Sheet Metal: In SolidWorks 2011 drawings, you can now have a visible bounding box for a sheet metal flat pattern. Right click the drawing view, and select Properties. Below the bend note display setting, there is now a check box in the View Properties tab to display the bounding box. This box can be dimensioned, and the grain direction is a parameter of the flat pattern (accessible by editing the flat pattern feature in the model).
Detailing: Dimensions can be moved or copied from one view to another. Drawing views can be copied or cut then pasted to an alternative drawing sheet. Sheets can be re-ordered within a document or copied to an entirely different drawing. Experiment with this functionality by exploring your right click menus, the Edit menu, and the copy/cut/paste Windows shortcuts.
Defeature: New in SolidWorks 2011, with the defeature tool, you can remove details from a part or assembly and save the results to a new file in which the details are replaced by dumb solids (that is, solids without feature definition or history). You can then share the new file without revealing all the design details of the model.
Walk-Through: Walk-Through - You can use the Walk-through function to explore or create a video of the 3D geometry of plants or other systems. You "see" the geometry of the system as you maneuver through it. You can save what you see and play it back for further study. To activate the function, click View > Lights and Cameras > Add Walk Through.
Modify Sketch Dimensions as You Go: In SolidWorks, it is standard practice to just sketch the geometry close to, but not exactly what you need. Dimensions set the final value. You can have SolidWorks prompt you for input at the time you create every dimension by turning on the system option, "Enable onscreen numeric input on entity creation". This option is found under Options>System Options> Sketch.
Placing the First Component in Assemblies: For every assembly, there must be a first component. When placing the first component of a bottom up assembly, be sure to just click the green checkmark at the upper left of the "Insert Component" dialog and the first component will be locked to the origin of the assembly. No mates are required to locate it that way, and any mass properties that are dependent on the center of gravity will be based off a known point, the origin.
Go Directly to Document Properties, Don't Pass Go: If you ever want to change the document properties you may get tired of going to Tools ---> Options ---> Document Properties. A quicker way get there is to RMB on the name of the file (at the top of the tree) and there is a selection for "Document Properties."
View Assemblies Easier with Tree Filter: If you have ever worked with a large assembly, it becomes difficult to work with if you need to make changes to the mates per component. As you may know there is a folder in each component which groups the associated mates. So instead of viewing the features of each part, put those in a folder and show the mates and dependencies instead. There are a couple of ways to show this functionality. The first is to turn it on through the View pull down menu ---> FeatureManager Tree --->By Dependencies. The second would be to Right Mouse Button (RMB) on the name of the assembly at the top of the FeatureManager design tree ---> Tree Display ---> View Mates and Dependencies Extra Credit: Make a hotkey so you can toggle the tree between the two ways.
Thickness Analysis Tool: The Thickness Analysis tool may prove helpful to those needing to ensure a plastic part will not have sink marks in thicker areas or assist in the placement of vents and gates within a mold. Knowing where the thin areas of a part are may also assist in machine ability issues. As the name implies this tool allows for the evaluation of a parts thickness. The analysis can be set to show regions thicker or thinner than a specified value, the ability to localize analysis for large or complicated parts and the ability to create reports of the analysis results. The report can have the analysis applied to predefined views for design review documentation and clarification for those not able to view the model within SolidWorks.
Use AutoTrace to create features from pictures inserted into Sketches: If you have a picture that you would like to turn into a sketch to create a feature, there is a simple utility built into SolidWorks to do just that. It's called AutoTrace and if you want to use it, you'll need to click on Tools, Add-ins and enable it first. Once enabled, it will allow you to take a sketch picture and have SolidWorks trace the image into splines. Not every image will lend itself well to the AutoTrace feature. For best results, use a high resolution, high contrast BMP file that has nice clean edges. An image editing application, such as GIMP, can be used to tidy up and convert the picture prior to inserting it into SolidWorks. To learn more, search the Help file for "AutoTrace" and "Sketch Picture." Display States in Part Files: Don't forget that Part Files now have Display States, too. You can control different display properties for various objects in the part file (see table). Each variation can be stored as a display state to easily toggle between your saved preferences. Just like assembly display states, you can create new ones from the bottom of the Configuration Manager. You can toggle between existing states from the Configuration Manager or by right clicking on the >> button at the top of the Feature Manager.
Hide/Show
Display Mode
Appearance
Transparency
Parts
X
Bodies (Solid and Surface)
Features
Hideable features such as sketches
Faces
Going with the Flow: Preparing your SolidWorks model for a Flow Simulation study. Everyone has preferred ways of preparing 3D geometry for a FEA or CFD study, here are some "best practices" for a smooth transition between design and, in this case, a thermal and/or fluid flow analysis.
