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Every once in a while, a question comes up on the forum or through other paths about the orientation of the global coordinate system and related view triad in SolidWorks. Users wonder why the Y-axis is pointing up and X-Z represents the top plane or table top when looking down from the top, while in some other CAD or CAM systems they may have used, the Z-axis is pointing up and X-Y represents the top plane or table top. Well, unfortunately, there are at least two defacto "standards" in the modeling industry for the orientation of the global coordinate system. I call them the Y-up and Z-up coordinate system standards. Both of these coordinate systems are right hand rule coordinate systems, they just happen to be rotated differently. So, neither of these systems is "wrong" and as they say, that is the great thing about standards...so many to choose from .


The good news is that there are a couple of ways to overcome issues users may encounter while working with SolidWorks alone or in conjunction with other systems because SolidWorks uses a Y-up coordinate system as default.

 

Switching SolidWorks to use a Z-up coordinate system:

 

You can switch SolidWorks to emulate a Z-up coordinate system. This can be done for any individual part or assembly document or you can do it in your part and assembly templates so all new parts and assemblies have this orientation.

 

Image of empty SolidWorks document before changing orientation:

y-up.gif

To switch to a Z-up coordinate system for all new part documents:

  1. Open a new part.
  2. Hit the spacebar and pin the View Orientation dialog.
  3. Double click on Front to switch to a front view.
  4. Shift click on the z-axis of the view triad (looks like a blue ball at the center of the triad from this angle in the lower right corner of the screen) to rotate the view 90 degrees. An alternative method is to use Alt-leftarrow on the keyboard 6 times to rotate the view 90 degrees (assuming the setting for arrow key view rotation in Tools->Options->System Options->View is set to the default value of 15 degrees).
  5. Single click on Top in the Orientation dialog and then select the Update Standard Views button (second one on the Orientation dialog). This command updates the view orientations so the view you are looking at (rotated Front view) is now considered the Top view.
    orientation_dialog.gif
  6. Rename the default planes to be correct for the new orientation. You can rename each default plane by single clicking twice on the name in the FeatureManager tree or one single click once and then select F2. The mapping is Front becomes Top, Top becomes Right, and Right becomes Front.
  7. Save the part as a new template or overwrite your original template.

 

Image of empty SolidWorks document after changing orientation and renaming planes (I also rotated the view for the screenshot so Z is facing up in the viewport):

z-up.gif

 

To switch to a Z-up coordinate system for an assembly, repeat steps 1-7 for a new assembly document.

 

To switch any existing part or assembly to a Z-up coordinate system, open the document and perform steps 2-6. Unfortunately, these models are already built using references to the original planes and orientation so you cannot easily re-orient the original features. However, if you do want to re-orient the solid or surface bodies, you can use the Move/Copy Body feature which will add a feature that rotates the bodies. Also note that using the "Update Standard Views" option on existing files can drastically affect drawing views created from the part/assembly in question (a warning message indicates this when using the command) so be careful in making this change if you do have drawings of the particular model.

 

Exporting Data into a Different Coordinate System:

 

If you have models built in the Y-up system that you need to export to a CAD/CAM system that uses Z-up coordinates, you can do so by first making a Coordinate System at the origin that has the Z-up. To do so:

  1. Create a Coordinate Systemleaving the coordinate system origin blank and selecting the right plane as the X axis and the front plane as the Y-axis.
  2. When exporting to formats like IGES, STEP, etc. using Save As, choose the Options button and set the Output coordinate system to the newly created coordinate system.

 

If your preferred approach is to use the Y-up global coordinate system for general modeling, but still want to easily export to a Z-up system, you can create and save the Z-up local coordinate system into your part and assembly templates and use that for exporting without having to create it in every part.

 

I hope this helps working in whichever global coordinate system you prefer.

 

-Wilkie

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 about scene floor - This setting is accessed via the right mouse button while over blank space in the graphics area. When this option is turned on, it changes the behavior of view rotation across all documents. When the option is on, SOLIDWORKS rotates more like a turntable around the Y axis (by default) so the model acts like it is sitting on a floor that you are rotating around to look at the model. You can change what plane is used for the floor in the Edit Scene PropertyManager.

 

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).
cursor.gif

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 few 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. Starting with SOLIDWORKS 2013, by default, it also brings up the view selector around the model, which is useful for selecting standard views as well as some other useful views of the model. There is a button to turn off the view selector in the view orientation dialog. See this help topic for more information about the view selector.

 

Ctrl+Spacebar - Starting with SOLIDWORKS 2013, brings up the view selector around the model, which is useful for selecting standard views as well as some other useful views of the model. See this help topic for more information about the view selector. Note that the view selector was in a fixed orientation in SOLIDWORKS 2013 and 2014; it was updated in SOLIDWORKS 2015 to come up in the same orientation as the model and rotate with the model view.

