Fill out those Custom Properties: Custom Properties are good for so many things. We use them to fill out Bills of Material and drawing title blocks, but there are so many other aspects that are enhanced if these are populated consistently. Here are some examples. Let's say you have a property called "Vendor." You could use the Advanced Select command to help you select all components in your assembly that were purchased from a particular vendor. Now, let's imagine that you have a "Cost" property. You could use Assembly Visualization to find which components in the assembly cost the most. So, since we agree that they're important what are some easy ways to populate them? For starters, you could set up a template that has them pre-filled with characters to indicate the desired format. For example, a "Date" property could have a default value of "DD/MM/YYYY" to help people remember what format to use. The next step up would be to use the Custom Property tab on the Task Pane. Sure, it takes some setting up, but it can really be worthwhile. If you are automating your designs, you can use DriveWorks to populate them. Naturally, Enterprise PDM can read and write to these properties and display them on data cards.
Design for Automation: So, if you plan to automate your designs with DriveWorks or maybe just configurations, there are special considerations to help you plan for success. Some of the simple concepts are to make sure that you don't create parent/child relationships when you create new sketches and features. An easy way to do this is to hide your existing solid body before you start a new sketch or feature. This means that you'll be reliant on planes or layout sketches for reference, which is a good thing for automation. Be careful about using equations or derived sketches. They can add lots of power, but always create a dependency which might get in the way. Instead, consider using Linked Values and put your equations in DriveWorks or in a design table. Lastly, if you might want to swap out parts in an assembly (such as two types of end-caps), model one part, then use File, Save As to create the other and change what is different. This will keep all the internal ids the same for both parts.
Assembly-Level Fillets: In assemblies in 2011, you can create fillets and chamfers, which are useful for weld preparation. As with other assembly features, you can propagate these features to the parts they affect.
Replacing Mates: The Replace Mate Entities tool is enhanced in SolidWorks 2011. To activate the tool, select a mate, a component, or a Mates folder and click Replace Mate Entities. The Missing Entities popup toolbar is now available while you replace any mate entities, not just while you replace a component that includes mate entities. While replacing multiple mate entities, you can postpone the solving of the mates. Select Defer update so that all mates are solved together when you exit the PropertyManager, instead of solving individually each time you select a replacement entity.
Remove a feature from a non-SolidWorks file: Sometimes SolidWorks Feature Recognition fails to recognize certain features in an non-native part file. Don't worry; there are ways to edit your imported parts.
How to link SolidWorks model custom properties into an Enterprise PDM drawing file data card: EPDM file data card variables can be "linked" to file custom properties, yet how do you link a custom property from a SolidWorks model to a SolidWorks drawing data card? You will need to create an additional data card variable block/attribute mapping for the drawing extension (slddrw) in the EPDM variable editor. Use the block name $PRPSHEET (this must be spelled with capital letters) and the attribute name should be the property you want to retrieve from the model, for example "Description." Ensure the existing "Description" block/attribute mapping is still setup for the drawing extension as well as (CustomProperty/Description). Now the description custom property model will be "copied" to the custom properties of the drawing when the drawing is saved into the vault, and will thereby show up in the drawing data card. NOTES: • The EPDM SolidWorks add-in must be enabled • The linked properties will be copied/updated each time the drawing is saved from within SolidWorks.
Flow Freezing can help to reduce calculation time in some thermal Flow studies: As with any analysis, there is a tradeoff between accuracy and computational effort or time. The more cells that you pack into a mesh, the longer the study will take to solve. It is often the case in a Flow analysis that several different processes develop at different rates as the calculation progresses. This is often the case with heat transfer problems with forced convection, where the fluid flow process develops more quickly than the thermal gradient. The calculation as a whole will then march along at the pace of the slowest process, which can often lead to long solution times for complex studies.
Upgrading your release of SolidWorks: Are you one of those users that upgrades once a year to the latest release of Solidworks? During the upgrade, you can update your toolbox to the matching version. If you forget to do this, as most users do, it is very easy to manually update the Toolbox. To do this…
Sketching Tip - Virtual Sharp: Here's a quick little tip that might save you some time. Sometimes in a sketch (or in a Drawing) we need a point entity located at the virtual, or imaginary, intersection of two lines. With no command active simply CTRL-select the two lines and then issue the Point command. This will place a point entity at the virtual intersection. You can now dimension to or constrain geometry to this point so to easily satisfy your design requirements.
SolidWorks Content: Did you know that SolidWorks provides instant access to thousands and thousands of standard models and data. Some of the content available includes: Structural Members for Weldments in various standards (think steel shapes such as square tubing, c-channel, wide flange, etc.), Piping components for Routing in various standards (flanges, fittings, etc.), Robotic components (LEGO, FIRST, etc.), Electronic Components for CircuitWorks (ICs, resistors, coils, transistors, etc.), and symbol libraries for schematics and P&IDs. You can access these components through the Design Library. At the bottom of the "tree" in the top pane of the Design Library you will see a node that says "SolidWorks Content." By selecting this item in the top pane you can access the various folders that contain these types of models/blocks. Then, CTRL+click on the library of your choice to download a zip file containing a huge variety of models and data for that particular category. Unzip the downloaded file and place the extracted folders and files in the appropriate location on your hard drive or network. This information and data can save you hours or even days of internet searching or creating this content from scratch.