> The best time to think about analysis is when creating the original 3D model. Recommend creating a secondary "Flow" configuration, where a version of the part or assembly can be created that is better suited toward the requirements of the analysis. This might include suppressing cosmetic features and parts, sealing open seams in sheet metal, creating lids to be used for boundary conditions and creating disabled volumes to be used for mesh refinement or post processing. It is much easier to think about these things as geometry is created than to go back and do the work during the analysis setup. Create a Flow configuration for each part, where necessary, and reference these simplified configurations in the top-level assembly using its own Flow configuration. This may sound like a lot of work, but when incorporated into your standard procedures, it should greatly reduce the setup time associated with your Flow simulation. > Run an interference check using "treat coincidence as interference" to understand where parts have face to face contact and where they do not. Although interfering components won't necessarily cause a problem in Flow Simulation, they may not be desirable in thermal studies with conduction. > Run the "Check Geometry" tool within flow to confirm that Flow has detected a fully enclosed fluid volume (for an internal Flow study) and that no invalid contacts exist. Invalid contacts such as line or point contact between components are a frequent cause of problems in a Flow study. Flow Simulation might "fix" some of these issues internally and will highlight others that it cannot fix. Click through any reported issues and they should highlight in the graphics area. Take the necessary steps to remove point and line contact by adding or removing material. > In some situations, Flow may not be able to locate the problem that is causing the solver to fail. In these situations, it is necessary for the user to find the issue by inspection of the model or by using various "tricks of the trade." With experience, even these issues can be located without a great deal of effort. Start by creating a large rectangular (or whatever shape you wish) mulitbody or assembly component that envelopes half of the model. Anything within this new volume will essentially be absorbed by it and if the offending geometry is included, the problem should vanish. If the problem still exists, then move the block to the other side of the model. Refresh your model and study each time and use Check Geometry as needed to interrogate the model. When you have located the general area of the model that is causing the problem, then next step is to systematically reduce the size of the block until you have pinpointed the problem. This is an iterative process, but can move relatively quickly in most cases. If your problem involves an enclosure of some kind, run a separate test study on just the enclosure with no other components present. > Finally, with any analysis, particularly those that are prone to difficulties, always start with the most simple representation of the study and add complexity as needed until you reach your requirements. This is critical and will aid you in moving smoothly through the analysis process. It is all too common for engineers to throw everything into the mix at once, including beautiful, render-ready geometry and every analysis bell and whistle available, then wonder why they can't just push "Run" Think ahead and develop your own process for going from design to analysis and you should find Flow Simulation a fast and powerful tool for designing better products.
Importing Technique: For those who import files from other CAD systems into SolidWorks, often they run into situations where files will not knit properly and instead of importing a nice solid, they get unknit surfaces and gaps in their surface bodies. This may be because the tolerances between the surfaces may be larger than what SolidWorks can handle. Next time you import the surfaces try importing the bodies as unknit surfaces. Scale the surfaces down by a factor of 10 using the Scale Feather and then knit the unknit surfaces with the Knit Feature. The scaling will decrease the size of the gaps between surfaces and potentially within the tolerance range for the surfaces to be knit properly. After the surfaces are knit, rescale the file back up to by a factor of 10!
Delete Surface Holes: When working with imported geometry or surface modeling many users are already familiar with the Untrim command. Untrim will pull back the edges of a surface (typology) to reveal the underlying geometry of a surface when selecting edges. But Untrim is only effective for external edges of a surface you wish to untrim. When it comes to untriming internal edges of a surface like a trimmed internal hole or cut, Delete Hole is more effective and less resource intensive. To Delete Hole select one of the edges of the hole you wish to delete and hit the "Delete" key. A dialog will come up asking if you wish to delete the "Feature" or the "hole". Choose the hole. (note: delete hole does not work to remove gaps between surfaces only holes within surfaces)
Updating the Convert and Print Task Add-in in Enterprise PDM: When you upgrade an Enterprise PDM file vault to a new service pack (or version) - the existing convert and print task add-in (SWTaskAddIn) will not automatically update with latest version. If you do not update the add-in, it is possible that fixes done to the task add-in may not apply to the upgraded vault. To ensure you are running the latest, updated version of the task add-in (SWTaskAddIn), do as follows after the vault upgrade: 1. Verify which version of the current task add-in is used by right-clicking the enterprise tray icon > task host configuration: - If it is 2010 SP0 - version would read 2010000523 - If it is 2010 SP1 - version would read 2010010616 - If it is 2010 SP2 - version would read 2010020714 If using an old version, you need to upgrade the existing task add-in in the vault: 1. Open administration tool on a upgraded client - log in as Admin. 2. File > open > browse to c:\program files\solidworks enterprise pdm\default data\ 3. Load the "Convert_GB.cex" file. 4. Drag-and-drop SWTaskAddIn to the add-ins node (not the convert task). Select Yes to update the existing add-in. 5. Verify via the task host configuration that the updated add-in is loaded. 6. On clients that act as task host it is recommended to exit enterprise and log in again to the view to ensure the updated add-in is loaded.
