Tipping the SOLIDWORKS Fantastic
An inescapable truth is that 3D modeling is an inherently complicated activity. Anyone who has done it knows that. Why? It’s because 3D modeling is all about building high-quality, accurate digital representations of real-world or potentially real-world objects, or sets of objects. Another almost universal truth is that in most 3D modeling programs there are multiple ways to approach doing everything. For those who may be new to 3D modeling and are confused by that, let me explain. If you want to model a rectangular block, you have a few choices. You can extrude a sketch X distance. You can sweep a sketch along a path. You can even input x, y and z coordinates for the corners. All will get the exact same 3D volume. So, if there are so many ways to do things, how do you know which to use?
I have a few tips on how I recommend that 3D modeling be done. Here they are, in no particular order.
1. Use common orientation. (If your models are always oriented in the same way, you’ll never have to guess.) When we started out our 3D modeling training, chances are we were taught the Right-Hand Rule, which follows: Hold
your hand in front of you, with the palm facing you. If your thumb sticks straight out, your index finger points straight up, your “tall man” finger points straight at you and the rest of your fingers curl down, you see the basis of how most modelers work. Your thumb is the X-axis, your index finger is the Y-axis, your “tall man” finger represents the Z-axis, and is perpendicular to the X- and Y-axes. Got that? Now, if you are modeling a tube, do you model it standing straight up or on its side (or perhaps going right into the screen)? It can make a difference when you bring it into an assembly. I’m not saying any of those orientations are more right or wrong than the others, just that you should know why you are modeling in a given orientation. The best way to decide on an orientation is to know how your model will be used. If it’s a test tube, it will likely be used standing straight up. However, if you are designing a dispensing machine, the orientation might be different. Orient your model based on how the object will be used.
2. Constrain everything! (An unconstrained sketch is a landmine waiting to go off.) Unless you don’t
particularly care what happens to your models, never, never, ever just leave your sketches unconstrained. That is the surest way to build disaster into your model. First of all, the whole point to parametric modeling is to attempt to capture design intent. That means dimensioning what is important to the design. If you know something must always be 2.5 times as wide as it is tall to work, that is design intent, and you should not only dimension it that way but also add in an equation to make sure it stays that way. Why? Some people might think it’s the same thing to dimensionally constrain the sketch 1 unit tall by 2.5 units wide. But, what if someone later comes along and changes it to an arbitrary length that works out to be 4 times as wide. The design intent was to control it per its function. But without anything to tell someone else that information, that intent is lost. Likewise, always fully constrain assembly components. I have seen far too many people just eyeball a location and call it good. When I open an assembly, I don’t want to be able to click and drag its components. Remember, if something can move, it will, and usually in unpredictable ways. In SOLIDWORKS, if something is unconstrained, you will see lots of little minus signs next to things. Those are red flags that bad things are going to follow. Fix them!
3. Name everything! (Provide vital information to those who may come after you.) If you yell out
“Hey!” in a crowded room, lots of heads will turn. It’s not a good approach if you if you were trying to get the attention of just one particular person. Features are like that. Your feature tree is going to get really crowded. If you don’t remember what feature did what, you’re going to have to go looking for it. That’s not an efficient use of your time. But if you name things, you will know, at a glance, what is what. Name features, folders (use folders to organize your features), configurations—anything you can! Whoever works on your models next will love you for it.
4. Helical sweep (simple, fast, easy). There are numerous ways to get where you are going. It’s always good
to know another road. If you want to create, say, a spring, try this. Create a sketch for a profile. Then make a sketch of a straight line on the same plane as the profile. Then use the Sweep command. Select the profile sketch first, then select the straight line to be the path. Change the Profile Twist to Specify Twist Value, and you will have the option to control the twist by degrees, radians or revolutions. Most often you will want to control it by revolutions. All that’s left is to tell it how many you want. Ba-da-BING! There you go!