 

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.

triad.gif

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).
triad2.gif

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

 

Copyright © 2009 Dassault Systèmes SolidWorks Corp. All rights reserved.
Do not distribute or reproduce without the written consent of Dassault Systèmes SolidWorks Corp.

This blog post is the seventh in a series of technical tips about the SolidWorks User Interface. Call the series "Everything you wanted to know about -----, but were afraid to ask". The first few posts will be about the various types of toolbars available in the system. This post is about the SolidWorks Context Toolbars.

 

Context Toolbars

Context Toolbars were introduced for part and assembly documents in SolidWorks 2008 to provide easier access to the most common commands/options that relate to the current selection. SolidWorks 2010 adds the Context Toolbar for Drawing documents. The following image shows an example of the context toolbar alone on the left and the context toolbar on top of the right mouse button shortcut menu on the right:

context-toolbar.png

These toolbars work similar to the “Mini Toolbar” introduced in Microsoft Office 2007; on selection, they show up partially transparent and become opaque if you move your mouse onto them or disappear when you move your mouse away from them (assuming you don’t want to use the toolbar). The context toolbar is positioned very close to the mouse when making selections in the FeatureManager tree (similar to the Mini Toolbar in Office) but is positioned further away when making selections in the graphics area so it is easier to make multiple selections of geometry without moving your mouse away to dismiss the context toolbar first. The context toolbar also disappears if you hit the CTRL key to make multiple selections and comes back when you let go of the CTRL key.

 

The default behavior is that the Context Toolbar shows when you select an object with the left mouse button. It also shows at the top of the shortcut menu if you use your right mouse button to make a selection (or after you have made a selection). You can customize when the Context Toolbar is used through Tools, Customize, Toolbars; choosing to use it for left click (selection), right click (shortcut menu), for both, or for neither.

 

The buttons shown on the context toolbars are hard coded and cannot be customized by the user. SolidWorks has chosen to put the most commonly used commands from the shortcut menus onto the Context Toolbars for easier access. It takes a little bit of time to learn the icons, but many users find this approach much more efficient once learned. There are tooltips on the icons to help describe what each button does. Another benefit of the context toolbars is that the icons are in a more predictable location than on the standard shortcut menus and can be used with less "hunting". Once users become familiar with the icons and their placement, they can often even use the buttons by "muscle memory" instead of visual scanning for their location.

 

If users see anything I have missed about Context Toolbars in this blog post, please comment and I will try to update the blog.

 

The following are previous blog posts about toolbars:

      Regular Toolbars

      The Menu Bar

      The CommandManager

      The Heads-Up View Toolbar

      Toolbar Flyouts

      The Shortcut Bar ('S' key)

 

Enjoy,

Wilkie

 

Copyright © 2009 Dassault Systèmes SolidWorks Corp. All rights reserved.
Do not distribute or reproduce without the written consent of Dassault Systèmes SolidWorks Corp.

This blog post is the sixth in a series of technical tips about the SolidWorks User Interface. Call the series "Everything you wanted to know about -----, but were afraid to ask". The first few posts will be about the various types of toolbars available in the system. This post is about the SolidWorks Shortcut Bars ("S" Key).

 

Shortcut Toolbars ("S" Key)

The Shortcut Bars are user customizable toolbars that were introduced in SolidWorks 2008. The intention of the Shortcut Bars is to allow users access to commonly used commands in different "environments" with very little mouse movement. There are four versions of the Shortcut Bars, one each for parts, assemblies, drawings, and sketches (the default Shortcut Bars for each environment are shown below):

ShortcutBarAll.gif

To invoke the Shortcut Bar, simply hit the S key and the Shortcut Bar will popup right next to the mouse. The Shortcut Bar disappears as soon as you select a command from it or click anywhere else in the SolidWorks application window. The keyboard shortcut used to invoke the Shortcut Bar can be redefined in the Others category in Tools, Customize, Keyboard if desired.

 

To customize what commands are on the Shortcut Bar, when the Shortcut Bar is up, choose Customize from the right mouse button shortcut menu on the Shortcut Bar as shown below:

ShortcutBarCustomize.gif

The Customize dialog will open to the Commands tab and you can customize buttons on/off of the Shortcut Bar like any other toolbar. When the Customize dialog is up, you can also resize the shape of the Shortcut Bar by dragging any one of the edges. Repeat the procedure in each of the document modes to customize the four versions of the Shortcut Bar.

 

The Shortcut Bar is a good interface for users who want access to many commands with little mouse movement, yet don't want to have to memorize many individual keyboard shortcuts. Many power users have adopted the Shortcut Bar as their primary interface to accessing commands, hiding the CommandManager and regular toolbars so they have a very large area for their model display.

 

If users see anything I have missed about the Shortcut Bar in this blog post, please comment and I will try to update the blog.

