror them after. It's gonna happen as I'm I'm creating it. Stick around if there are any other questions. Also in case you missed it, there's a button just at the top right there in your interface on GoldCast that says register to PatternFast I think. So that's just a registration link to that next webinar that I talked about. If you want to catch that next webinar, can just click on that link, register there. So hopefully we can continue learning through these tips and tricks webinars that be running throughout the year. I see Isaac just had a question about where the Sketch Expert tool is. The Sketch Expert tool is gonna be accessed when you an over defined or issues with your sketch. You can just access it from just jump back into SOLIDWORKS here. But you would access it just from the dialog down here. So here you can see if you have it full screen, hopefully you can just see the text here. It says under defined. If my sketch did have errors or it was over defined, it will say over defined. And if I just click on that, that's where I can activate the Sketch Expert tool. Just keeping an eye on the Q and A. If you do have any other questions, again, feel free to email me. I can fill my email just in the chat here in case you missed it. So my email my email is just in the chat there in case you missed it, and you wanna send me an email after the webinar. Yeah. I think we're coming up on the thirty minute mark here. So thank you everyone again for joining. If you have any questions, shoot me an email. And, yeah, keep keep an eye out for the the new webinars that we'll be running. Hopefully, you can catch those and learn some more things.