The SOLIDWORKS 2016 Premiere is right around the corner, and this year's theme includes "How It's Made" presentations by local best-in-class companies. As we count down the days until the first event, let's take a look at a series of objects made in SOLIDWORKS.
How It's Made
It's very rare now to see a phone without a case. If cases didn't exist, many of our phones wouldn't stand a chance. As durable as some phones can be, it seems as though it's human nature to drop them as much as imaginably possible. I know that holds true for me.
So, let's get to it. How can a phone case be modeled in SOLIDWORKS?
Cell Phone Case
In this example, we will start with a completed model of our phone. Whenever I am looking for a model for reference, I always check 3D Content Central. However, I found a pretty detailed and native SOLIDWORKS Nexus 6 model on GrabCAD that I'm going to use. The model had some inaccuracies in the dimensions, but it works well for our purpose.
Now, the first thing we will need to do is create a base piece for our phone case. There are many ways we can do this with lots of cuts and extrusions and lofts and sweeps. However, there is a much easier way to do this using only two features.
We'll start with a surface offset. [Insert >> Surface >> Offset...] We are going to offset all of the faces pertinent to the case at a distance of 0in. This will create a surface body using all of the relevant faces. We will select all exterior faces, excluding the front faces, camera faces, and any faces for jacks and charger ports.
Once we create our copied surface body, we will use the Thicken command to create a solid body for our case. [Insert >> Boss/Base >> Thicken] Be sure to point the direction away from the phone and to disable "Merge Result."
Just like that, we have a phone case! We still have to add clearance for our charge cable, earphone jacks, and buttons.
Now we can add allowances by using the move face command. We selected only the external faces of the model for our surface offset. This left holes for our earphone jacks, charger cables, and buttons. Now we can select the faces of those holes and use the move face command with the "Offset" method to add clearances. [Insert >> Face >> Move]
For the right-side buttons, we need to make a few modifications to our case to make them accessible. First, we'll take out the bridge piece between the two buttons, as it just provides an unnecessary obstacle. For this, we just use an extruded cut with the "Up to Next" end condition.
Now we'd like to have a nice chamfer on this edge to make the buttons more accessible. However, as you can see, SOLIDWORKS wasn't able to add a very deep chamfer before the geometry became inconsistent.
We can get around this by creating a small chamfer that does not interfere with the surrounding edges and faces and following up to make it deeper.
We'll use a move face feature on the chamfered faces with the "Translate" method. This allows us to bring the surface down and manually create the chamfered edge that we needed.
Now we need to do something similar to the earphone jack to chamfer that edge. The result will give us a nice chamfered edge, and the cable should now have enough clearance to fit.
Now we finish it up with some cosmetic fillets and chamfers, and we are ready to customize!
Now you can call yourself a phone case master.
As always, happy modeling!
By: Cody Pendzich, Technical Support Representative