 

The following are previous blog posts about toolbars:

      Regular Toolbars

      The Menu Bar

      The CommandManager

      The Heads-Up View Toolbar

      Toolbar Flyouts

 

The last topic in the series about toolbars will be:

Context Toolbars

 

Enjoy,

Wilkie

 

Copyright © 2009 Dassault Systèmes SolidWorks Corp. All rights reserved.
Do not distribute or reproduce without the written consent of Dassault Systèmes SolidWorks Corp.

This blog post is the fifth in a series of technical tips about the SolidWorks User Interface. Call the series "Everything you wanted to know about -----, but were afraid to ask". The first few posts will be about the various types of toolbars available in the system. This post is about Flyout Tool Buttons in SolidWorks.

 

Flyout Tool Buttons (or Toolbars Flyouts)

There are two general types of toolbar flyouts in SolidWorks.

  1. Toolbar associated flyouts- These flyouts are derived from the regular toolbars and were introduced in SolidWorks 2004. Think of these as taking a regular toolbar and embedding it into another toolbar as a single button. When you hit the button, it flies out a list of all of the commands that are defined on the regular toolbar associated with that flyout. To change the definition of the flyout, you simply make the regular toolbar visible, customize the buttons that are on that toolbar, and then hide the toolbar. Add-in toolbars, if implemented using the CommandManager APIs, automatically create a toolbar associated flyout for each API toolbar. The Reference Geometry and Curve toolbar flyouts as shown below are examples of toolbar associated flyouts that are shown on the Features tab of the CommandManager by default.
                   toolbarlinkflyouts.gif
  2. Hard coded flyouts- These flyouts were introduced in SolidWorks 2008 to allow more flexibility in grouping similar commands together into single buttons. There is a predefined set of these flyouts in SolidWorks and they cannot at this time be customized by the user (although we are considering adding customizability in the future if there is enough demand). There are three different behaviors for these flyouts:

 

    • Simple flyout- this type of flyout has one single behavior whether you hit the icon or arrow portion of the flyout (the mouse over effects only show one "hit" zone). The behavior is to always flyout and show the commands that are defined on the flyout (same behavior as the toolbar associated flyouts). The icon shown on the top level button is an icon chosen to represent all of the contents of the flyout. The View Settings flyout on the Heads-Up View Toolbar is an example of a simple flyout:
                   simpleflyout.gif
    • Last used flyout- these flyouts have two zones on the top level button, one for the icon, and one for the arrow flyout. The icon portion always shows and executes the last command used from the flyout. The Line flyout on the sketch tab of the CommandManager is an example of a last used flyout:
                   lastusedflyout.gif
    • Most commonly used flyout- these flyouts have two zones on the top level button, one for the icon, and one for the arrow flyout. The icon portion always shows and executes the first command listed on the flyout. When we defined these flyouts, we put the most commonly used command of the group at the top of the flyout list. The Pattern flyout on the Features tab of the CommandManager is an example of a most commonly used flyout:
                   patternflyout.gif

We chose to implement these three different behaviors so that we had flexibility depending on the type of commands on the flyout. Our research showed that the majority of users disliked the top level icon always changing to the most recently used command, especially in cases where the icons of the commands within the flyout are drastically different. In such cases, users would have trouble finding the button again once the icon changed. For cases where the icons are similar and there is no clear “winner” on the flyout as to what users would use most (such as rectangle), we used the "last used" type. For cases where there was clearly one type of command used more than others (such as Line vs. Construction Line or Convert Entities vs. Intersection Curve) we chose the "most common" type. The simple flyout is the least used but is used in cases where we want to group less commonly used commands under one button.

 

You add flyouts to the toolbars in the same manner as other toolbar buttons; drag/drop them from the Tools, Customize, Commands dialog. The flyouts are available from the “Toolbar Flyouts” category. The image below shows the customize dialog for the flyouts category and highlights the different types of flyouts (this is the order they are always shown in this dialog):CustomizeDialog.gif

A general behavior of all toolbar flyouts is that only commands that are currently available show on the flyout; i.e. if a command is currently grayed out in the top level menus, it is completely hidden from the flyout. This is a similar behavior to the right mouse button context menus where unavailable commands are hidden.

 

Lastly, there are some other hard coded flyouts "sprinkled" throughout other toolbars in the system that have special behaviors and do not fall into the architecture described above. Examples of these are the Select, Undo and Redo flyouts in the Standard toolbar and the Change Suppression State button in the Assembly toolbar.

 

If users see anything I have missed about Toolbar Flyouts in this blog post, please comment and I will try to update the blog.

