There are many different ways to manipulate the model view in SolidWorks. This blog post will attempt to put most (all?) of the methods into one document for reference and describe a bit of history as to why some commands work as they do. Maybe you will discover some methods you didn't know existed before.
Mouse Manipulation
This is perhaps the most popular form of model view manipulation since it doesn't require you to move your hand off of the mouse and in conjunction with a couple of keyboard "accelerators", can perform most of the common view manipulations. Here is an outline of all of the manipulations you can make with your mouse. This help topic also outlines most of these methods pretty well.
Rotate View- middle mouse button drag. If the model is fully in view, SolidWorks rotates about the model centroid. If not, SolidWorks uses an algorithm to automatically select a piece of geometry that is in the view and projects a point onto it to rotate about (the entity and rotation point are highlighted in magenta during the rotation). SolidWorks used to always rotate about the model centroid regardless of whether the whole model was on the screen or not. For models that were off the screen, this often caused to the model to rotate in a way that it would "fly off the screen". There used to be an option in the View, Modify menu to always rotate about the screen center which some users preferred since it never had the problem of the model flying off the screen, but once we implemented this new behavior of automatically calculating a rotation point for the "trouble cases", the option was no longer required.
Rotate View about Entity - first, single click on a piece of geometry (face, plane, edge, vertex, sketch entity, etc.) with the middle mouse button and it will highlight in magenta and show a rotate cursor with a green line through it (as shown below).
Then drag with the middle mouse button. It will rotate about that entity until you let go of the middle mouse button and then the entity is deselected. One limitation; this function does not work while editing a sketch. When describing this functionality, I've heard many people describe using double click to select the entity and rotate, but you don't have to try to time this so you select the entity and hold the mouse down on the second click (that is a hard manipulation for some to do). Simply single click the entity with the middle mouse button and then click and drag the middle mouse button anywhere on the screen as you normally would to rotate; it is basically a select action followed by a rotate action (the select action is just done with the middle mouse since you might also be in the process of doing a normal left mouse selection set).
Roll View - Alt key and middle mouse button drag. This rotates the view parallel to the screen about the model centroid.
Pan - Ctrl key and middle mouse button drag. Note that in drawings, you do not need to hold down the Ctrl key; both regular middle mouse button drag and Ctrl middle mouse button drag work (since you can't rotate in drawings).
Zoom In/Out - Shift key and middle mouse button drag. If you have a wheel on your mouse (if not I highly recommend you get one with a wheel), then you can zoom in/out with the mouse wheel.
Turn Camera - Ctrl-Alt keys and middle mouse button drag. This is only available when you are viewing a camera view and are either editing the view or have turned off "Lock camera position except when editing" in the camera definition.
Related Settings - the following are a couple of useful settings to change the behavior of the mouse manipulation:
Zoom about screen center - under the View, Modify menu. Changes the behavior so that when using the mouse wheel, the view always zooms about the screen center (not many people want this, but some do). The default behavior (with this option off) is that when you zoom in with the mouse wheel, it takes the point that your mouse is over and zooms it towards the screen center. Once you get used to this, it works really well for zooming in on something that is not currently in the center of the screen. Sometimes people ask why we didn't just make it zoom up centered on the mouse location (instead of making it also move towards the center of the screen). We found in both internal testing and with users that zooming about the exact location of the mouse cursor more often caused the desired point of focus to wander off the screen when scrolling the wheel multiple clicks. The behavior we have now works very well. Note that regardless of this setting, zooming out always zooms out about the screen center (again, we found in testing this was the best behavior).
Reverse mouse wheel zoom direction- under Tools, Options, System Options, View. By default, scrolling the wheel forward towards the screen (or "up") zooms out (like you are pushing the model with the wheel away from the screen) and scrolling it towards you (or "down") zooms in like you are pulling the model towards you). Some people like to reverse this behavior if they are used to another system that does it in the opposite manner and especially if they are switching between the different systems often.
Mouse speed - under Tools, Options, System Options, View, View rotation. Defines the speed at which the view rotates for Rotate View, Rotate View about Entity, Roll View, and Turn Camera.
Keyboard Manipulation
The following are default keyboard shortcuts in the SolidWorks installation for manipulating the views.
Spacebar–brings up the view orientation dialog for choosing standard views, saving/recalling user defined views, and changing the standard view definitions (i.e. switching all the orthogonal views so for example front is top, bottom is front, etc.) This last functionality is very useful if you are used to a coordinate system that has Z pointing up instead of Y pointing up.
F - Zoom to Fit
Z - Zoom Out
Shift+Z - Zoom In
Ctrl+1 thru Ctrl+7 - These function keys are defined as the standard orthogonal views as follows: Front, Back, Left, Right, Top, Bottom, and Isometric
Ctrl+8 - Normal To (see below for more details about the Normal To function).
Ctrl+Shift+Z - Previous View. This is like Undo, but for undo of view manipulation instead of entity/feature creation/edit.
Arrow Keys (Up, Down, Left, Right)- Rotates the view by a predefined increment, about the model centroid, around the screen's horizontal or vertical axis (see Related Settings below).
Shift+Arrow Keys (Up, Down, Left, Right)- Rotates the view 90 degrees, about the model centroid, around the screen's horizontal or vertical axis.
