The title kind of sounds like it could be the headline of a relationship article but this post is actually going to be about fully constraining your model in an assembly.  When inserting parts inside of an assembly it is really easy to fix the part and continue on.  This allows you to fully constrain a part so that it doesn’t move and it is extremely quick and easy.  However, as easy as it is I am a major opponent to the practice of mating because it is easy to quickly float that part, move it a very little amount and fix it again and no one would ever know.  That is until the part gets made and stuff comes out wrong.

As is with most things in SolidWorks there is an alternative way to quickly fully constrain a part with only a few quick clicks.  When you insert a part into an assembly you can mate the origins of the part with a coincident mate and select “Align axes”.  How you may ask, where here you go.

To start simply insert a part into an assembly.  Select the origin of the part you just inserted and the origin that you would like it mated to.  In the picture below you will see that I want to mate the origin of the part I inserted to the origin of the assembly.  After you select the 2 origins select the mate command to begin the process.

Automatically when you do this SolidWorks will select the Coincident mate as your choice, which is correct.  Here is where you will notice one difference from what you would normally see with the coincident mate.  Underneath this mate you will see a check box for the ability to Align axes.  This is automatically selected for you.  If you would wish to be able to rotate around the axis you would want to uncheck this option but for what we are trying to accomplish you will want to leave it checked.

Now all you have left to do is accept the mate and your part is now fully constrained inside the assembly as shown below.

Now this option might not always work for you but with a little thought into what you are hoping to accomplish in your assembly when making the part you may be able to incorporate a little design intent so that you are able to use it.

Well, there you have it.  Another alternative to a SolidWorks process that is a little safer than just fixing the part wherever it may land in the assembly.  I personally still like to mate all 3 planes of my part file to something in the assembly but that is just a personal preference.  How do you fully constrain the parts in your assemblies?  Let me know!

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.