Customize Mouse Gesture tool bar: You may have heard of the new mouse gesture activated shortcut in SolidWorks 2010. It is activated by holding down the right mouse button, and dragging the mouse to the right. A donut shaped shortcut tool will appear that can be customized to your liking. By default, the donut will have 4 shortcuts on it, but that can be customized to 8. Customize the mouse gesture shortcuts the same way you customize any toolbar in SolidWorks, which is by right clicking over a fixed toolbar and selecting "Customize". There is a new tab in the customization dialog now titled "Mouse Gestures" From there, you can add your own choices of features and tools to the gesture based popup, which is context sensitive. For even more choices than the maximum of 8, you can add a shortcut to the shortcut toolbar normally activated by the "S" key.
Parametric Text Notes in Sketches: In SolidWorks 2010, you can now link a text note in a sketch to a custom property. When adding a text note in a text, just click on "Link to Property" in the property manager of the text being added. From here you can link to either a custom property, or a SolidWorks Special Property like the configuration name. With this method, the text, and any feature that is created from the sketch it resides in, will update every time the property changes. This a great technique for cases where a property like a part number or mold ID number needs to be molded or cast into a part.
Technical Resource Document - SolidWorks Rx: SolidWorks Rx is a troubleshooting tool that SolidWorks includes to give you first-pass, diagnostic information about your SolidWorks usage. For complete instructions - visit our technical resources page.
Midplane End Condition with Instant 3D When creating an extrusion by dragging the green arrow, hold down the "m" key to switch to a Midplane end condition. This only works if you are using Instant 3D and creating a feature by selecting the green arrow that is available after selecting an unabsorbed sketch.
Isometric Section View in Drawing Ever want to show a section view displayed in an isometric view? This is simple to do and gives your drawings the real feel for your parts and assemblies. Create a section view like you normally would and then right click on the new view. You are given the option "Isometric Section View," select this and it will change it into a 3D view. If you don't like it, right click again and "Remove Isometric View."
Free Structural Members for Weldments SolidWorks' Weldments can use a sketched "wireframe" representation of a welded structure, and then apply industry standard structural shapes (beams) to the wireframe sketch entities. But, "of the box" we only get a few examples of the type of profiles used with the Structural Member tool (ansi & iso, angle, rectangular tubing, channel). Instead of creating the missing structural profiles you need, there are extensive libraries freely available for download directly from the Design Library. Under SolidWorks Content -> Weldments you will find links to profile libraries defined by ANSI, ISO, DIN, JIS and others including Unistrut. Unzip the contents of the downloaded file(s) and include that folder under File Locations -> Weldment Profiles. The scope of these libraries is impressive. ANSI has over 2000 profiles including steel & aluminum, wide flange, T sections, MC channel, pipe, and much more.
Gauge Tables Reduce Errors Gauge tables are simple spreadsheets used by Sheet Metal that can impose manufacturing or company standards for material thickness, allowable bend radii and bend allowance technique. Typically applied through the Base Flange command, once a gauge table is selected any Property Manager fields that require input values then change to drop-down pick boxes. Now, unless you override the table, you can no longer key in a non-standard material thickness. Also, for any allowable thickness you must select an allowable bend radius, unless you override the table. Create gauge tables for specific materials (304SS vs. copper) or bending techniques (air bending vs. bottoming), different machines, customers or vendors. Check out the examples found in \lang\english\Sheet Metal Gauge Tables. Be sure to include the path to your saved tables under File Locations -> Sheet Metal Gauge Table.
Mouse Gestures New in SolidWorks 2010 is Mouse Gestures. You can use a mouse gesture as a shortcut to execute a command, just like a keyboard shortcut. To activate a mouse gesture, just right-drag your mouse and the guide will appear showing the command mappings for your gesture direction. This can be customized for up to eight gestures for drawings, assemblies, parts, and sketches. To view or edit the current mouse gesture assignments, click Tools > Customize. From the Customize dialog box, select the Mouse Gestures tab.
