You've probably figured out that you can use the three "base" workplanes to make most initial sketches (the top, front, and side planes), and that you can create new "offset workplanes" using the base ones. The base planes and offset planes can be used to create most sketches used for a conventional part, but you may run into problems when forced to to make a three-dimensional angled cut or extrusion, that doesn't lie parallel to any of the three base planes.
You can perform this operation by making a lofted elipse, but that gets tricky since you have to compensate for the angles in the elipsis dimensions. You can also use a 3d sketch in Inventor, but personally I find them a hassle in comparison to the method I'm trying to explain on this page. It involves making a new workpane, based off an axis, which is tied to a sketch that you can view and change anytime you want. When you change the sketch, it'll automatically move the workplane with it. Parametric modeler at its best!
The most practical application for this in paintball markers is making an angled hole in the part (usually a complex part). However, it should be said that you should avoid having to make an angled workplane like this unless you have no other option (for size reasons, probably). Angled cuts like this can only be made on special machinery, or after making a custom "fixture" that will hold the part stationary at an angle, and use a regular drill press (or other machine). Needless to say this type of thing should be avoided since it will drastically increase the cost of the part.
For models you make that have no need to be produced, though, it's just fine.
Both Inventor and Solidworks have support for this feature. In fact, it's the exact same process for either program. I'll explain both of them.
Inventor:
For the purposes of this I will just use a sample block to start the model (2x1x1). The part looks like this:
The first step is to create your "construction" 2d sketch that will tie into the position of the workplane. This should be positioned depending on the feature you will use the workplane to create. For instance if you are making a cut into the side of the part, you may wish to make the sketch on the outside edge so you can measure it (and later on use the measurement to make the cut in reality). In the same part I chose the front face as pictured...
The sketch you need to make is simple, it just needs to use one line, which you can dimension to the surrounding parts. I made a vertical line 0.45" up from the bottom, 0.7" from the front. You'll use the end of the line to base the workplane.
When finished, exit the sketch and click the "work axis" command (located in the toolbar, or the pull-down menu). Move the mouse over the top point of the line, and a dot with an X will appear around the endpoint (it will be red when you move the mouse over it, then blue when you click on it).
After selecting the endpoint of the line, you will need to designate the direction of the axis. You can't simply click on the base axis in the leff-hand menu, rather what you have to do is select a workplane that bisects the axis you want to make. This means the axis will pass perpendicular through the "bisecting" plane. In the example below I select the side plane, which will make the axis horizontal through it. You can select the base workplane in the left-hand menu, or a plane on the surface of the model itself, it just depends on what part you're trying to make.
The new axis looks like this (below). Note that you can use this same method to create axes anywhere on your part, without having to make two points.
Now it's time to make the new workplane. Start be clicking the "workplane" command (on the toolbar, or in the pull-down menu) and select the axis you just made.
Next step is to select a workplane (or face on the model) that will connect perpendicular with axis you selected. For example I clicked on the front side of my sample block, which will make a horizontal plane to connect them. (when you move the mouse over the face, a preview of the new plane will appear, as shown below)
As soon as you click it, you're presented with an "angle" dialog box. This allows you to adjust the angle of the workplane around the axis you used to create it. This can be different depending on the face used to create the plane, but in my example a 90º angle would be flat horizontal. I adjust the angle to 60º, which produces this result...
The 3d workplane is now established. At this point I suggest removing the visibility for the 2d sketch and work axis you've already created. You probably won't need to see them to make your operations (if you do, then leave them visible). I turned them invisible here.
Click on the workplane to start making a sketch. In this sample part I'm going to make an angled drill cut into the side of the part, so I'll be making a profile that will be revolved when finished. Note that you will have access to specific Project Geometry lines and points based on the origins and axes of your angled workplane. You can dimension the part to anything you make in the sketch (even the Project Geometry of the part, so long as Inventor can resolve it [which it usually can unless it's a spline/loft surface]).
This is used to make a 3d feature on the part, and has many uses for fourth-axis components.
Now, the beauty of the parametric modeler is that you can edit the "construction" 2d sketch you previously made, and it will change the position of the workplane and thus the position of the features you make. In this example I change the position of the vertical line and it shifts the workplane backward, moving the workplane along with it.
This next picture shows the model before I changed the construciton sketch, and also the position after I changed it.
The hole moves down and back instead of "just back". If you don't immeditely understand why this happened, just know it's because of the angled workplane's origin axes.
Solidworks:
This is the exact same method as described in Inventor. I start with this basic block solid:
You'll have to make a sketch to base your "construction" 2d sketch. In this example I chose the side face on the block...
Make a line which will be used to base your new workplane. In this example I made the line below...
Now you'll need to produce a work axis. Select it in the menu shown below, then click on the endpoint of the line.
After clicking on the endpoint, you'll have to select a bisecting plane to create the axis. As explained above this is a workplane that will pass around the axis perpendicular. I select the side face of my block model, which makes a horizontal axis as shown.
Now it's time to make the 3d workplane. Start by selecting the plane command in the menu shown here.
Click on your axis, then you'll have to select a perpendicular face that will cross the new workplane. In this example I click on the front face of my block model, which will make a horizontal plane passing through it.
The menu to the left will prompt you with options on the new workplane. One of them is the angle, which I adjust to 45º. SolidWorks will show you a preview of the new plane...
The 3d workplane is now established. You can choose to hide the "construction" features (2d sketch, axis) if you don't need to see them to make your 3d operations. Either way, you can use the new 3d workplane to make 3d features on the part, such as drilling an angled hole through the part (which is what I show in this example). Create a new sketch on the new workplane and make your sketch.
After revolving it, this creates the following cut:
By editing the "construction" 2d sketch you can control the position of the 3d workplane, and thus adjust the position of the 3d features on it. In this example I change the height of the 2d line I already made, to change the 3d hole I already made.
Applications:
As mentioned one of the more important uses of this is the ability to make an angled cut on a part, that doesn't lie on any of the "base" planes for the model. When doing this type of thing, you can make your construction 2d sketch on the outside face of the part, then create specific dimensions for the axis line (as described). When you make the angled sketch on your 3d workplane, you can tie the center of the drill bit (revolution axis) to the same position as the work axis. This creates a realistic model that could be produced in reality by measuring the position of your construction 2d sketch, and the two angles of the revolution feature (the angle of the workplane, then the angle of the drill bit lines on that plane). The best example of this that I can think of is the internal eye ribbon "canal" on a Shocker body, which is an angled hole drilled using a drill press and custom fixture, based on the outside measurements that I just described. This angled hole connects the outside of the Shocker body with a vetical hole on the underside, to allow the vision ribbon a path to the inside of the frame.
Expensive to make, but in this case it's easier than the alternative (making the body longer to eliminate one of the angled axes).