SolidWorks Enterprise PDM with Mouse Gestures: You can use a mouse gesture as a shortcut to execute a command, similar to a keyboard shortcut. Once you learn command mappings, you can use mouse gestures to invoke mapped commands quickly. Every function available in the in-context menu offered by the SolidWorks Enterprise add-in can be assigned to a mouse gesture in SolidWorks 2010. To reassign a mouse gesture command in SolidWorks: 1. Create a new document 2. Load the SolidWorks Enterprise PDM add-in 3. Click Tools > Customize… and select the Mouse Gestures tab. 4. Set Category to Enterprise PDM 5. Click the Command column header to sort the commands 6. Choose one of the mouse gesture directions to reassign, and in the row for the new command 7. By default, four directions are available. Select 8 gestures to assign commands for eight gesture directions. 8. Click OK to save.
Direct Editing with Child Recognition: SolidWorks 2010 allows you the ability to directly edit parametric solids not native to SolidWorks. Direct editing will now import child features. Just select on the feature and edit. FeatureWorks will then recognize the feature and the child features, allowing you to edit as desired.
Hole Wizard Headaches: Remember the days of having to select a face first when using the Hole Wizard. No longer is that the case. In SolidWorks 2010 the Hole Wizard is smart enough to know if you want a 3D sketch or when you select the face it will us a 2D sketch. Take a look into your available standards too, notice Australian Standard (AS) is now available as well.
Pack and Go: You know where the assembly is, but how about all of the parts? Some of them might be on your desktop, a few in My Documents, others on a network drive. Sure, you could use File, Find References, but then what about the drawings? How can you safely copy these files? Pack and Go is a powerful and flexible file management tool. For example, when using it on assemblies there are options to rename parts/sub-assemblies, add a prefix/suffix to all files, and then save the files to a new folder or Zip file. It can also automatically locate and include drawings, simulation results, and PhotoWorks renderings! Pack and Go can be found under the File menu in SolidWorks, and is also available from right mouse clicking a document in SolidWorks Explorer. Please note - Pack and Go is not a suitable replacement for secure document revision control. That need is best satisfied by SolidWorks Enterprise PDM.
Rapid Dimension: New for drawings in SolidWorks 2010 is Rapid Dimension, enabling you to quickly place dimensions that are automatically spaced for easy reading. To access this feature, turn on the Smart Dimension tool and apply a dimension to a drawing view as you normally would. Once your selection has been made you'll notice the Rapid Dimension manipulator (halved or quartered pie pieces). Simply hover over the pie piece to preview the dimension, and left mouse click to confirm the position. If needed the spacing can be changed from Options, Document Properties, Dimensions, Offset distances.
Robust Virtual Components: Virtual components have been around for a few releases and they get even better in SolidWorks 2010. Virtual components are parts and assemblies that have been created in the context of an assembly, and are saved entirely inside the defining assembly. This makes it extremely easy to rename components directly in the Assembly tree avoiding the need to open, save as copy, and then use Replace Components. Making one instance of a virtual component independent of other instances is a simple Rt.-click menu selection. Also, the folder where you store your assembly doesn't become cluttered with unused part and assembly files resulting from design iterations. At any time you can save the virtual component to an external file with a Rt.-click. SolidWorks 2010 has all of this and more: External components can now be made virtual while inserting them or with a Rt.-click in the Assembly tree; Virtual component names now always include its parent assembly's name (which updates automatically when moving or copying to another assembly); External references in moved or copied virtual components are ignored; A new system option allows you to automatically override the creation of virtual components and save new components to external files.
Sketch Pattern & Sketch Fillet Enhancements: SolidWorks 2010 welcomes new functionality in a number of sketching tools. Now, sketch entities created through Linear or Circular Sketch Patterns are fully parametric as they include the Number of Instances as a displayable, changeable, and configurable parameter. This works great for creating configurations, design tables, and equations where you need to control the quantity of sketch entity copies. Also, the Sketch Fillet tool now has a preview (with virtual intersections) that you can drag to adjust the radius. Or, you can set the radius in the PropertyManager before or after selecting entities. Also new are an entity selection list and the option to apply a dimension to each created fillet. Workflow is better as the fillets are not created until you click OK in the Property Manager.