 

The following are previous blog posts about toolbars:

      Regular Toolbars

      The Menu Bar

      The CommandManager

      The Heads-Up View Toolbar

 

The next two topics in the series about toolbars will be:

Shortcut Bars ('S' key)

Context Toolbars

 

Enjoy,

Wilkie

 

Copyright © 2009 Dassault Systèmes SolidWorks Corp. All rights reserved.
Do not distribute or reproduce without the written consent of Dassault Systèmes SolidWorks Corp.

You may have seen a post I recently created on the SolidWorks Blog about Usability Testing @ SolidWorks. We are always looking for feedback on both released products and new things under design and development. There is no need to travel to Concord to participate in our usability feedback sessions - you can participate right from your desk. We use GoTo Meeting web conferences.

 

Two examples, right now.

 

First, we are looking for somewhere between eight and ten people to participate in a study about 3D ContentCentral. It doesn't matter if you are a frequent 3D ContentCentral user, or if you have never used it before - we are looking for a wide range of 3D ContentCentral experience. As long as you have about an hour to spend from your office, and have a working Web connection, you can participate. This study is helping to improve navigation and 3D ContentCentral home page design. This study is in progress now, and we expect to be running it through to the middle of next week.

 

Next, we are also looking for eight to ten relatively new SolidWorks users. Specifically, we're looking people who have less than 12 months of experience using SolidWorks, although you may have some (not a lot mind you, some!) experience with other CAD packages. This is a study about sketching and modeling in SolidWorks. As with the 3D ContentCentral study, this study is in progress now. Likewise, you can participate from your desk.

 

If you are interested in possibly participating in either of these studies, please send email to usability@solidworks.com and provide us with a couple of hour time slots that would work best for your schedule.

 

More generally, we keep a list of people who are interested in participating in future feedback sessions. This list is our first "go to" point when we are looking for input and feedback on our designs. If you're interested in joining this pool of SolidWorks usability testers, please fill out our short sign up questionnaire. When your profile matches an upcoming feedback session, we will contact you.

 

Tom Spine

SolidWorks User Experience

This blog post is the fourth in a series of technical tips about the SolidWorks User Interface. Call the series "Everything you wanted to know about -----, but were afraid to ask". The first few posts will be about the various types of toolbars available in the system. This post is about the SolidWorks Heads-Up View Toolbar.

 

Heads-Up View Toolbar

The Heads-Up View Toolbar was added at the top of the document graphics area in SolidWorks 2008 to provide easy access to viewing functions that affect the graphics area. Below is an image of the default Heads-Up View Toolbar.

viewtoolbar.gif

In SolidWorks 2008 and 2009, this toolbar contains a limited set of viewing commands and which commands are currently visible on the toolbar is controlled by using the right mouse button shortcut menu on the toolbar. To completely hide the toolbar in SolidWorks 2008 or 2009, you must deselect all of the buttons in the visibility list. If you have hidden the entire toolbar to make it visible again, move your mouse to the very center of the top of the graphics area and hit the right mouse button to get the visibility menu.

 

Starting with SolidWorks 2010, this toolbar has been upgraded to be consistent with normal toolbars; hide/show visibility of the entire toolbar is controlled in the same manner as Technical Tip: SolidWorks Regular Toolbars and customization is also handled in the same manner (i.e. any button can be added/removed from the toolbar through the use of Tools, Customize). The only differences between this toolbar and a regular toolbar are: 1) It cannot be undocked. 2) Visibility control is stored twice; once for drawings and once for parts/assemblies. 3) Customization of what buttons are shown is stored twice instead of once; once for drawings and once for parts/assemblies.

 

This toolbar shows in the currently "active" viewport of the graphics area (of which there is only one by default so it is always visible). To activate a viewport, click in the viewport.

 

When we added the Heads-Up View Toolbar, we also added some new flyout toolbar buttons to make some of the most common viewing functions easier to access. These flyouts can be placed on any toolbar (not just the Heads-Up View Toolbar) by dragging them from Tools, Customize, Commands, View. The specific view flyouts that we added in SolidWorks 2008 are:

 

View Orientation- This flyout has all of the standard view orientations, user defined orientations, and options for splitting/linking the viewports. The standard views are shown in a common orientation that is easier to interpret than the linear layout of the View Orientation dialog or the Standard Views toolbar. Below is an image of the view orientation flyout shown with two user defined views on it.

vieworientation.gif

Display Style- This flyout consolidates the five different display styles into one flyout, occupying less space. The user can still customize the interface to have the individual display style buttons on their toolbar if they use certain styles more often than others and want direct access with one click instead of two.

displaystyle.gif

Hide/Show Items - This flyout performs the same function as selecting items to hide/show in the top level View menu, but overcomes the number one complaint about the menu which is you cannot select/deselect multiple items without invoking the menu multiple times. Unfortunately, the single select behavior is a behavior of Microsoft menus which cannot be overridden, so we introduced the Hide/Show Items flyout as an improved method to hide/show multiple display items. The image below was taken in SolidWorks 2010 where starting with Beta3, the icon in the lower right corner is used for toggling dimension names on/off (this is now a per document setting instead of a system setting).