5. Sweeping along edges.(It makes running wiring and/or tubing simple.) Sometimes you want to control the
path of, say, wires. A really interesting way to do that is to use the edges of a solid as a path to sweep along. Create a solid that represents your path. Then create a 3D sketch and extract the appropriate edges. Then create your profile perpendicular to your path. Once all that’s done, just sweep the profile along the 3D sketch and hide (not suppress!) your solid. This can also be done with a surface.
6. Reversea cut. (Sometimes you just need to save the middle.)Sometimes it’s easier to choose what you want
to keep than what you want to cut. You don’t have to create a big box around a small sketch to take out what you don’t want. You can just create the sketch of the cut and when it comes time to make the cut, just select “Flip side to cut.” Instead of cutting out only what is contained within the sketch, SOLIDWORKS will get rid of everything outside the sketch. It comes in handy.
7. Draft vs. taper. (When you put it on can make a difference.) Depending on how you are making your
parts, you might have to include draft. Draft makes your part smaller at one end than the other, so, for instance, it can be ejected easily out of an injection mold. Taper can do that too, but taper is applied one face at a time (that is, selected one at a time). Draft is applied to every face in your sketch at once. SOLIDWORKS makes things somewhat confusing because it calls them both the same thing. But one is applied during the creation of a feature, and the other is a feature in and of itself. So, use Draft in an extrude if you want the whole model tapered. Use Taper if you just want selected surfaces tapered.
8. Flex (flexibility, the right way) There are many ways to bend a wire. The way that occurs to most 3D
modelers is to sweep along a path. But the smart folks at SOLIDWORKS have given us another way. Face it, in the real, physical world, that wire is coming off of a roll and being cut to size. Using the sweep method, you will probably end up with two models in different configurations so that you can show both on a drawing. That’s a lot of work. And, your mates will multiply too. Why not just model it straight and bend it the way you would in real life? Use the Flex command. Create your model. In the Flex command, select your model. You’ll notice two planes, one at each end. Drag plane 1 to where you want the bend to begin. Plane 2 goes where you want the bend to end. If you want to bend the wire all the way to the end, leave plane 2 alone. Then, all you need to do is give the flex an angle.
9. Renaissance modeling. (Use the right tool for the job.) Anyone who has read my writings for very long should be familiar with the term “Renaissance Modeling.” It is a term I use to address the many tools and methods modelers use to build. Simply put, you have a box of tools. You need to know when to use what, and why. Too many modelers take a carpenter’s approach to modeling—when you have a hammer, everything looks like a nail. You can make as many assumptions and arbitrary rules as you want, but not all of them are going to turn out well. I know people who always do things the same way. They are constantly modeling themselves into corners, needing someone’s help to get out. These people are not popular with the other modelers they work with. If some functionality or other is included in a software package, it is there for a reason. Someone is going to like it. As a renaissance modeler, I prefer to know all the tools in my 3D modeling toolbox, their advantages and drawbacks, and when to use each of them.
10. Mating to planes vs. faces. (There’s room for both.) There is some debate among my friends at work about whether you should mate your assembly components to planes or only use faces. Having read the above paragraph, it should be no surprise that I am an advocate of using both—when they are called for. The advantage to mating to faces is that it more accurately represents the real-world application of the component. A screw will go into a hole; therefore, it can be concentric. It will go until it stops at the head. Cool. That’s great! But sometimes you want to drop, say, a component into a box. There isn’t a right or wrong approach. I would use a plane in the center of the box. Why? Because accuracy isn’t a factor, and if that component (or the box) ever changes to something else, the mate won’t explode the way it will with a face mate. Use what’s appropriate and you won’t go wrong.
There you have it, my 10 tips for SOLIDWORKS users. I’m sure there are many other tips and just as many arguments about these. But if I leave you with nothing else, I want it to be that just perhaps you might not have used these before. And learning something new will only make you a better modeler.