Solving engineering problems is pretty damn hard. And usually, finding out which problem you need to solve is the hardest problem of them all.
“Can’t I just mate this follower along this cam, no matter how they rotate?”
“How does this chain drive move these product carriers through the machine?
Lucky for you, we have created another set of tips the will make your mental models and CAD models behave more like their real world counterparts. This allows you to find out what is really happening a lot quicker. It will also save you some frustration. Isn’t that what really counts? 😉
In this post I’ll show you how to create smarter sketches by using paths and smarter assemblies by using cam mates.
Sketch paths in SOLIDWORKS are combinations of sketch elements. This feature allows you to model real world items like ropes, chains and cams:
Pretty neat, right? Do you already remember a project where you really could have used this?
In the image on the right I have used the tangent relation to bond the two cams together. You could also just have a coincident relation with an end point of a line and move that line along the beaten path.
To create a path, you first need at least two (connected) sketch elements. They can form a closed shape or they can be open ended. The elements don’t even have to be tangent! You can create any weird shape of connected elements and turn that into a path.
Al you need to do then is select the sketch items, right click and select Sketch Tools > Make Path. In older versions, the Make Path button was located directly in the right mouse click menu. You can also click Tools > Sketch Tools > Make Path and as always, you can use the search bar to find the button that is hidden somewhere is the button jungle called the UI. This video by Innova Systems shows the process nicely:
From now on the sketch elements behave like a single unit. That also means you can’t select the individual lines without the next trick…
The Select Other feature is so useful that SOLIDWORKS decided it deserved one of the best spots in the right click shortcut menu. It lets you select something behind or within the object that you are clicking. In parts and assemblies, this allows you to select faces behind the current face. Just try it and see what happens.
In sketches, it allows you to select items that belong to a path:
You may have noticed that I have added dimensions to my sketch to fully define the sketch, except for the orientation of the path. When you don’t need the exact dimension or if the dimensions get it the way when you rotate the cam (they do), you can turn the path into a block.
We don’t even need to make a path actually. Just draw a bunch of sketch items, select Tools > Blocks > Make and select the elements. The whole thing now behaves like one and you don’t need the dimensions. You can fix a point to make a cam rotate. This allowed me to create the same cam with less effort:
To create a virtual piece of rope is one thing, to make sure the length remains constant is another. Once you have grouped a set of sketch items together in a path, you can select the Path Length Dimension from the sketch toolbar. I keep my toolbar tucked away nicely on the left of my monitor, where it takes up the minimal amount of screen real estate.
When you have created this constant path length, you can finally model ropes and chains nicely. This once really helped us to find out how a complex design was going to move. We also found out most of our design were not going to work…
The path dimensions behaves like any other dimension. That means you can use them in equations and you can vary its value per configuration. You can even use them in design tables and custom properties if you’d like.
Now that we created fancy sketches of cams and decided on a design, it’s time to create some parts and an assembly. Let’s say we have the following cam and follower:
The process of mating these parts couldn’t be simpler. You just have to know where to look, as always. Right now we have to look in the Mates dialog and subsequently we go to the Mechanical Mates section. The first one is the Cam mate, now all you need to do is select a surface that belongs to the cam surface plus a surface on the follower. SOLIDWORKS does the rest and makes sure the cam surface is a set of tangent, closed loop surfaces. Where we didn’t need tangent lines for the sketch paths to work, the tangency really is required this time.
Another blog post, another tool in the belt. Fortunately a real craftsman can never have too many tools, no matter what his wife tells him.
What were you able to model using the sketch paths? We’d love to hear from you, just drop us an email or a message on LinkedIn. You can also check out our other blog posts, for example this article on Assembly Best Practices or on how to use Envelopes to easily divide and dedicate space within assemblies.
Until next time.