hideshow.gif

Apply Scene- This flyout was added to easily change between different background scenes. You can cycle to the next scene in the list by pushing the icon portion of the button or you can choose a specific scene by using the flyout portion. Users often ask how to make their background white and the image below shows the "Plain White" background selected. Note that scenes are per document, so if you don't want to use different scenes for different documents (i.e. you want a plain white or other background for ALL documents), go to Tools, Options, System Options, Colors and choose from one of the other options under "Background appearance".

applyscene.gif

Display Settings - This flyout contains three less commonly used display settings (again, consolidated into one flyout to save space). Again, the user can customize the interface to have these individual display style buttons on their toolbar if desired.

displaysettings.gif

If users see anything I have missed about the Heads-Up View Toolbar in this blog post, please comment and I will try to update the blog.

 

The following are previous blog posts about toolbars:

      Technical Tip: SolidWorks Regular Toolbars

      Technical Tip: SolidWorks Menu Bar

      Technical Tip: SolidWorks CommandManager

 

The next few topics in the series about toolbars will be:

Technical Tip: Flyout Tool Buttons

Technical Tip: Shortcut Bars ("S" Key)

Technical Tip: SolidWorks Context Toolbars

 

Enjoy,

Wilkie

 

Copyright © 2009 Dassault Systèmes SolidWorks Corp. All rights reserved.
Do not distribute or reproduce without the written consent of Dassault Systèmes SolidWorks Corp.

This blog post is the third in a series of technical tips about the SolidWorks User Interface. Call the series "Everything you wanted to know about -----, but were afraid to ask". The first few posts will be about the various types of toolbars available in the system. This post is about the SolidWorks CommandManager.

 

The CommandManager

The CommandManager was originally introduced in SolidWorks 2004 and was enhanced in SolidWorks 2008 and 2009. It originally was a "super toolbar" where you could simply choose as many normal toolbars as you wanted to be grouped into this super toolbar, so multiple toolbars could occupy the same space. You chose buttons in the "control area" of the CommandManager to indicate which normal toolbar you wanted to be active.

The main goal of the CommandManager was to allow access to many toolbars without taking up a lot of screen real estate since we know many users want as much space for their model as possible. It is obviously a tradeoff between space and mouse clicks, but we built some "smarts" into it so it would automatically switch the active toolbar when appropriate (like when going into or coming out of Sketch mode).

 

The CommandManager has now evolved into a tabbed container of toolbar buttons. It is similar to the Microsoft "Ribbon Bar" released with Office 2007, but is much more customizable and does not completely replace the menus. The user can make as many tabs as they like and put toolbar buttons and separators of their choosing on each tab. The CommandManager has three separate user customizable definitions (part, assemblies and drawings). There is also a "special" user customizable definition of buttons that shows up at the left side of the CommandManager when the user is in Edit Part in Assembly mode. Below is a picture of the current CommandManager:

CM.gif

 

Some users use the CommandManager for their most commonly used toolbars while others use it for their least commonly used toolbars (and use regular toolbars or other methods for more direct access with less clicks).

 

Below is a list of other behaviors that are available with the CommandManager:

  • You navigate between the tabs of the CommandManager by selecting the desired tab OR scrolling your mouse wheel when your mouse is over the CommandManager.
  • You can make the CommandManager a lot smaller by unselecting "Use Large Buttons with Text" (through Tools, Customize, Toolbars or right mouse button shortcut menu on the application/toolbar frame). This turns the text off and makes it about the size of a regular toolbar, with the addition of the tabs. Note that it is intended that the icon size itself is linked to the "Large icons" option in Tools, Customize, Toolbars and not controlled by the "Use Large Buttons with Text" option. This option was originally called "Show Descriptions" but users didn't seem to find that option and always asked "how do I turn off the large buttons" so we renamed the option to be more discoverable. The presence of the text is what makes the buttons large, not the icon size. Below is a picture of the CommandManager with the text turned off:

          CM2.gif

  • Most customization of the CommandManager is done when the Tools, Customize, Commands dialog is up, similar to customizing regular toolbars. Below are the things you can do while in customize mode.
    • Add an empty tab by clicking on the tab with the new tab icon on it (shown below) or by selecting Add Tab, Empty Tab from the right mouse shortcut menu on one of the existing tabs. If using the shortcut menu, the new tab is added after the tab where you used the shortcut menu.

