In the land of SolidWorks Assemblies exists a funny creature called the “Virtual Component”. Virtual components are typically used in top-down design when you need to create a new part in the context of an existing assembly. During the conceptual design process, when you frequently experiment with and make changes to the assembly structure and components, using virtual components has several advantages over the bottom-up design method as explained by the SolidWorks help system online:
You can rename these virtual components in the FeatureManager design tree, avoiding the need to open, save as a copy, and use the Replace Components command.
You can make one instance of a virtual component independent of other instances in a single step.
The folder where you store the assembly is not cluttered with unused part and assembly files resulting from iterations of component designs.
Some of the thinks that you have to watch out for are the inability to create a drawing of the virtual component. To make a drawing of a virtual component, you must save it as an external file. To save it as external you simply right mouse click on the file and save as External Part and it will ask for a file name and folder location. Simple as that.
Now to really throw a wrench in the works, how do PDM systems track these virtual items? Workgroup PDM will certainly let you add an assembly with a Virtual Part, but it has no means for really tracking it beyond the where used report. There is a setting to turn this on in the User Options, but selecting this option has significant performance impact. and since a virtual part is ususally only used relative to one design, this setting may have a low return on investment.
Enterprise PDM actually handles these quite nicely and if a virtual component is being used, it is shown in the check in dialog box in reports as well as the BOM tab, which is really where you want it displayed. Below is a quick video demonstrating the differences between Workgroup PDM and Enterprise PDM concerning virtual parts.
What’s the fastest way to show mates between two components in SolidWorks? This was a question posed to the tech team here at CAPINC at our internal Beat the Geek challenge last week. Let’s uncover some of the possible solutions:
One method is to use the Show Mates function that is part of context menu in assemblies when selecting a part. A very nice tool as it allows the use to see only the part (or parts) selected and the mates attached to that part. The View Mates window will appear and display a list of mates for the selected component(s). A nice feature is that it displays an icon that indicates mates that are in the path to ground. These mates hold the part in position relative to the origin of the assembly. They are shown first on the list, with a horizontal bar separating them from other mates. Mates can also be edited from this head’s up user interface. To view the mates for more than one component, simply hold the CTRL key down, and click the components, and invoke the context “view Mates” item by either left-clicking or right clicking.
Another way is to view the mates in the “Mates” folder for each component. This was added several years ago and is quite handy. Simply drill into a part the FeatureManager Design tree in the assembly, and one of the first folders under the part level is the “Mates in XXXX”. Here you will see all the mates belonging to that part. Note this only appears at the assembly level when viewing a part and not in the Part interface. A similar method for viewing mates is to change your tree display to “View Mates and Dependencies” Right Click at the top of the FeatureManager Design tree and choose Tree Display -> “View Mates and Dependencies”. Not the tree show mates under the parts instead of features, and the features can be accessed in a folder below the mates, eseentially reversing the default look and feel of SolidWorks. To reverse this behavior, go back to the Tree Display options and set it back to “View Features”
While there are a number of ways of showing the mates that belong to one component the winner is: Drumroll please… CTRL click two components and show the Property Manager. All mates for both components are listed, with the common mates in boldface at the top of the list. This just noses out the competitors inside of SolidWorks for the fastest method.
You can decide on what your favorite method is here:
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If you have a better way, please send us a comment!
Here is a video on the various methods hosted in our CAPUniverity YouTube site.
Which key do you hold down to “shift” drawing views around on the sheet without having to click exactly on the bounding box of the view or on the edge of a part or assembly in that view? Once, again the “ALT” key comes to the rescue. Simply hold the “ALT” key down then left mouse drag the view. This is not just a one trick dog, you can use the “ALT” key to move BOM tables and other tables the same way. Gone are the days of hunting around for the corner icon to move the table. Here is a short demonstration…
SolidWorks has an array of tools for furniture and cabinet design. With SolidWorks “Weldments”, stock wood sizes for creating frame based geometry can be accomplished quickly, with accurate cut lists. Part Library Features for wood joining methods and Smart components for assembling systems with mechanical fasteners make assembling and specifiying a complete job easy. I would like to share with you several example models and libraries that go along with a webcast that I ran recently. To watch, go to https://www1.gotomeeting.com/register/407230368 and you can the full story on furniture and cabinet design with SolidWorks. Here are the example files that I will be demonstrating during the webcast, uploaded to CAPINC’s 3DContentCentral Site. By the way, you can embed and post models to 3DContentCentral too. I will update this post after the webcast with videos of key aspects of woodworking design with SolidWorks.
By the way, you can embed and post models to 3DContentCentral too. I will update this post after the webcast with videos of key aspects of woodworking design with SolidWorks.
There are a number of ways not to use AutoCAD to create schematic diagrams out there. I prefer to use SolidWorks related tools to get my job done. I can take advantage of BOM’s, Libraries of symbols, parametric dimensioning and collaborate tools like eDrawings and Enterprise PDM. Let’s discuss how to create a simple schematic in SolidWorks Drawings mode.