Ctrl+Arrow Keys (Up, Down, Left, Right) - Pans the model.
Alt+Arrow Keys (Left, Right)- Roll View - Rotates the view by a predefined increment, about the model centroid, parallel to the screen (see Related Settings below).
G - brings up a magnifying glass that can be used to more easily make selections or to inspect portions of the model without having to change the overall view scale.
Ctrl+R- Redraws the screen. This used to be required a lot in the early days of SolidWorks when we used to have a lot of what we called "screen poo", but I never use it anymore. Due to improvements in the SolidWorks algorithms over the years, the graphics always seem to be up to date now. We used to have a button on the toolbars by default for this too, but again, it is not required so it is not visible by default.
Related Settings - the following are a couple of useful settings to change the behavior of keyboard view manipulation.
Arrow keys - under Tools, Options, System Options, View, View rotation. Defines the angle increment used for the Arrow Key and Alt+Arrow Key view rotation.
Zoom to fit when changing to standard views - under Tools, Options, System Options, View. Defines whether or not a zoom to fit operation is performed any time you switch to one of the standard views.
View transitions - under Tools, Options, System Options, View, Transitions. Defines whether or not the view animates to the new orientation when choosing a standard view or to view Normal to. If turned on, controls the speed of the animation. The animation is often useful, especially when looking normal to an entity so you don't "lose track" of the orientation of your model.
Reference Triad
Prior to SolidWorks 2009, the Reference Triad in the bottom left corner of the graphics area as shown in the image below was truly there only for orientation reference.
Starting with SolidWorks 2009, the Reference Triad can now be used to manipulate the view. The following manipulations can be made with the triad.
Select Axis - Click on an axis to look along that axis. This is equivalent to selecting a standard orthogonal view, but without making the mental mapping in your head as to which view is which related to your model. Note that if you are already looking normal to one of the orthogonal views, you can reverse the direction (for instance from front view to back view or vice versa) by clicking the axis that is currently pointing at or away from you (for instance, the Z axis on the triad as shown in the two orientations below).
Alt+Select Axis - Rotates the view about the arrow by a predefined increment. This uses the same angle increment as Tools, Options, System Options, View, View rotation, Arrow Keys.
Ctrl+Alt+Select Axis - Rotates the view about the arrow by a predefined increment in the opposite direction as Alt+Select Axis.
Shift+Select Axis - Rotates the view about the arrow by 90 degrees.
Ctrl+Shift+Select Axis - Rotates the view about the arrow by 90 degrees in the opposite direction as Shift+Select Axis.
Mouse Gestures
Introduced in SolidWorks 2010, this is a quick interface for executing commands by simply dragging the mouse while holding the right mouse button. While this is fully customizable, by default, in a part and assembly mode, the mouse gestures are set up to switch to the standard orthogonal views. I won't go into any detail here but will talk about mouse gestures in a future post. The detailed help on mouse gestures is available here.
View Related Toolbar Buttons
Most of the functions I have mentioned so far and quite a few more are available on toolbars (either by default or can be customized on). You can either put viewing buttons on the Heads-Up View Toolbar, Regular Toolbars, the Menu Bar, or the CommandManager. Most of the view related toolbar buttons are located in Tools, Customize, Commands, View. In many cases, it is quicker to use the mouse or keyboard shortcuts for the viewing functions so the toolbars aren't used as often. The exception may be if you are using a laptop without a mouse or a tablet PC where the buttons can be very useful. Some of these toolbar buttons that are commonly used for selections such as Normal To and Zoom to Selection are also available on appropriate Context Toolbars.
Normal To
The Normal To function allows you to change the view to be looking normal to various geometry. The documentation for this functionality is here. The following behaviors are supported:
- In an active sketch, but nothing selected -> views normal to the sketch (squares it up on the screen)
- Select a feature defined by a single sketch -> views normal to the sketch that defines the feature
- Select a planar face or plane -> views normal to the planar face or plane
- Select a cylindrical or conical face -> views along the axis of the face
- After one of the first selections above, make a second selection of a planar face or plane with Ctrl+select then use Normal To will orient the model so the second planar face is pointing up in the view. Without a second selection, the rotational orientation of Normal To is defined by the "natural direction" of the selected object. This "natural direction" is the same as where the Y axis of a sketch would point if you were to sketch on that selection and in most cases, relates to the global coordinate system of the part. Most users use Normal To with a single selection and then use Alt+arrow keys to rotate the view into a desired orientation if necessary.
- After choosing Normal To for any of the above, selecting Normal To again will flip the view 180 degrees (looking at the back of a selected face or plane for instance)
- Prior to SolidWorks 2010, if you were not in a sketch and didn't pre-select a piece of geometry before selecting Normal To, SolidWorks would prompt for a piece of geometry to look Normal To. Starting with SolidWorks 2010, if you are not in a sketch and have nothing selected, Normal To will switch to the closest orthogonal view orientation. This is a very quick way to "square up" the view and one of my favorite little shortcuts added to SolidWorks 2010. This new behavior is documented here.
Hopefully I documented most of the default ways that you can manipulate the model view in SolidWorks. Of course, you can get additional hardware that can also manipulate the model and can increase your productivity even more. If I have missed any common ways to manipulate the model view, please comment and I will update the blog post.
Enjoy,
Wilkie
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