                    CM-new.gif

    • Add a new tab pre-populated with all of the buttons from an existing toolbar by selecting Add Tab, <toolbar name> from the right mouse shortcut menu on one of the existing tabs.
    • Copy the definition of a tab from one document type definition (part, assembly, or drawing) to another by selecting Copy Tab to <document type> from the right mouse shortcut menu on one of the existing tabs. If the tab already exists in the target document type, it will ask you if you would like to over-write the definition.
    • Delete a user added tab by selecting Delete from the right mouse shortcut menu on one of the user added tabs. You cannot delete the tabs that are defined by default in the SolidWorks installation.
    • Rename a user added tab by selecting Rename Tab from the right mouse shortcut menu on one of the user added tabs.
    • Hide a tab by selecting Hide Tab from the right mouse shortcut menu on one of the existing tabs. Show a hidden tab (shown grayed in customize mode) by selecting Show Tab from the right mouse shortcut menu on one of the existing tabs. Note that you can also hide/show tabs when not in customize mode; simply select the name of the tab you want to hide/show from the right mouse shortcut menu when over any of the tabs.
    • Add buttons to a tab by dragging them from the Tools, Customize, Commands dialog onto the tab. When using "Use large buttons with text" mode, the default size/shape of the button is dictated by the adjacent button and you can tell what you will get by the "I" beam shape of where the button is dropped.
    • Remove a button by dragging it off of the tab or selecting Delete from the right mouse shortcut menu while over the button.
    • Change the "size/shape" of a button while using "Use large buttons with text" mode by choosing options from the right mouse shortcut menu while over the button. There are three different button sizes/shapes: without text, with text on the right, and with text below. The text below option is only available when the CommandManager is docked along the top of the SolidWorks window; text on the right is the only text option when the CommandManager is docked on the left, right, or undocked.
    • Add a separator before a button by selecting "Begin a Group" from the right mouse shortcut menu while over the button. A separator can be turned off by unselecting this option on the button that is just after the separator.
  • When you turn the CommandManager off (through Tools, Customize, Toolbars or right mouse button shortcut menu on the application/toolbar frame), SolidWorks automatically shows the regular toolbars equivalentto the visible tabs. This behavior was originally put in with SolidWorks 2004 when we wanted an easy way for users to turn off the CommandManager and get the equivalent regular toolbars (which was the default setup out of the box before the CommandManager was introduced). Now that we have other preferred methods to access commands such as the Shortcut Bar, we may want to take this behavior out to save users from having to go back and hide the regular toolbars after turning off the CommandManager.
  • Starting with SolidWorks 2009, you can dock the CommandManager on the top, left or right of the SolidWorks application or have it undocked. Simply drag anywhere on the CommandManager to move it, and to dock it, drop it on one of the three icons showing the possible docking locations. To have it floating/undocked, simply drop it anywhere in "space". The icons are used for docking as it becomes too difficult to get such a large piece of UI into a desirable floating position if the entire top, left and right of the application window are dockable locations.
  • Starting with SolidWorks 2009, you can dock regular toolbars adjacent to the CommandManager. Simply drag them to the right of the CommandManager if docked on top or below the CommandManager if docked on the left or right.

     

    If users see anything I have missed about the CommandManager in this blog post, please comment and I will try to update the blog.

     

    The following are previous blog posts about toolbars:

          Technical Tip: SolidWorks Regular Toolbars

          Technical Tip: SolidWorks Menu Bar

     

    The next few topics in the series about toolbars will be:

    Technical Tip: SolidWorks Heads-Up View Toolbar

    Technical Tip: Flyout Tool Buttons

    Technical Tip: Shortcut Bars ("S" Key)

    Technical Tip: SolidWorks Context Toolbars

     

    Enjoy,

    Wilkie

 

Copyright © 2009 Dassault Systèmes SolidWorks Corp. All rights reserved.
Do not distribute or reproduce without the written consent of Dassault Systèmes SolidWorks Corp.

     

This blog post is the second in a series of technical tips about the SolidWorks User Interface. Call the series "Everything you wanted to know about -----, but were afraid to ask". The first few posts will be about the various types of toolbars available in the system. This post is about the SolidWorks "Menu Bar".

 

The Menu Bar

The menu bar is the top-most portion of the SolidWorks application window (first introduced with SolidWorks 2008). The menu bar replaces the traditional Microsoft windows banner shown on most applications. Feedback from most users is that they want to maximize the amount of space for their model, so making use of this space makes sense instead of it being wasted on only the document name and windows controls. This practice is also starting to become fairly common with other applications like Microsoft Office 2007 and Apple iTunes also taking this approach. The image below shows what the Menu Bar looks like:

menubar.jpg

 

There are multiple areas within the Menu Bar as follows:

 