Add a plane even quicker You can quickly add a plane without going to Reference Geometry. All you need is an edge. Add a plane normal to edge by simply clicking the edge, then clicking Insert > Sketch. This will open a sketch on a newly added plane that is normal to the edge at the closest edge end point.
Speedy Sketching Ever wonder what Rapid Sketch does? So did I! This command can be turned on from the Sketch toolbar to blaze through sketch creation faster than ever before. Once activated choose the sketch tool of your choice and then hover over any planar face in your model. Start sketching once you see the Rapid Sketch plane appear. No need to exit sketches or change tools when moving between separate sketch planes, just hover, sketch and repeat! All the sketches are immediately saved in the FeatureTree as soon as you start another.
Sketching With Style The Power Trim function of the Trim command tool does a lot more than just trim like a scalpel. The real "power" comes from the lesser known artistic abilities. With Power Trim active left click and hold on a sketch segment and pull in either direction to gently trim or extend.
Weldment Groups You can now define a weldment group, a collection of related segments in a structural member. Configure a group to affect all its segments without affecting other segments or groups in the structural member. You can define a group in a single plane or in multiple planes. A group can contain one or more segments. A structural member can contain one or more groups.
Escape Key is a Time Saver You can press 'Esc' to interrupt long operations such as drawing view creation or long drawing document rebuilds. The operation will immediately cease so that other operations can be completed.
Customizing Hole Notes The Hole Wizard can be a useful tool, unless it's notating your holes incorrectly. This tip will describe what to look for and links to resources that will assist in customizing your hole annotations. Look for the file calloutformat.txt located in C:\Program Files\SolidWorks\lang\english directory. There are two versions of the file within this directory, calloutformat.txt and calloutformat_2.txt. calloutformat_2.txt is easier to understand. This file allows you to customize the order the variables in the hole note are written in, add/remove variable information, and adjust text values. Once the file has met company standards, simply place on a network location and point all Solidworks client machines to that file using the tools/options/File Locations pulldown from within Solidworks.
Adding a quick light source to a part By splitting faces on components, you can assign specific appearances to an individual face. Then, with the PhotoWorks add in turned on, apply an appearance to the split face, select the advanced tab at the top, select the illumination tab and a constant option, adjust brightness as necessary. When rendered, these can produce great looking LED strings or other luminescent features. Great for Marketing and Sales!!!
3D Content Central for free add-ins I'm sure everyone at some point has thought "surely other people need a feature in SolidWorks that does <insert your favorite item>." The good news is that there is a place where you can search for solutions, www.3DContentCentral.com. Many people are aware that this site has many parts and assemblies, both from other users and also certified by vendors.
This particular tip is referring to the macros on that site. I'll state first off that the macros are not tested by SolidWorks, so be careful what you download. With that out of the way, a particularly handy macro allows you to find the mass of an individual component in an assembly. www.3dcontentcentral.com
To use this macro, select a component, then run the macro. A popup dialog box will show you the selected component's file name, configuration name and mass (in kg). With very little effort, the macro can be edited to display the mass in lbs or any other preferred units.
Ok, so you can do this all through the existing interface, but I wanted to bring attention to 3DContentCentral's list of macros in hopes that many of you will use it and add to the list of macros.
So, you're asking how to find a component's mass from an assembly? Simply click Mass Properties, then in the Selected Items box, right click to clear the assembly from the list and select any component you want to analyze. Once you click Recalculate, you'll see the mass, volume, surface area and everything else you're used to seeing.
Component Configurations in a jiffy Adding configurations to parts is easy to do, but what if you need create the same configuration in an assembly and then activate the part's new configuration? The simplest way to accomplish this is from the assembly. As an example, we'll walk through creating a configuration called Simplified to multiple components at a time.