There is a recipe to concoct that will make for successful schematic diagrams in SolidWorks. The first ingredients are the symbol libraries. SolidWorks provides users with hundreds of symbols that can be found here in the SolidWorks Content tab. Simply go to the Design Library Tab on the right side of the screen and choose the SolidWorks Content node. Then expose the Blocks node. Here you will find Hydraulic and Electrical appear in the lower window. Hold the CTRL key and Left Click on the appropriate icon to download the library. Once it is done downloading, the best option is to store it in a central location, like a server or the Enterprise PDM Vault.
Next, you want to add this file location to your Design Library references. To do this, go to “Add File Location” button on the Design Library tab. Then point it to where you downloaded the files. It is a good idea from this point to save our settings as a SolidWorks registry file using the “Copy Options Wizard” so these file locations can be easily deployed to other SolidWorks users at your company.
I like to add the line format, layer and, weird but true, the explode line sketch toolbar to my SolidWorks drawing environment. The explode line sketch toolbar includes the Jog Line tool which is handy to do exactly what it states.
The advantages to using SolidWorks drawing environment here are that you can marry 3D Views of the piping system and 3D Schematic view, export eDrawings, PDF’s and other such formats SolidWorks can export, plus Enterprise PDM can automate the filling out of title blocks and the creation of said export formats thought an Approval workflow.
Another way to create the schematic is to actually drag the blocks into Layout mode in an Assembly. The advantages to building it here are the Bill of Materials function can be called. To execute this, you must convert the blocks to parts for the BOM to pick up on these; however, this is an easy step. After you have added all your 2DBlocks, right-click on the blocks in the FeatureManager Design Tree and choose “Make Part from Block” and choose the either the “On Block” setting or the “Project” setting. The “On Block” setting is usually fine as this will constrains the part to be co-planar with the plane of the block in the layout sketch, which is fine for a schematic diagram.
Once you have the blocks all laid out, you will have the opportunity to create a Bill of Materials in Assembly or Drawing mode. If you want to Balloon the block symbols to match the items on the BOM, you can use the Balloon Invisible components setting on the Balloon properties. They are invisible by default as there is no geometry. But if you select the balloon button and choose the part you want to balloon in the invisible components list, and then select he part to balloon in the display, you get the patching properties to balloon on that part.
Do you sometimes feel as though you are living in an alternate reality? Well, if you know me, that doesn’t seem so strange. Using the “ALT” key in SolidWorks can bring you great joy and help you achieve SolidWorks bliss.
The first cool use of the ALT key is in the realm of large scale design. If you have an assembly open, and it’s quite large, SolidWorks will try to reduce your graphics overhead by “decimating” the graphics. It will turn you really nice detailed models into chunky, block looking objects. This is usually for the greater good, but if you need to run an animation, fly through or need to see all the details of your SolidWorks model, this may be a hindrance. To remedy this, invoke the view command of your choice, like the Rotate option and then hold the left ALT key down (yes, it has to be the LEFT ALT key). With the left ALT key still held down, rotate and notice the full graphics are available! Check out the video below…
The other ALT key is set to make use of smart mating in assemblies. If you have the parts you already want to mate in the assembly, hold down the RIGHT ALT key (yes, the right ALT key) and drag the face you want to mate on top of another face you want to mate. All the rules of smart mating here apply, where are in the SolidWorks help system online, which you can click here to get to. Here is a video on smart mating using the Right ALT key!
What defines a smart company? Knowing when to adapt and change with the needs of the customers they serve. You all may have heard of the new 2D Product DraftSight, which came out recently. There is quite a buzz about the product. But you may ask yourself, why have they come out with DraftSight? The SolidWorks 2D Editor still exists and and just underwent a name change. But as you may know SolidWorks has never been shy about changing to the best technology available. In fact this has happened many times over the years at SolidWorks and Dassault Systemes. I would like to cite several of these examples for you.
The rendering tool in SolidWorks, PhotoWorks, has had two different rendering engines over the years, one from Lightworks Design LTD, and one currently being employed Mental Ray from a company called Mental Images. Even more recently, SolidWorks has announced that PhotoWorks has been retired and PhotoView 360 is the new rendering platform of choice. PhotoView 360 is a CPU based rendering tool, while PhotoWorks is a GPU based tool. In fact, there is lot’s of great info and downloadable materials for PhotoView 360 at the website of the company that developed the PhotoView 360 technology, Luxology, which you can check out here.
In the simulation realm, COSMOSFlow was replaced by NIKA’s FloWorks product, alter renamed to what is currently in use, SolidWorks Flow Simulation. With this technology, you can simulate liquid and gas flow in real world conditions, run “what if” scenarios, and quickly analyze the effects of fluid flow, heat transfer, and related forces on immersed or surrounding components. This was a big deal, as the old COSMOSFlow was developed by Blue Ridge Numerics and being distributed by SRAC (Structural Research and Analysis Corporation) and Nika was a competitive tool. But SolidWorks and Dassault Systemes found that by swapping these solvers the user had a better experience and the technology was better for the application. COSMOSFlow was based on the Finite Element technique and FloWorks was and still is based on the Finite Volume method. To learn more about SolidWorks Flow Simulation, take a look at this video.
