Tips for taking the CSWP

Although I've still got a few things to go over I'm almost ready to take a shot at the CSWP. In preparation I've collected a few notes for myself on best practices for the test. As always I'm welcome to additional Tips/Tricks/Questions and even light criticism.

1. Prepare for the test and allocate a time: Once begun each section of the CSWP must be completed in one sitting so prepare everything before hand. In addition to studying preparation can involve opening Solidworks, Starting a file, Setting dimensions to that of the test (should always be checked). Opening a Word Document or Image editor to help document/note/or enlarge test questions, Presetting Equations (A=, B=) if using equation method, creating a directory and file structure for the test.

2. Take the test on a system you are familiar with. Don't look for a workstation with better performance unless you plan to import your user settings. No point in wasting time looking for a command that for years has been on your primary toolbar but isn't on others.

3. Do NOT rely on the image provided as a template. Dimensions are changed from test to test so the image used will not be to scale (this is noted). Rely on the dimensions.

4. Assume unseen features extend through all. Typically only a single view is given, with detail views for zooming, so again trust the dimensions and if an edge looks to come to a point assume that it does.

5. If the model seems to be missing something DO NOT overreact. At the "How to pass the CSWP" session at Solidworks World at least half of the "questions" were some variation of "I failed the test because it was ill defined and I didn't know what the picture meant". Again make a best guest assumption and follow through. If you complete the test and feel it was unfairly written state your case to the certification specialists at Solidworks, Avelino and Mike are more than happy to help if you are polite.

6. Make sure to properly sketch about the origin shown in the image. Most questions ask for a Center of Mass or overall mass. For the former it is crucial that the model is oriented exactly as modeled, for the latter not so much but don't take the chance.

7. Read all questions before beginning. Pay attention to material changes, origins, dimensional changes. Note which values appear in balloons as these are the ones that will change.

8. Save your work. Relaunching after a failed Cosmos simulation is easier than retaking the whole test. If you do have a legitimate preformance failure you may be granted a retake. Even if Solidworks will grant you another shot at it no one wants to waste another 1.5 hours, if you save and can recover with a passing grade this will not be an issue.

9. Use the help files if necessary. They are a part of the software. If you see the exam and realize your studying wasn't comprehensive enough do what you can first and then see if a search will help you.

10. Relax. With any test anxiety can be a killer. It's not life or death so take a deep breath.

Combine; Add, Subtract, Common and Sketching with Pictures: A designer's best friend

Many products these days are more than just simple polygons slapped together. Increasingly ergonomics and design are becoming the driving force behind device designs. These complex shapes can be difficult to model. Some designers use mainly surfaces, which are plentiful and powerful within solidworks, but of course there is another way to make some of these items.

Fortunately a few key things happened to allow for a great example of this use. The first was finding a modeling challenge over at Product Design Forums. The second was an email that dropped into my inbox for the new Beta release of Solidworks. Now working in a Beta version can be a hassle but this one came with a perk to good to pass up, full access including Photoworks( a product they are dumping for their own Photoview 360) but in the mean time I've got 27 days of Photoworks fun so let's play.

To start off with the combine method for the phone model and render I wanted to sketch the profile views given. This can be done freehand but where's the fun in that. Instead I imported the image using Tools>Sketch Tools> Sketch Picture. The first step was actually to make a reference line. I knew I was going to want to size the phone to 105mm so I drew a line 105mm and dimensioned it. This gives a nice reference which allows me to do a click and drag resize.
Note here I've turned on tranparency to eliminate the primarily white background. The next step is to utilize the picture to define the geometry. The front view can be done with a few splines. Here though I only modeled one half and mirrored the other half. For organic features where symettry is important using the Mirror command will save a lot of headache.

Once I had the top view I moved to the bottom. A reference line should not be necessary here. Instead the previous sketch can be used as a reference. (Note: Not using the previous sketch can cause design problems down the line as will be shown in later images). For the bottom sketch I decided to try another method. With the sketch picture inserted the AutoTrace function can be used.

On this picture autotrace seems like it isn't going to be the best option, instead I used some of the basic tools to model my outline. I didn't realize till after but it's important to see that the bottom view is not the bottom profile. Looking up the view contains the edges that stick out and the actual bottom is smaller than the profile of the image, again another reason autotrace was a bad option.

Regardless the autotrace function is intresting and has plenty of application for gathering the design intent pulled from freehand sketches, marketing images and the like. AutoTrace does have to be activated though in the Add-Ins menu (Tools>Add-Ins...). This is the same screen that will be used to later activate the Photoworks Add-In. However Photoworks is a robust add in and can eat up preformance so while I'm modeling I'll leave it be.Next I modeled the side and top view, then it's time to build some solids. I could use these views for surfaces but I prefer solids as they are more the focus of the CSWP. The first step is to extrude the front view giving a basic outline of the phone. Next up the side or top view. To test how this method works I jumped ahead (reviewing and fixing will be the next post). On subsequent extrudes though there is one key to note. The "Merge Result" check box should be cleared, the reason for this is built into the name "combine".

To combine bodies a model ust first have multiple bodies. Clearing the Merge Result box means this extrude will not merge with any existing portion of the model. Solidworks automatically adds a "Solid Bodies" folder to the feature manager tree (depending upon your settings this may always be present but empty) which will show how many bodies are present.


