Like Flat Stanley or the Travelocity “roaming gnome” who has been spotted in Hawaii, on the slopes of Banff-Lake Louise, and checking out the view of Times Square, the SolidWorks World backpacks have also made their way around the world. Recently we learned about one of the more interesting places the backpacks have appeared.

Bruce Crawford, editor of Castings SA and Metalworking News, has attended SolidWorks World for the last four years, and faithfully brings home his bag every year. Rather than replacing last year’s model with the new one, Bruce has a greater plan for his SolidWorks World bags – his annual trip to Kruger National Park in South Africa with his family and friends!

Kruger National Park is a famous park in South Africa that boasts the “most diverse game viewing experience in Africa.” Each year, Bruce and his crew travel through the park on a three night, two day excursion, with a tracker and ranger leading to way. The SolidWorks World bags are used as day packs to carry water and snacks as the group travels 5-6 hours per day by foot to see the animals in their natural habitat.

When we spoke to Bruce, he told us about one of the more interesting sights on their journey, "We were about a kilometre away from the end of the first morning's walk and came across this 4 metre African python that was in the process of devouring a buck. We must have missed the action by about an hour. Not many people are in the right spot at the right time, especially on foot."

Like Flat Stanley the roaming gnome, the SolidWorks World bags have been to the far ends of the earth. Has your SolidWorks World bag been on a family trip to Italy and walked over the Ponte Vecchio? Or seen the depths of the Grand Canyon?

We’d love to hear where your bag has gone, so please leave a comment below and share your amazing journey! Or send pictures to pr@solidworks.com and we'll aggregate them in a future post.

The property manager that we are able to create for our files is very similar to the Property Manager users are used to seeing when inserting Toolbox Fasteners.

There are two different ways to create a Configuration Publisher with in SolidWorks and which one you use depends on the file you have and what you are trying to accomplish with that file. The first is what I would call an “open ended” file in that there an unlimited number of configurations that you can create. The second is what I would call a “closed set” file in that there is a very specific set of variables and possible configurations. There are pros and cons to each of these methods and you will need to decide
what is going to work best for your particular case.

So to create the Configuration Publisher for a file that has an “open ended” set of configurations you need to create a Single Line Design Table. In this design table you will want to include all of the parameters that might have the ability to change, including all custom properties.

One tip I like to point out is using the powers of Excel for items like concatenations to automatically create your Custom Properties for description and part number.

Once your Design Table is created you will need to go to the Configuration tab and Right Click on the Part Name and choose Configuration Publisher. In the Configuration Publisher dialog box, you build the custom PropertyManager in the center pane. You drag controls (list boxes, number boxes, and check boxes) from the palette on the left to the center, and set attributes for those controls in the pane on the right. You can see from the set of screen shots below we created controls for the different items we defined in our design table, there are several different options you can set for each control such as weather the control is dependent upon other properties, or you want it to perform with in a specific range. You can see what the completed Property Manager looks like below. (I have included the files used in the screen shots at the bottom of this article for everyone to review and use as an example.)

To create the Configuration Publisher for a file that has a “closed set” of configurations is a little simpler in that we need to create a Full Design Table that includes all of our possible configurations. You also need to make sure that you have a row for each configuration, a column for each variable and
a value for each variable.

Once your Design Table is created you will need to go to the Configuration tab and Right Click on the Part Name and choose Configuration Publisher. The Configuration Publisher dialog box appears and the design table opens in a separate window. Because the design table has multiple rows and contains values for each variable and for each configuration, a control appears in the palette for each variable in the design table. All you need to do now is drag each variable you want displayed to the center pane and in the right hand edit are enter the Name and set the options for each item. You can see what the completed Property Manager looks like below. (I have included the files used in the screen shots at the bottom of this article for everyone to review and use as an example.)

If you would like some additional information on Configurations and Design Tables, please take a look at a presentation I did with a former CATI colleague Joe Rowesy at SolidWorks World this year.Download DesignTables The Complete Story-SWW2012

Example Files Download Config_Publisher-Single-Multi

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Josh Altergott is Support Manager at Computer Aided Technology, a SolidWorks Value Added Reseller with locations in Kentucky, Missouri, Kansas, Wisconsin and Illinois. He is a regular contributor to the CATI Tech Notes blog.

