NASA Leverages Stratasys 3D Printing for Space Vehicles

An agile white vehicle roams the Arizona desert, maneuvering the unforgiving terrain as the wind and sun beat down and temperatures swing from one extreme to another. NASA astronauts and engineers are test-driving a rover over rocks and sand, up and down hills in an environment that simulates the brutal conditions of Mars.

The rover is integral to NASA’s mission to extend human reach farther into space. Its cabin can accommodate a pair of astronauts for days as they study extraterrestrial surfaces. Its twelve rugged wheels on six axles grapple over irregular, unsure terrain.

To design such a specialized vehicle, NASA engineers drew on ingenuity and advanced technology. For example, about 70 of the parts that make up the rover were built digitally, directly from computer designs, in the heated chamber of a production-grade Stratasys 3D Printer. The process, called Fused Deposition Modeling (FDM) Technology or additive manufacturing, creates complex shapes durable enough for Martian terrain. 

Jim TeDesco
Marketing Manager
Computer Aided Technoloy, Inc.

SolidWorks Weldments from Profiles to Cut Lists - Part2

Welcome to the second part of the SolidWorks Weldments blog series! In this section we will look at creating:

• Sketches for Weldments


• Weldment Structural Members


• Options for End Conditions

Where to start?

Either closed or open 2D Sketches can be used, it doesn't matter. SolidWorks Weldments uses closed profile sketches to sweep along the sketch segments.

We will join a 3D Sketch to this skeleton. (3D Sketches are located on the Sketch drop down menu)

Now we will create a Structural Member based on these sketches. To access the Weldments tool bar right click the dark grey tabs below the Command Manager ribbon.

Once the Weldments tab is accessible you should be able to select the Structural Member button. A closer look at the Weldments toolbar:

You can select any size you want from the Standard menu. In this case I used a Square Tube. Click inside the Groups box to start your sketch selections.
The Groups box allows you to pick up sketch segments that belong to the same section of the Weldment. Here we are just picking the lines from the 2D sketch.

There are many Settings to sort through. Here is a closer look.

Apply Corner Treatment allows us to specify a corner option for the whole Weldment.
These settings can be applied individually at each corner by right clicking the pink dot
as seen in the above image.

Merging allows you to make the selected segments all one body. This can affect your cut list, especially when your Structural Member is made up of several arc segments.

The G1 and G2 allow for weld gaps to be created between the Weldment sections.

Mirror does just what is says. You wouldn't notice much of a difference in this example as
the profile is that of a square tube.

Alignment, this allows us to change which axis of the sketch to align to an entity in the sketch.

Rotation angle of the profile can be set here.

Locate Profile, this button allows us to move to a different vertex or point inside of the profile
sketch. We will see this in the next few images.

This is an image of the default profile location.

After clicking the Locate Profile button we can choose any vertex or point in the sketch and the profile will move.
Now that we have the profile positioned, use the green check mark to accept the Structural Member.

Start a new Structural Member and pick the line segments of the 3D sketch. Use these settings for the End Condition and Gap.

Let's focus in on this corner to see the settings we have applied. Currently the profile is shifted, we will need to use the Locate Profile button
again to align the profile to the existing Weldment.

Here is what the alignment should be.

After confirming the Structural Member command you will notice that the tubes intersect. They will need to be trimmed.
This will be covered in the next section of the Weldment blog series article.

Please check back to the CATI Blog as the Dedicated Support Team will continue posting our series of articles that goes further into the details of SolidWorks Weldments. All of these articles will be stored in the category of Daily Dose.....of SolidWorks Support and links to each article with their release date are listed below:

• SolidWorks Weldments from Profiles to Cut Lists - Part1 (Bryan Pawlak 2/26/14)


• SolidWorks Weldments from Profiles to Cut Lists - Part2 (John Van Engen 2/27/14)


• SolidWorks Weldments from Profiles to Cut Lists - Part3 (Blake Cokinis 3/3/14)


• SolidWorks Weldments from Profiles to Cut Lists - Part4 (Neil Bucalo 3/4/14)

Thank you for reading!!
John Van Engen
CATI Senior Technical Analyst
CSWST CSWE

SolidWorks Weldments from Profiles to Cut Lists - Part1

This month we are going to take a deep dive into SolidWorks Weldments. We are going to discuss the profiles, feature manager options, modification tools such as Trim/Extend, and drawings including views, Cut Lists, and Custom Properties.

Let's start by defining a Weldment, a Weldment can be defined as a unit formed by welding an assembly of parts together.

Inside of SolidWorks we handle this in a multibody part file. This way we manage one single file instead of tens or hundreds of part files in an assembly. So by default you will see that the Merge Bodies checkbox is automatically turned off when a Weldment is created.

The first thing that you need to do is access the Weldment commands. Like all functions in SolidWorks this can be done is many ways: You can turn on the Weldments toolbar by going to View, Toolbars, Weldments; You can right click on the Command Manager tabs and select Weldments; or you can go to Insert, Weldments when inside a part file.