Open an assembly in SolidWorks and go to the Configuration Manager. Right Click on the top entry and click Add Configuration which will naturally add a configuration to the assembly. Name the configuration "Simplified" and before you click OK, scroll down to the bottom of the Property Manager to the Parent/Child Options. Expand this section to see all the components of the assembly (parts and sub assemblies). Place a check next to each component that needs a Simplified Configuration. If you choose to check a part that is part of a subassembly, be sure to check the subassembly as well. Once you click OK, you can then click on the Feature Manager and will notice that all the components selected (and the top level assembly) have the new Simplified configuration active. Open or edit each component and modify it as needed.
Instant 3D Modify Dimension Dialog Box is Reduced If you have instant 3D turned on then when you click on a dimension only once it shows a reduced dialog box that only allows you to change the dimension. If you want to bring up the regular dialog box, double click on one of the blue dots associated with that particular dimension and it will bring up the regular modify dimension dialog box.
Purple Dimensions From time to time everyone needs to create a cut. Have you ever left the sketch under defined for the one edge that is away from the part? Sure, everyone has! Why do you leave it under defined? Well that's because when you create a drawing and import the model items, you don't need that dimension to be shown on the drawing so you leave it off. The best practice is to throw a dimension on the entity and then uncheck the button "Mark dimension to be imported into a drawing." This turns the dimension purple and allows you to fully define your sketch.
Bi-directional Material Property Editing from Title Block I'm sure everyone at some point has thought "surely other people need a feature in SolidWorks that does." The good news is that there is a place where you can search for solutions, www.3DContentCentral.com. Many people are aware that this site has many parts and assemblies, both from other users and also certified by vendors.
This particular tip is referring to the macros on that site. I'll state first off that the macros are not tested by SolidWorks, so be careful what you download. With that out of the way, a particularly handy macro allows you to find the mass of an individual component in an assembly. www.3dcontentcentral.com To use this macro, select a component, then run the macro. A popup dialog box will show you the selected component's file name, configuration name and mass (in kg). With very little effort, the macro can be edited to display the mass in lbs or any other preferred units.
Ok, so you can do this all through the existing interface, but I wanted to bring attention to 3DContentCentral's list of macros in hopes that many of you will use it and add to the list of macros. So, you're asking how to find a component's mass from an assembly? Simply click Mass Properties, then in the Selected Items box, right click to clear the assembly from the list and select any component you want to analyze. Once you click Recalculate, you'll see the mass, volume, surface area and everything else you're used to seeing.
Control Part Sizes Using an Assembly Design Table Some top-down assembly designs may benefit from a design table structured as a configurator that builds mating parts based off direct, dimensional input. By first creating an assembly sketch containing only construction geometry that has the dimensions required to control the sizes of the parts, you can reference and control the dimensions of the control sketch in the assembly design table, enabling a convenient way to configure all the required component sizes easily from the assembly level. Use top down design techniques like "Convert" and "Up to Vertex" end conditions, referencing the control sketch when designing the parts top down. The control sketch dimensions can then be controlled by the assembly design table. Without this technique, The user must switch back and forth between different part configurations to control the various component sizes, making a much less direct method of configuring the assembly.
Add an item to your design library Have a commonly used part, sketch, assembly, or even feature? Add it to your design library, making it easily accessible each time you need to you use it. Your design library can be found on the right hand side of your screen in your task pane. Verify your task pane is visible under VEIW. Once in your design library you can add either a folder or an individual file. If you add an individual file you must add it to a folder in your design library. You can also create a folder in your design library. Hover mouse over design library task bar to choose your weapon of choice.
Standardize your company's part templates Set your template for your company so there is no confusions about what units to use. Open a new part under the templates tab of the dialog box. Set your Document Properties under options. Save the new template in a folder as a Part Template (*.ptrdot). To add the folder to your template tabs, go to options and add the folder under file locations, Document Templates.