SolidWorks offers you an alternative behavior. A toggle setting is available under Tools>Options…>System Options>View. Unselect the Zoom to fit when changing to standard views option. While this setting is unchecked, swtiching between Standard Views will no longer force the model to zoom to fit.

Let’s consider a material from the Simulation material database. Alloy Steel has the following properties (numbers rounded):
Young’s Modulus – 30 x 10^6 psi; Poisson’s Ratio – 0.28; Mass Density – 0.278 lb / in^3; Yield Strength – 90 ksi

What will happen to the Finite Element solution if one material property varies? I’m going to start with a simple model in tension and apply Alloy Steel as the material using the default property values. Then I will change Poisson’s Ratio and re-run the study several times in order to compare the displacement and stress results. Recall that Poisson’s Ratio is a measure of the lateral strain to longitudinal strain for a material, or E_lat / E_long (pretend the E’s are Greek epsilon’s). Poisson’s Ratio is relevant to the linear elastic portion of the stress-strain curve and is unitless. One thing to note, if you do not define Poisson’s Ratio for a material, Simulation will assume that Poisson’s Ratio is equal to zero. There is a pop-up warning, too, just in case you forget to enter a value. Note that if you do not have Poisson’s Ratio for a material, 0.3 is a good initial estimate. But definitely exercise all of your options to find out the correct value for your design materials.

For a ½” square bar, 4” long, I have fixed one end and applied a 10ksi force at the opposite end, putting the bar in tension. After running the analysis with default material properties, I set a baseline with Trend Tracker. After creating several custom Alloy Steel materials, varying Poisson’s Ratio from 0.0 to 0.5, I re-run the analysis with each custom material. Trend Tracker will record the details for maximum displacement and stress in the model.

As you can see from the chart, the Von Mises Stress results vary approximately 16 ksi and the displacement results vary 0.00006 inches. As percentages, this is a 28% variation in stress and a 1.2% variation in displacement. I don’t think most of us would be concerned with 1.2% variation in our models, but 28% is an entirely different matter! I did, however, choose the model with this purpose in mind. The high stresses are at the fixed end at the sharp corner – something most Engineers would avoid in their designs. Now that a 28% variation has your attention, let’s look at a more practical model.

This is a simple bracket, a modification of a part in the SolidWorks Essentials manual. I’ve applied a fixed boundary condition to the bolt holes in the base and a normal force to the counter bore face. I’ve repeated the rest of the analysis, just like the square tensile bar, including using Trend Tracker and varying Poisson’s ration from 0 to 0.5.

For this “practical” model, the Von Mises Stress results vary approximately 4,300 psi and the displacement results vary 0.0006 inches. The percent variation in this model is 5.8% for stress and 6.6% for displacement. If you’re designing for a large Factor of Safety, less than 6% variation in your stress results is not significant. Using SolidWorks Simulation, however, most of us are designing for the lowest acceptable Factor of Safety in order to save the maximum amount of money possible on material costs. In this scenario, a 6% variation can be significant!

So the next time you’re analyzing that awesome design, consider reviewing the sensitivity of your analysis by varying a material property or two. Now you’re armed with powerful information you can share in your next design review. Material property variations from your vendors are no longer an issue! Now go make your products better with SolidWorks Simulation!

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Bill Reuss is a CAE Specialist at 3DVision Technologies, a SolidWorks Value Added Reseller with locations across Ohio, Indiana, and Kentucky.  He is a regular contributor to 3DVision Technologies' Blog where you will find new ideas to improve your productivity with SolidWorks Simulation.

At the time this article is written, SolidWorks 2012 has several capabilities of both Hide and Suppress, and even a way to essentially capture the benefits from both.

Hiding Parts in Assemblies

Think of hidden components in a SolidWorks assembly as just that... NOT VISIBLE.

From there, they are essentially exactly like a visible part.

Hidden parts still participate or are included in:

• Collision Detection
• Mass Properties calculation
• Dynamic Assembly Motion
• BOM’s
• Pack n Go
• Etc.

In most situations, there are options to “Include” or “Ignore Hidden” in the event that you do not want to control whether they are included in the calculation.

Hidden parts also take the stress off the video card since it does not have to display them.

However, hidden parts are still loaded into memory, therefore their math data takes up part of the memory footprint.