A Use for Multiple Split Lines: If you frequently use the SPLIT LINE feature break single faces into sub-regions, for the precise placement of a load or boundary condition you have noticed that the SPLIT LINE command only works on one closed contour at a time. There might be a way to inscribe multiple SPLITs without so many steps. If the face you are splitting is planar, cylindrical, or conical, you can use the command INSERT - FEATURES - WRAP. This command was intended for taking a planar sketch, and wrapping it upon a curved face. It just so happens, it works fine on planar faces, too. And, unlike the SPLIT LINE command, the "Inscribe" option of WRAP will correctly handle multiple closed contours. However, one limitation that WRAP has, that SPLIT LINE does not, is that the WRAP command only expects to act within the confines of a single face. So it is a cool trick that works for multiple contours, but they must lie within a single face, and the face must not have any compound curvature.
Using SolidWorks Property Tab Builder: SolidWorks provides a tool for easily adding custom properties to multiple part and assembly files efficiently called the Property Tab Builder. This tech tip will cover using the SolidWorks Property Tab Builder to add the "Material" custom property to all of the components in our main assembly file. To start SolidWorks Property Tab Builder go to Start > All Programs > SolidWorks 2011 > SolidWorks Tools > Property Tab Builder. To add the custom property, drag a textbox from the left pane into the Groupbox in the center pane. This will add the blank property and the right pane will display the Control Attributes for the custom property you are adding. Make sure that you drag the Textbox into the Groupbox and not outside in the blank space. Now we will use the right pane to update the Control Attributes for the custom property to be added, we are using the SolidWorks property "Material" for this tech tip. Next save the custom property file into your templates folder. The builder should default to the correct location; to verify this you can check the Folder Locations for Custom Property Files from within SolidWorks in the Options dialog. To add your property open the main assembly file in SolidWorks. In the tree select all of the components that you wish to add the custom property to. To load the custom property file into the assembly we will pick the Custom Properties tab in the task pane on the right of the screen. Here you will choose the custom property file we saved earlier from the drop down menu. Once you have chosen the custom property template for SolidWorks to apply it will verify the components that you are adding the property to and allow you to update the value used for the custom property. Save your assembly and all part files and you are finished. The custom property (Material in this instance) has been added to all of the components chosen.
Turn Full Preview On: When working with fillets especially, you should turn on the Full Preview, but turn on Full Preview wherever available. This will allow you to know when the fillets will fail. For example if you are selecting edges and the preview goes away, you know you should deselect that last edge because for whatever reason it will not create the fillets with that edge selected. Basically it is a visual check to tell if the command will work or not, and best of all it is included in the software and requires little or no computing power to render.
Apply Color Weldment Profile Sketches: When you create parts using weldments you might benefit if you change the color of the sketch for different thicknesses. For example if you are working with 1 x 1 square tubing but different thicknesses, how can you tell them apart unless you check the thickness? A quick way to visual know the thickness is to change the profile sketch color and then resaving the file. Once you insert the profile sketch in to the weldment part, make sure you show the profile sketch and presto, you can now see which tubes are what thicknesses.
Arc Length Dimensions: You can use the smart dimension tool to create the arc length dimension. The arc length is from end to end and giving you the total length of that arc. To create an arc length dimension, start your smart dimension tool then select the arc, then both endpoints of the arc. During selection, SolidWorks will switch between three different dimension types.
Multiple Split Lines: I frequently use the SPLIT LINE feature to inscribe faces into sub-regions, for the precise placement of a load or boundary condition. But if I want to apply several such boundary conditions, the SPLIT LINE command only works on one closed contour at a time. Is there any way to inscribe multiple SPLITs without so many steps? You can split a planar, cylindrical, or conical face with the command INSERT - FEATURES - WRAP. This command was intended for taking a planar sketch, and wrapping it upon a curved face. It just so happens, it works fine on planar faces, too. And, unlike the SPLIT LINE command, the "Inscribe" option of WRAP will correctly handle multiple closed contours. However, one limitation that WRAP has, that SPLIT LINE does not, is that the WRAP command only expects to act within the confines of a single face. So it is a cool trick that works for multiple contours, but they must lie within a single face, and the face must not have any compound curvature.
Upgrading to SolidWorks 2012: Are you ready to upgrade to SolidWorks 2012? If you have a network license, please upgrade your SolidNetWork License Manager first! After the upgrade, launch the SNL Manager on your license server and choose to activate. This step is critical, as it registers the 2012 product so that 2012 licenses can be distributed to your clients. This will not be a problem for clients still running older versions of the software; the 2012 SolidNetWork License Manager will continue to support them.
Preparing for a Future Upgrade: If you are simply planning to upgrade in the future, please consider the following if they apply…