Large Assembly Loading lf you've ever needed to work on components in a large assembly, but wanted the ability to make specific selections without loading the entire assembly, you're in luck. When loading an assembly from File, Open select the assembly, check off "Quick view / Selective open" and then click Open. A graphical view of the entire assembly will load in a fraction of the full load time. Select the desired components to load into memory and click Open. If you miss a selection, or would just like to open more parts, click Show Hidden Components on the Assembly toolbar and choose the additional components you'd like displayed.
RealView Rendering Want to make your models and assemblies look even more realistic without using PhotoWorks? Of course you do! Simply turn on RealView graphics, along with Shadows and Perspective View (all of these can be found under the menu View, Display). Next, change the scene to Ambient Occlusion. While not in motion your models will be quickly rendered using video game shading technology. For even better appearance be sure to apply the appropriate materials to your components and turn off any other on screen distractions like origins or planes (View, Hide All Types). Please note - you must have a RealView supported graphics card to take advantage of this functionality. Visit www.solidworks.com to verify.
Customize your Keyboard Commonly used tool can be linked to your keyboard so the tap of a key will turn on your tool. My personal favorite is linking the temporary axis to the T key. This customization can be used for almost anything in SolidWorks to reduce mouse miles, from inserting a feature to saving a file. Where to find: Tools, Customize, Keyboard tab. Be sure to check your keyboard setting to maximize efficiency and personalize your SolidWorks.
Clean up your Feature Tree A large number of features can be a sight for sore eyes. Clean your feature tree up by placing features in a folder so you can find them with ease while editing. Right click on a feature, select Add to New Folder. A new folder will be placed in your feature tree. By default you will be asked to name the folder. To place other features in that folder, just click and drag the feature into the new folder. Remember, you can also name each feature and sketch by slow clicking on the feature to edit the name. This will save you time when editing parts.
Disabled Bodies in Flow Simulation After Make use of disabled bodies in SolidWorks Flow Simulation to focus in on detailed results in a particular area of your study. Simply create a new part or body in your model, disable it from the Flow study using Component Control, and then make use of its faces and volume to display results in that area.
Equation-driven Motors in SolidWorks Motion Using expressions for motor definitions in SolidWorks Motion allows you to create feedback loops. For example, you could use this to maintain the velocity of a vehicle driving over a series of hills at 10.0 m/s. First, create a result graph {linear velocity of vehicle} showing the linear speed vs time. Next, define a motor using an expression like; Motor speed = 10000 degrees/sec x (10.0-{linear velocity of vehicle}).
How to move a group of sketch entities: After creating a series of sketch entities you may want to move the sketch entities around on the screen as a group. When attempting to click and drag an entity you may notice that only that entity will move leaving the other entities where you left them. This often happens if there aren't enough constraints to hold the entire sketch together. Here are a couple tips to help you move under constrained sketch entities around the screen as a group.
Tip 1: Move Entities. Move entities allows you to pick a group of entities and move them around. Using Delta X and Y coordinates or by picking From/To locations.
Tip 2: Stretch Entities. Similar to Move entities, stretch entities will allow you to move a group of sketch entities but keep them attached to any entities that you did not select to move. This will result in the entities between the moved and stationary entities to stretch, hence it's name.
Tip 3: Align Sketch. It's in an unlikely location, but the Align Sketch tool found on the 2D to 3D toolbar allows you take all the entities in your sketch and map any point on that sketch to the origin. Simply select a point on the sketch and click the Align Sketch button.
Tip 4: Ctrl + Click-and-Drag. You may already know you can copy sketch entities by highlighting them and clicking and dragging the selected entities while holding the Ctrl key. But if you let go of the Ctrl key halfway through the drag, you will move the entities instead of copying them. Use this tip to your advantage, it doesn't require you to click a command off a toolbar.
Creating Midpoint Reference Points on the Fly: The hard way to create a midpoint or reference point on a piece of sketch geometry was to create a physical reference line or a reference point in your sketches so you can dimension to that midpoint. There is a better way though: when you are using the SmartDimension tool you can right click a line (or other entities) and choose Select Midpoint from the menu you are now able to dimension to the midpoint.