Suppressing Parts in Assemblies

Think of a suppressed part as a ‘deleted part that is very easy to UNDO’.

When a part is suppressed, all dependencies associated with that part is also suppressed such as Mates, Assembly Features, and other referenced items.

The part is treated as if it doesn’t exist.

If the suppressed part is UNSUPPRESSED, it will again solve like all other parts.

The Best of Both Worlds

There is a little known menu selection that can give you the performance of having parts SUPPRESSED, when they are really only HIDDEN.

When you HIDE components, follow that by right-clicking the ASSEMLBY NAME at the top of the Feature Manager and selecting “Unload Hidden Components.”

This will ‘flush’ the math footprint of the parts and give you better performance when you don’t want to see parts, but don’t want to suppress them either.

This is great for toolbox parts where you need them for an accurate part count on the BOM, but don’t want the added strain on your video hardware.

This menu item needs to be selected again if more parts are hidden. It is more of a runtime function than a persistent setting.

The easiest way to SHOW Hidden Components

You can easily spot Hidden Parts and Assemblies in the top level of your Feature Manager, but when those Parts and Assemblies are subcomponents of other Assemblies, it becomes much more difficult.

The ‘magic button’ for this situation is on your Assembly Tab called "Show Hidden Components."

This will take all SHOWN components and ‘temporarily’ HIDE them, while taking ANY and ALL HIDDEN components and SHOWING them, regardless of their depth in the Feature Manager.

Select the parts on the screen that you would like to now SHOW and they will ‘temporarily’ HIDE them where they will join the other SHOWN components.

Select components on screen by:

• CLICK
• Window Select (Crossing or IN)
• Ctrl-A (Select All)

Once you are done, select "Exit Show-Hidden."

Now all the SHOWN components will reappear from their ‘temporary’ hidden state.

NOTE: Suppressed Parts and Assemblies will NOT be included in the SHOW HIDDEN COMPONENTS function.

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Darin Grosser is a SolidWorks Elite Application Engineer, Certified SolidWorks Expert and a senior member of the technical staff at DASI Solutions, a SolidWorks Value Added Reseller with locations throughout Michigan and Indiana. He is a regular contributor to the DASI Solutions Blog.

(Exporting 2D DXF files) We design in a 3D world, but many parts are manufactured from flat sheet. The flat pattern of a sheet metal part and flat plates used in weldments are examples. Laser and waterjet cutters of flat parts may want to use a DXF file instead of native geometry. Let’s look at several ways to create DXF files.

Option 1 File > Save As > DXF is the most general method. The dialog at the right requires several inputs from the user: Be sure to select a view that is normal to the flat part and deselect the others. The output alignment tools specify the X and Y axes and whether the part is flipped on an axis.
Option 2 For an inherently flat part or an unfolded sheet metal part, right click on the face and select Export to DXF/DWG from the context menu. In this case, there’s no dialog to select a view because the face determines the view. This workflow is a little faster.
Option 3 You can also right click the Flat Pattern feature in the Feature Manager to see a different dialog. For cutting only, just select Geometry as the entities to export and set Output Alignment as desired.

There’s yet another way to do this. One of our customers wanted to make a SolidWorks drawing as an intermediate step, but the title block, dimensions and annotations were exported to the DXF and interpreted by the laser cutter as actual geometry.

There’s a solution: Create a second sheet and edit Sheet Properties so no format is displayed. Set the sheet scale to 1:1. Return to Sheet 1, select the Flat Pattern view and Control-C to copy it. There may be a warning that not all items in the view can be copied, but ignore it. Change to Sheet 2, left click anywhere on the sheet and Control-V to paste a copy of the flat pattern view. Now delete any dimensions and annotations. Right click the bend lines and Hide. There will be a message that bend notes will be hidden as well. Click Yes to continue. The desired result is Sheet2 that contains nothing but the outline geometry of the flat pattern, with no notes, annotations, title block etc.

Finally File > Save As > DXF, click the Options button and select “Export active sheet only” > OK > Save

The drawing now serves two purposes: Sheet1 is fully dimensioned and annotated as a design document, while Sheet2 is never printed but used only for DXF export.

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Art Woodbury is an Applications Engineer  at CAPINC, a SolidWorks Value Added Reseller with locations across New England. He is a regular contributor to their CAPINC University blog.