 

When you create the first Structural Member in apart, a Weldment feature is created and added to the FeatureManager design tree. The software also creates two default configurations in the ConfigurationManager: a parent configuration Default[As Machined] and a derived configuration Default[As Welded].

 

In SolidWorks 2014 we now have 2 different ways to manager our library of Weldment profiles. We have the traditional method of creating a single sketch for each profile size, or the new method of using a Design Table to control configurations of various sizes in a single part file.

SolidWorks provides us with a small sample of profiles in our standard installation. Since everyone does not use Weldments we do not install the large databases by default, but SolidWorks does make theses available for download in your Design Library.

Here are the default profiles that are available to you out of the box.

 

Additional profile libraries can be downloaded from the Design Library, under SolidWorks Content, Weldments. To begin the download, hold down your control key and click on the standard you want to download.

A dialog box will appear prompting you to select a location to save the zip file.

 

 

 

 

 

 

Here is a list of all the additional profiles that can be downloaded.

 

Creating Custom Weldment Profiles

To create a custom Weldment profile:

1. Open a new part file


2. Start a sketch, and draw your profile. The origin becomes the default insertion point and you can select any vertex or sketch point as an alternate pierce point.


3. Close the sketch


4. Select your sketch in the FeatureManager and go to File, Save As


5. Choose the location you want to use to save the file.


6. Set the Save As file type to Lib Feat Part (*.sldlfp)


7. Click Save.

 

 

Setting the Weldment profile folder location.

To set the Weldment profiles location.

1. 
   
   Open the SolidWorks System Options (Tools, Options)
   
   


2. 
   
   Select File Locations in the left column
   
   


3. Select Weldment profiles from the pull down menu


4. Click Add to browse to your folder location.

The default file location is:

C:\Program Files\SolidWorks Corp\SolidWorks\lang\english\weldment profiles.

 

 

 

 

Files can be stored in any location. I suggest that you create a folder called Weldment Profiles. When you map to your folder location in the system options, point to this folder. When you extract your downloaded zip file, you should end up with the standards folders inside of this folder.

Inside of the standards folder should be the Profile Types folder.

Inside of all the Types folders you should have the individual library feature files.

 

Configurable Weldment Profiles:

New in 2014 you can now add different configurations of a structural member and save them in a single library feature. For example, instead of having 50 separate library features for square tube sizes you can have one library feature with 50 configurations controlled by a design table. This allows us to manage and change these profiles much easier than before.

 

We hope this has given you an insight to how to access the Weldment tools. Please check back for part 2 of this series as we discuss how to apply these profiles to your parts.

Please check back to the CATI Blog as the Dedicated Support Team will continue posting our series of articles that goes further into the details of SolidWorks Weldments. All of these articles will be stored in the category of Daily Dose.....of SolidWorks Supportand links to each article with their release date are listed below:

• SolidWorks Weldments from Profiles to Cut Lists - Part1 (Bryan Pawlak 2/26/14)


• SolidWorks Weldments from Profiles to Cut Lists - Part2 (John Van Engen 2/27/14)


• SolidWorks Weldments from Profiles to Cut Lists - Part3 (Blake Cokinis 3/3/14)


• SolidWorks Weldments from Profiles to Cut Lists - Part4 (Neil Bucalo 3/4/14)

CATI

WHERE DID IT GO?!?!?!?!

“I was working on an assembly in SolidWorks and when I tried to rotate the part/zoom to fit, the entire assembly disappeared!”

This is one of the more common problems that I have encountered while working support.  There are many reasons this can happen; mates or the lack thereof, nothing is fixed, everything is floating or perhaps just a bug in the system.  Regardless to the reason this happens, there are easy ways to fix it.  In this case, the assembly was originally as shown below,

Later on when opening the assembly it can be apparent that something is wrong.  In this case, the assembly now looks like this,

If I’m paying attention, I’ll see that the cue ball is missing.  Unfortunately, the missing part/parts are sometimes internal and not so easily missed.  When trying to rotate this assembly, everything disappears completely.  The same happens when zoom to fit is attempted.  There is one very easy way to locate the missing parts.  By right clicking on any part except the first which is fixed at the origin, the option “Move with Triad” should be selected.  If this is not shown, click the double arrows at the bottom and choose “Customize Menu” at the bottom.  This will allow you to place a checkmark next to “Move with Triad” so that it will always be there when right clicking on parts.

Using this command, each part in the assembly can be located as shown below.  The Triad will always stay the same size no matter how much zoomed in or out you are.  The first picture shows where all of the remaining parts are located, while the second picture shows where the missing part is.

It is important to check every part as there might be more than one missing, likewise the missing parts might not be in the same location.  For curiositys sake the distance from the origin can be measured.