How do you put a perspective view on a drawing? The traditional way to add "Perspective" within parts and assemblies is not available within the drawing environment, but it is still possible to place a perspective view into a drawing. To show a drawing view with perspective, you will need to create a custom view in the part or assembly file and that is the trick.
Do you use Excel and SolidWorks? Not only can F2 rename a feature, sketch, configurations, planes, etc. but it can also help inside excel. Take a look at a cell that has a formula. If you want to edit the formula, typically you would click in the cell and then click in the address bar. Next time you need to edit the formula, move to the cell and hit F2. This will take you to the end of the formula and allow you to start editing.
Quick way to set the End Condition: Whenever you are creating an extrusion (cut or boss) you have to set your end condition (unless you are setting it to a blind depth which is default). Instead of going to the property manager and using the pull down, try using your Right Mouse Button and selecting from the list displayed. This will reduce your mouse miles significantly!
SolidWorks Explorer: This tool is used to find references and rename SolidWorks files. When you first start this program, it will ask you for your PDMWorks user name and password. Some users might not be using this function so is there a way to disable this from popping up automatically? There is an option you can uncheck once you have by passed that message and SolidWorks Explorer is running. The third icon from the left is "Options." Once you have the options dialog box open, select the "Add-Ins" tab and then uncheck the box next to "SolidWorks Workgroup PDM."
Input Dimension Value: Designing in metric but thinking in inches? Try using the optional dual units setting in the Measure tool. Just click the Units/Precision button in the top header of the "Measure" dialog box. Here, you will find the options for precision and custom units settings in the Measure tool, including the "Dual Units" option.
Dual Units in the Measure Tool: Ever get tired of having to double click every new dimension in a sketch each time one is placed in order to edit the dimension's value? Try using the System Option "Input Dimension Value." This option will cause the Modify box to open every time a new dimension is placed in a sketch so that the value can be edited.
Convert to Sheet Metal: The Convert to Sheet Metal command lets you specify the thickness, bends, and rips necessary to convert a solid part to a sheet metal part. This tool which combines the shell, rip and insert bends command into one can be found from Insert, Sheet Metal, Convert to Sheet metal.
Format Painter: This tool has been moved from SolidWorks Utilities to the core SolidWorks package. Format Painter copies visual properties from dimensions and annotations to other dimensions and annotations in the same document or another document. Format Painter is supported by parts, assemblies, and drawings.
Reuse your SolidWorks Motion Elements: You can save motion elements such as springs, motors or force specifications for reuse in other models. Add motion elements to the Design Library as you would add other items. All motion elements in the Design Library are saved with the .sldsimfvt extension. While in any motion study, drag saved motion elements from the Design Library to your model.
Make Complex Sketches Easier: In SolidWorks 2009, you now have the ability to generate an equation-driven sketch. The tool can be found under Tools, Sketch Entities, Equation Driven Curve and the inputs required are an equation and ranges for any parameters used in the equation. Complex polynomials and harmonic equations can be easily used as well allowing users to make very complex sketches.
Easier Appearance Manipulation: In 2009, colors and textures have been combined in to what are now knows as appearances. Because of this one source of display data, factors such as RealView graphics and whether the model has been rendered in PhotoWorks do not cause display information to be lost. This leads to much easier application and manipulation of appearances. Appearances can now be applied from the Appearance tab in the task pane, the display pane or the Appearances selection within any right-click menu.
Fully Define Sketch: The fully define sketch feature allows you to automatically generate relations and dimensions within a sketch. This is particularly useful when 2D data has been imported in to SolidWorks and you need the data to be fully parametric. This is also a very useful tool when removing in-context references and still maintaining the underlying geometry. The fully define sketch tool can be found from Tools, Sketch Tools, Dimensions, Fully Define Sketch.