Logo/Menu Area: By default, the traditional Microsoft menus are hidden from view. In our research with customers through visits and focus groups, we found that most users only want to use the menus for uncommonly used functions. They prefer to access commonly used functions through other approaches such as toolbar buttons and shortcut keys. For these users, the menus don't always need to be present and more room can be made available on the menu bar for toolbar buttons. To access the menus, you can simply move your mouse over the logo and the menus fly out to the right. If your mouse moves over the menus, they stay up so you can select a menu item. If you exit the logo area from the bottom, the menus will disappear (so you can more easily access the rest of the menu bar if you didn't intend to use the menus). If you click on the logo area instead of just hovering over it, the menus will fly out and "stick" out until you either choose a menu item or click elsewhere to dismiss the menus. Below is an image of the Menu Bar with the menu "flown out":

menubar-unpinned.jpg

Of course, not all users like the menus to be hidden all the time or do not like the flyout behavior, so you can make the menus permanently visible by selecting the push pin at the right end of the menus. Below is an image of the Menu Bar with the menus pinned.

menubar-pinned.jpg

Note that the flyout behavior of the menus has been improved in SolidWorks 2009 SP04. If you like the idea of the flyout menus, but they would fly back in unexpectedly when you were using them, you may want to give the unpinned behavior another try. Specifically, improvements were made so the menus do not fly back in as often when your mouse moves from the logo area to the menu area or when your mouse rides along the top of the menu (when the SolidWorks application is maximized).

 

Standard Microsoft keyboard navigation of the menus still works with these SolidWorks menus, regardless of whether or not they are pinned. When you hit the Alt key to navigate, the menus will first flyout if they are not pinned, and you can navigate further from there using the underlined letters or arrow keys. Some users leave their menus unpinned and then use the Alt key as a hot key just to get the menus to fly out and then use mouse navigation from there (it saves a little mouse movement/dance over to the logo and then to the menus). Note that SolidWorks respects the Microsoft setting under Display Properties, Appearance, Effects to hide/show the underlines on the menus.

 

Toolbar Area: There is a section on the menu bar where toolbar buttons can be added and by default, this area replaces the "Standard" toolbar from SolidWorks 2007 and previous versions. Buttons are added/removed from here in the same manner as any regular toolbar; simply drag and drop from the Tools, Customize, Commands dialog. Note that the icons in this area are always 16x16 pixels and purposely do not change with the "Large icons" setting used for other toolbars.

 

Document Name: The currently active SolidWorks document name is shown in the blank space in the middle of the menu bar.

 

Search Box: The SolidWorks Search box is used for searching for SolidWorks models and other documents.

 

Help Button: The icon portion of the button brings up the main SolidWorks Help. The flyout arrow gives access to all of the menu items on the regular SolidWorks Help menu.

 

Window Control Buttons: The standard windows functions of Minimize/Maximize/Restore/Close are present on the right of the menu bar.

 

If users see anything I have missed about the Menu Bar in this blog post, please comment and I will try to update the blog.

 

The following are previous blog posts about toolbars:

      Regular Toolbars

 

The next few topics in the series about toolbars will be:

The CommandManager

The Heads-Up View Toolbar

Toolbar Flyouts

The Shortcut Bar ('S' key)

Context Toolbars

 

Enjoy,

Wilkie

 

Copyright © 2009 Dassault Systèmes SolidWorks Corp. All rights reserved.
Do not distribute or reproduce without the written consent of Dassault Systèmes SolidWorks Corp.

This blog post is the first in a series of technical tips about the SolidWorks User Interface. Call the series "Everything you wanted to know about -----, but were afraid to ask". The first few posts will be about the various types of toolbars available in the system. This started as one comprehensive post about toolbars, but turned out to be too long so I have split it up. The first post will be about "regular toolbars".

 

Regular Toolbars

SolidWorks has always strived to follow Microsoft standards and since SolidWorks 95 has supported "standard" Microsoft toolbars. I put standard in quotes because Microsoft has enhanced their toolbars over time, yet have not provided those enhancements in their standard toolbar toolkit. Our programmers have had to program such enhancements into the SolidWorks toolbars over the years so you won't see a one-to-one behavior of SolidWorks toolbars to Microsoft toolbars (the amount of functionality you get with Microsoft toolbars varies between different Microsoft application anyway; the Office suite having the most advanced toolbars up until they removed them in Office 2007). For the rest of these toolbar posts, I'll call these "regular toolbars" since standard can be used to mean many things and is also the actual name of one of the regular toolbars in SolidWorks. For clarity, the following is the Curves toolbar which is an examples of a regular toolbar:

 

      CurvesToolbarSmall.gif

 

Toolbar visibility: The visibility of each of the regular toolbars is stored four different times; one visibility state for each document type (part, assembly, and drawing) and one state for when no documents are open. We've seen reports on the user forum where a user will say that the visibility is being controlled differently for different documents of the same type (for instance, 2 part documents). I am not sure how this could be possible since this visibility information is stored in the registry, not inside the documents. Certainly if it is repeatable, it should be submitted through their technical support representative.