An now DraftSight, which is a new 2D drafting tool for modifying and creating new 2D documentation. This is superior to the SolidWorks 2D Editor, formerly DWGEditor. First thing I noticed is that it was only a 41 mb download! That is smaller than most viewers nowadays. Then I noticed the interface, which is modern and even makes use of mouse gestures like they introduced in SolidWorks 2010. After ogling the cool interface, I opened several drawings from my customers that usually opened slowly in SolidWorks 2D Editor and noticed they opened almost instantaneously. The product is free as well! For a tech support plan, API or LISP programming and personal tech support services, there will be a fee, but the fee is much less than upgrading AutoCAD for every release they come out with. Please go ahead and download the product and join the SWYM community here. On the SWYM community page there are tons of instructional videos and helpful tips. SWYM actually stands for “See what you mean”. Now don’t think that there are scores of engineers at Dassault Systemes or SolidWorks writing a new 2D drafting package. They partnered with Graebert GmbH and have based the product on ARES, which is working alternate solutions for the 2D CAD users community. I have been evaluating their tools recently and have started using the Linux distribution of ARES, which is nearly equivalent interface-wise to the Free DraftSight product for Windows. Check out the video below…
What does this all mean? SolidWorks and Dassault Systemes have great scouting. Like a baseball team who sends out scouts to watch the other games happening around the league, trying to find the next big thing or looking to see what our competitors are doing well, SolidWorks and Dassault want to be champions. There is a lot of meaning to the name of the company Dassault Systemes. DASSAULT actually means “For Assault” or “For Attack” in French. Dassault Systemes was a spin off of Dassault Aviation which was originally founded by Marcel Bloch, an aviation pioneer. Bloch later changed his name to Dassault, an alias his brother had used in the French Resistance. Thanks for bearing with me on this stroll down memory lane…
Have you ever wanted to make sure an inspection balloon could be tethered to another annotation item, like a dimension? Here is how to accomplish this is a few short steps. First, dimension your drawing in the normal way. Then add your balloons, notes, symbols, ect… by double clicking the view that you want to associate them with first. This activated the view and makes any item you draw or add notes note stick to that view for good. Then you can add balloons, notes ect… After you add the info you need, CTRL-select the balloon and the dimension and Right Mouse click to get your context sensitive menu. Here you will choose the Group flyout command and choose the Group command. If you want to move the balloon after it has been grouped, hold the ALT key down and drag the balloon. This will keep the grouped relationship in tact.
Check out the video below showing how to create a fully ballooned drawing ready for inspection with the balloons grouping process. For more info on fully ballooned drawings, watch this webcast.
Alright, so you have selected a bunch of faces for applying a load. Now you want to pick those same faces to apply a mesh control to them to make sure that you have accurate results. As you may already now a smaller element size in a region improves the accuracy of results in that region. It’s just a pain to re-select all those faces, right? Not really. I found this trick recently to help re-use that selection set.
For this example in the video below, select the faces that you want to restrain or add loads to in the normal way. It sometimes helps to select in wireframe mode and use a SolidWorks selection filter to grab all the faces of the model quickly. Use the “X” key to select “faces” quickly. Then apply the load or restraint as usual. Once that occurs and you set up the rest of the model, the selection set is then available for re-use. For example, to add a mesh control to reduce the element size on the selections for loads and restrains, simply pre-select the aforementioned load or restraint, rich click on the mesh icon in the Simulation Study Manager and choose Mesh Control. You will then notice that the faces are all selected as you would have hoped. I have not tried this in SolidWorks 2009, but it definitely works in SolidWorks 2010. This also has worked for quite some time in SolidWorks Flow Simulation.
I recently had a question from a customer asking if there was a way to convert a regular old named or projected view to a complete section view. Let’s say you fully detail a view up with many dimensions, notes, symbols, etc… and then you want to convert it to a section view to revel more details. My first answer was no, we cannot perform such an action. However, after having my morning coffee the next day, I had a revelation; why not use the “Broken Out Section View” option?
The broken out section view is typically used to review the inner workings of a part or assembly view in a small portion of the view, rather than making a separate section view. When the user creates a broken out section, SolidWorks promptly places you into the spline tool where you can draw a boundary for the sectioned out area. Then you can manually enter a value for the depth or choose an edge in a projected view to determine the depth. But rather than drawing a small spline area for the broken out area, you can draw the spline all the way around the view, or even draw a rectangle before entering the broken out section command and then it will use that for the boundary.
The dimensions in the view that still make sense at the section depth still appear. in other words, dimensions to features which no longer appear in the view are removed automatically. I hope this post get’s you out of a jam!
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