In this case, this ball is now over 12 kilometers from the origin.  To move it back, the Move with triad can be used, mates can be used, or simply deleting that part and then reinserting it.  Each method works differently but can all be used to fix this problem.

 

Chad Whitbeck, CSWP

Applications Engineer, CATI

What is "Dissolve Sketch Text?"

 

 

 

 

 

 

 

 

When adding text to a part, SolidWorks has made the task simple.Text is added by using the ‘Annotation’ feature in the Sketch Command Manager. Text can be used with Extrude Boss/Base or Extruded Cut.

 

 

 

 

 

 

 

 

For this example, a guide curve was used to position the text.

 

 

 

 

 

 

 

 

 

 

 

Notice the test is all one Annotation entity. For some applications, text is best utilized when it’s a series of splines and lines. To do this, right-mouse click on the text and pick Dissolve Sketch Text in the menu.

 

 

 

 

 

 

 

 

The Annotation is now converted into lines and splines. 

 

 

 

 

 

 

 

 

Note: Dissolve Sketch Text cannot be undone.

After the Dissolve was added, the Extruded Boss phsically looks the same.

 

 

 

 

 

 

 

 

Judy Marlo
CATI Application Engineer

Stratasys 3D Printing Helps Thermos Be an Industry Leader

Thermos engineers constantly innovate to stay a household name.  That's why since 2006 Thermos' state of the art research facility in Japan has been home to two Stratasys 3D Printing Technologies.  Starting with a Dimension FDM machine in 2006 and later adding the Objet260 Connex, Thermos has been able to create products with the impressive look, feel, and ergonomics their customers have come to expect.

Visit the CATI website for the entire Thermos Story.  

Jim TeDesco
Marketing Manager
Computer Aided Technology, Inc.

Injection molding, Many unknowns ...One answer: SolidWorks Plastics

SolidWorks Plastics simulates how melted plastic flows during the injection molding process to predict manufacturing-related defects on parts and molds. You can quickly evaluate manufacturability while you design, to eliminate costly mold rework, improve part quality, and accelerate time to market. A Results Adviser provides troubleshooting steps and practical design advice to help diagnose and solve potential problems.

Some key unknowns are time, pressure and temperature reached in cavity to eject the part.e 

Fill Time represents position of the fluid at regular intervals as it fills the cavity. Red color precedes the blue regions. Fill time is a key result and is calculated by default every time you run a test.

While you glance over outputs, the results advisor has a green light indicating the part can be successfully filled with injection pressure of X psi and clamping force of Y ton. The software also tells you the pressure is reasonable and gives a % of the max injection pressure the machine you picked can create. Based on these outputs, the software suggests any geometric changes that can improve part design e.g thickness can be reduced by z% and still have the same fill time. 

Pressure at end of Fill is the pressure required to fill the entire mold including the sprue, runner, gate and cavity.

Air Trap are caused when converging polymer melt fronts create an air pocket in the mold cavity. By appropriately venting, flash or burn marks can be avoided.

Cooling Time given an idea on totaly cylce time, in addition to when the part can be ejected. Cooling Time calculation is based on 90% part temperature is less than material ejection temperature.

You can  model cooling lines to get accurate results on warp effects, if any. More on that to come.

If you are trying to predict and avoid injection molding manufactuing defects, eliminate costly mold rework, improve part quality or reduce time to market, you ought to take a look at SolidWorks Plastics.

Rajat Trehan

Product Manager

Computer Aided Technology Inc.

The Future Generation of SolidWorks Engineers

With my earlier article this week letting everyone know that it is National Engineers Week I asked that everyone get out and do their part to spread the work to the next generation of Engineers. I followed thru with that with a visit to my son Conner's Kindergarten class.

I spent about 20 min talking with Mrs. Hickey's class about engineering. I wrote about my visit to Mrs. Hickey's class in my monthly blog article for SolidWorks. If you would like to read more about this please find the article thru the link below. http://blogs.solidworks.com/tech/2014/02/the-future-generation-of-solidworks-engineers.html

Thanks

Josh Altergott

CATI Support Manager

SolidWorks Select Other

You may have known that the Select Other command in SolidWorks is very useful when trying to select hidden faces or edges of a model while using a command such as adding a Mate or applying a Fillet.  But did you also know that you can use this awesome tool to selectively turn off faces of complex models allowing you to temporarily see into a part for better understanding of complex surfaces?  Let me show you how to do this in SolidWorks 2014.

First, we will left mouse click on a face of this complex part model.  Doing this we see the familiar pop up toolbar and gives us access to the Select Other command:

Next we will use this mouse changing icon to right mouse click on faces that we want to temporarily hide:

The result is we can now see deep into this model to see the surfaces are blended together to help us fix or patch surfaces in imported geometry for example.  The uses of this command are really quite numerous and very user friendly.  Give this a shot the next time you are faced with an imported model from a vendor or supplier that you need to clean up in SolidWorks.  You may be surprised how useful this can be.  Enjoy!

Brian Reel

CATI