Like most things in SolidWorks, there are several ways this can be done. Probably the simplest starts with orienting the model the way you want the drawing view to be. That can be done a variety of ways. Two of the simplest are starting with one of the standard views and rotating by holding down Ctrl and using the right and left arrow keys on your keyboard, or by Ctrl+selecting two non-parallel surfaces and then the Normal to button from the Standard Views toolbar, which will place the model with the first face selected normal to your screen, and the second surface selected at top. When you have the model oriented the way you want, hit your spacebar. That will bring up the Orientation dialog box. Select the New View icon.
Name your view and save, and the View will be available to use in your Drawing. Select it from the view's PropertyManager.
If your drawing view has the correct face normal to the screen, but you need to rotate it, you don't need to create a new view. Just click on the drawing view to highlight it, then click on the Rotate View icon in your heads-up toolbar (see below). That will allow you to enter a value for how much you want to rotate it. It will rotate counter-clockwise, so if you want it rotated 90° clockwise you'll need to enter -90°. By the way, I occasionally have a body that comes into the drawing at an odd angle because that's how it's oriented in the model. When that happens, and I want it horizontal or vertical, I place a sketched line in the view, make it horizontal or vertical, then use the Smart Dimension or Measure tool to determine the angle between it and a model edge. That's a big help with knowing what value to enter for Rotating the view. Delete the line and dimension after determining the value.
Another option for rotating a view is to select an edge of a drawing view, go to Tools > Align Drawing View, and select "Horizontal Edge", "Vertical Edge", etc., but you may or may not get the results you want.
Still another option is to go ahead and insert a view, then right-click on it and choose Drawing Views > Relative View.
That will take you to the model where you can choose which faces (or Planes) you want front and right. If this is a multi-body part you will also have an option to choose which body or bodies you want included in the view. When you click OK in your model it will place a new drawing view oriented according to your selections. You can now delete the original view if it's not needed. This might be a good option if you're in a multiple user environment, because if someone updates the model's standard views it won't affect drawing views that were inserted using this method.
Relative View was one method commonly used for showing selected bodies before the Select Bodies... button was added (see How can I show a single body of a multi-body Part in a Drawing?), but I don't believe I've used this method since then. Once you've clicked Okay you can't go back and edit your selections, which is one big reason I don't like to use it. I described it here because it's an option for a drawing view orientation without the need to create a new view in the Part file.