Join Gabriel Corbett for an in-depth discussion in this video Linear and circular patterns, part of Cert Prep: Certified SOLIDWORKS Professional (2015).
- Linear and circular patterns are used quite a bit in the certification exams. I'm going to go through a couple of examples of how to use both of those. So first off I have a part here and I want to make a circular pattern so I'm going to choose this front face here, click on okay, click on Normal To and then go ahead and start a sketch. I'm just going to draw a simple circle. Now, I'm going to define that Bolt Hole Circle by the centerpoint here, I'm going to snap that to the center of the circle. Now I'm going to go ahead and choose a dimension here, I'm going to say 225 and then I want to make this circle here construction geometry.
So I'm going to click on Construction and switch that over to Construction Geometry so it knows where it is. I'm going to use another center line from the origin to the center of the circle and then I can define that angle. All right, and that angle here, I'm going to call it 20 degrees and then define the size of that circle with a 30 millimeter circle, okay? Once I have that I'm going to go ahead to Features and I'm going to say Extrude cut and I'm going to cut that all of the way through the parts Through All and click okay.
Now I'm going to take this one hole that goes all the way through the part and I'm going to pattern it around. So I'm going to go to Circular Pattern, I'm going to choose my reference axis which is going to be the center of this cylinder here, notice I can choose that. And then notice, by default it's choosing a 15 degrees spacing in 9 of those. I can change the spacing if I wanted to, up or down, I can type in a value here, like 30, or 25, whatever I'd like, and then how many of these I'm looking for.
So if I put 30 and I put 9, I'll go all the way around here, if I make this say, 20 degrees then I can go and add 13 or 12 of these holes around this part. I can also use equal spacing but that's going to be putting holes where there's no material to cut, so we don't want to be doing that one for this example, so turn that off. Let's use 12 and click on okay. That's as simple as the circular pattern is. Let's jump over to 2.11.2, you can see I've got two hexagons already laid out as a sketch.
So I just created the sketch here which is Sketch Two and I made it Cut Extrude through this part. Now I want to create a linear pattern of this and create a honeycomb. So I'm going to click on Linear Pattern and I'm going to choose my first direction as this one here so it's going to be any linear edge in the direction I like to travel which is going to be this one here and then down here for Direction Two I'm going to choose this edge here. Now, for the spacing I can just type in a value here or I can link this to a global variable, I can even pull sketch entity values into this.
So first, before I do that I'm going to click on the feature I want to pattern and that's going to be this Cut Extrude, so there it is, and flip the direction here, and flip it there. Hold on, there it is. All right, that's what we're looking for. So you can see I had the exact values here, three millimeters and 1.732. Now, that's not by accident, it's exactly the values we need but I can also just type in a value here. I can say 3 millimeters or 30 millimeters and it's going to give me a preview of what's going to happen here. I can also flip the direction to any how I'd like.
Same thing up here, I can define this value to be anything I'd like so right now it's at three, I can change that to any value above that or below that, it doesn't really matter, but I want to make sure that I define how many instances I'd like, so you can see I have 23 here. Actually, I want to have four and as soon as I go to four, notice it gives me a preview but that's not really what I'm looking for. I want this to be exact honeycomb and to do that I can actually reference this sketch originally here. So right here in this first value I'm just going to say equal to, and click on Equal, and I can choose a function or a file property, or if I double-click inside of this feature here, you can see that three right there, I'm going to choose that three.
And then for my spacing here I'm going to say that's also equal, and I've laid out the sketch right here and that's my spacing there, and then I'm just going to make this a little bit smaller so it's three and click on okay, and that's my linear pattern. So a bunch of different ways you can use that. So you can just type in a value, you can link to an equation or a value, you can even link to a sketch. I just wanted to point out before we close on this one that if I look a sketch, I define it so that I see that I have a three millimeter spacing between these and I pulled a reference value here, how far it's going to be up to that next instance.
So I added a little smarts into my sketch using some construction geometry so I could choose those when I create the pattern so they come out perfectly. So those are the basics for both a circular as well as a rectangular pattern. Most of the time in the exams I've seen, there is going to be either one of these used so make sure you brush up on it and are very familiar with creating a pattern, especially the circular pattern.
He also breaks down the three segments of the test (part modeling, configurations, and assemblies), providing strategies that will help you pass each section. At the end of the course, there are two sample exams to practice what you've learned.
- CSWP requirements review
- Working with sketch entities, tools, and relations
- Using the boss and cut features
- Performing sweeps and lofts
- Smoothing corners with Fillet and Chamfer
- Creating linear and circular patterns
- Setting up equations
- Creating multibody parts
- Setting mass properties
- Working with materials and constraints
- Inserting components
- Setting up reference geometry
- Arranging features to change the part
- Working with suppression states
- Using a design table to build configurations
- Establishing standard drawing views
- Annotating your drawings