The visibility of toolbars is controlled in the following places:

    • Using the right mouse button shortcut menu on the SolidWorks application/toolbar border.
    • View, Toolbars on the top level menus.
    • Tools, Customize, Toolbars

 

Toolbar position:Regular toolbars can be docked along the top, bottom, left or right of the SolidWorks application frame or undocked. There are a couple of exceptions of toolbars that contain horizontal controls (like the layer and web toolbars) that can only be docked on the top or bottom. When undocked, the shape of the toolbar can be changed to some extent (the separators in the toolbars force grouping and sometimes limit how you can shape the toolbar). The position of regular toolbars is stored in the registry once for each toolbar. We sometimes get requests for "locking" the toolbars into a particular position because the toolbars move around. Theoretically, the behavior should be that they are "naturally" locked in place unless they MUST move due to something else happening. Events that can trigger the toolbars moving are: 1) The SolidWorks window is resized down so small that it must push the toolbars together (eliminating empty space). 2) another toolbar becomes visible that is trying to occupy the same space - this can happen if you are trying to layout toolbars between different document types and put the same toolbar in two different positions between document types - remember, one single toolbar can only be in one position across the different document types. In past releases, we received a lot of complaints about toolbars moving around, but we have been diligent about fixing problems where this occurs unexpectedly so it really should not happen outside of the cases mentioned above (and perhaps for older API/Add-in toolbars mentioned below). Toolbar chevrons, as detailed below, were introduced in SolidWorks 2004 and further enhanced in SolidWorks 2005 and eliminated the problem of toolbars "jumping" to other rows/columns when the SolidWorks window was resized.

 

Toolbar size: There are two different sizes of toolbar buttons; small (16x16s pixel per icon) and large (24x24 pixels per icon). You choose between the sizes in Tools, Customize, Toolbars. As an example, the Tools toolbar is shown in both small and large size below:

 

ToolbarSmall.gif

ToolbarLarge.gif

 

Toolbar chevrons:If the SolidWorks window is resized down to a size such that all the toolbars on a row can not physically fit, each toolbar starting from the right/bottom are truncated and the truncated buttons are accessed through a chevron at the end of the toolbar. Below is an example of the Tools toolbar shown with the chevron expanded:

 

ToolbarChevron.gif

 

Customizing toolbars:You can add/remove buttons from toolbars by going to Tools, Customize, Commands tab and dragging/dropping toolbar icons on/off the toolbars. You can also remove buttons or move them between toolbars by using Alt-drag on the buttons at any time (without being in the Tools, Customize command). You are not restricted to putting buttons on the toolbar on which they are defined in the customize dialog. Any button can go on any toolbar. You cannot at this time make your own, blank toolbar. Most users who want a new toolbar simply take a toolbar they are not using otherwise, remove the buttons from it, and add the buttons they desire onto it. You can also add toolbars through the API as mentioned below.

 

API/Add-in Toolbars

Third party programmers and users with programming skills can program their own toolbars through the API. There have been various methods for creating toolbars through the API over the years. We suggest using the very latest "ICommandManager Interface" APIs which use the same underlying architecture as the regular toolbars in SolidWorks and provides the same customization ability to the end user. A complaint that comes up on the user forum somewhat regularly is that a third party's toolbar cannot be customized or used in the SolidWorks CommandManager. Unfortunately, this is because the add-in is using older toolbar APIs and must be upgraded to the ICommandManager Interface to take advantage of customization and the CommandManager. Please ask the maker of the add-in to upgrade their implementation if you want to customize the toolbar or use the buttons from it in the CommandManager or on other toolbars.  The older API toolbars also exhibit positioning problems occasionally and we advise using the new toolbar APIs as the code and architecture for these is more up to date.

 

If users see anything I have missed about regular toolbars in this blog post, please comment and I will try to update the blog.

 

The next few topics in the series about toolbars will be:

Technical Tip: SolidWorks Menu Bar

Technical Tip: SolidWorks CommandManager

Technical Tip: SolidWorks Heads-Up View Toolbar

Technical Tip: Flyout Tool Buttons

Technical Tip: Shortcut Bars ("S" Key)

Technical Tip: SolidWorks Context Toolbars

 

Enjoy,

Wilkie

 

Copyright © 2009 Dassault Systèmes SolidWorks Corp. All rights reserved.
Do not distribute or reproduce without the written consent of Dassault Systèmes SolidWorks Corp.

Hi All,


Welcome to the new User Interface blog. Tom Spine and I will be the primary contributors to this blog, but we likely will have "guest bloggers" from the SolidWorks User Experience Design and User Interface Development groups. We already have many ideas for blog subjects, but we would like to hear your ideas on what types of blog subjects relating to user interface would help you day to day in your use of SolidWorks. Please post comments back to this blog post with your ideas and we will add them to our list for future blog posts.

 

That's it for now. Short and sweet.

 

Thanks,

Wilkie