rocksolid tutorial: in context cylinder stroke animation

Just like what triggered my post last weekend “rocksolid tutorial: modeling a variable profile helix cut” I was recently asked a question by a member of my user group about how to simulate the stroke of a cylinder in SolidWorks.  So here we go, this is how I would simulate a simple cylinder stroke in SolidWorks.

As you can see in the above picture I have quickly assembled a bottom plate (green) that is housing a gas cylinder (yellow) in a pocket.  I also have a top plate (red) that is mated to the bottom plate with a distance mate called “open/close distance” which we will discuss later.  My gas spring was modeled with a simple single sketch profile revolve as you can see below.

By creating my gas spring as a revolve it is extremely easy for me to add a coincident mate between the top of the edge (which represents the end of the gas spring cylinder) and the bottom edge of the top plate.  You can see that I have both of those entities highlighted in red in the above picture.

Once you I added this relation you can see that the sketch of my gas spring is now fully defined.  You will notice that I also have added a driven dimension on the overall length of the gas spring which I can monitor to make sure that it does not exceed the limits of the stock spring.

Once I have done that you can exit your sketch and stop editing the part in your assembly.  Now you are ready to edit the mate that I mentioned earlier.  I have named this mate “open/close distance” so that I can quickly find which one I need to change.  By editing this mate you can simulate the top plate moving downward towards the bottom plate therefore compressing the gas spring cylinder.  You can see in the above picture that my distance “open” distance is 5.170in.  When I change this value to 4.170in., which is my closed distance (shown below) you can see that my cylinder compressed like I am wanting to see.

This is just a quick and easy way to simulate this cylinder compression.  As is with most things in SolidWorks, there are many ways to accomplish this exact thing.  If you prefer using an extruded boss/base cylinder you can use the “Up to Surface” option which will result in the same results.  If you have another favorite way to do this type of thing please feel free to share.