After extruding all three views I combined them using the Insert>Features>Combine option. I selected "Common" in the feature manager which meant that only the part of the model contained in ALL of my bodies would stay. Below is the result.
Looking at the above image the curves of the phone can begin to be seen, but so can the problems with this method. By only using simple extrudes most of the complex surfaces and curves failed to appear. To fix this I can go back and lock some of the geometry and utilize Lofts and guide curves which should give me the end result I want, but that will be another post.

If you have any tips, problems, or questions about how to model this portion leave a comment. Otherwise take a look at the next post to see how the design fares using lofts.

Feature Conditions- Start and End: How to define Solidworks Models

Choosing how and where to start and end solidworks features can significantly impact the design intent of a model. Although there are numerous start and end conditions in general, the selection criterion on a feature by feature basis is very specific and surprisingly intuitive.

The easiest way to review these is by example. For the model on the sample test I opted to build the side profile first. In this way I was able to maintain most of my geometry in a single sketch. However there was a curved portion that I modeled as a second sketch. To do this I highlighted the face, right clicked and selected sketch. This "start condition" is then the face selected. If this face is eliminated errors will occur.

Because my base sketch of the first extrude contains this line I know that this face will be built anytime the base sketch is unsuppressed. Making this sketch on the face causes it to be a "child" of the first sketch.

Parent child relations are time dependent in the feature tree (ie. order matters). Identifying which features are truly child features will help determine what start condition should be selected. This face is clearly a parent child as it clearly always is meant to create a single block with all edges tangent to others.


The sketch is then created. I used the auto relation to the midpoint to ensure that the half circle would always rebuild regardless of the thickness of B (my initial extrude). For the end condition I know that I only want the part to be of thickness D, as shown in the sample test. I could use a blind extude and link the dimension to D but that just leaves one more equation I have to worry about. However I know that the bottom face is always going to be "D" distance due to parent sketch (pictured below). Because of this it's easier to simply use the "up to face" end condition. It is also good to note that the selected surface is viewed by the software as extending indefinitely so even of a feature extends outside of the modeled and shown portion of a surface the extension of the surface will be used to cut.





The basic end condtions are:
Blind- Very basic will go through any modled componetns for a given distance.
Through All - Will extend up to and thru all existing bodies
Up to Next - Will extend only up to the next surface
Up to Vertex - Will extend up to a given vertex. The vertex does not have to be in the line of the extrude of cut. Up to will be measure perpendicular using an extrude direction.
Up to Surface - Great for relating to existing geomety
Offset from Surface - Useful for clearances this is used in many part designs to create uniform wall thicknesses and allow for tolerance clearance.
Up to body - For multi body parts or in asemblies. Good for components that are to be modeled with zero clearance. Care should be taken when using this in manufacturing as it applies to tolerances.
Midplane - Uses the sketch as the center line of a mirror. Good for modeling but dimensioning these can lead to confusion as the overall thickness will be doulbe any input value.

The HELP menu. How I passed the CSWA.

One of the beauties of taking an exam like the CSWA or CSWP is that to complete it you need access to Solidworks. Not only does this give you the ability to create parts and gather an answer to modeling questions but it also gives you access to the help menu. I can not count the number of times I've heard critics of the CSWA or CSWP declare "How would I know that, I never use that part of the system" usually this comment is in response to a multiple choice question which only appears on the CSWA exam.

I had no issue with ANY of the multiple choice, and see why some designers claim the test is lacking because of them, When I took the CSWA (at Solidworks World 2008) every single one of the multiple choice questions could be answered in under 60 seconds by simply accessing the help menu and checking the answer. Most I knew right off, but the peace of mind that comes from seeing it the question and answer verbatim in the documentation was a huge boost to my-in test moral.

The HELP files are PART OF SOLIDWORKS which means they are entirely usable during the exam. Use them.

Basic Extrude Features, Shells, Dimensioning and Mass Properties for the CSWP

After sketching on the CSWP prep list comes the basic 3D features. For the exam it's possible to get by with only the basic features if the model is designed correctly, although others may help significantly. The extrude and cut features should be fairly easy to figure out for any user who is accustomed to dealing with CAD design. Draw a sketch and extrude it into a 3D of said sketch or make a cut in the shape of the sketch.

Shell gets a little bit more in depth with the ability to select faces to keep or remove with the shell. Typically this is only a single face which is the opening of the part, however a part can be shelled with no faces selected which will result in a hollow component.

As with the sketch features the extrude and cut tools should be familiar to most users. The biggest issue with parts such as the one seen in the sample test is how and in what order to build the features. For the second problem on the test there are tons of ways to model the same thing all of which will yield the same answer. This is where dimensioning correctly can come in handy.

Dimensioning is critical and should be linked to features that will not change. Mid points, center lines and construction geometry are all very helpful in laying out a sketch. For example a hole can be centered between edges by drawing bisecting construction geometry lines first and then sketching the circle at the intersection point.

Make sure to look ahead though so that these construction lines connect to points that will remain even if some features are removed. In this example the lines extend to the outer edges not the inner edge, which will disappear when the Shell feature is suppressed.


Voila. 4 Features and a few basic equations and the first question is done. Another 30 seconds of changing variables and question 2 is out of the way as well. Now comes the biggest tip of all.

SAVE YOUR WORK!

Even on the CSWP test is is important to save work. Crashes happen and rebuilding an entire part with design intent is the easiest way to eat up testing time. 3 hours will go quickly so make sure a copy of your model is saved for each question.

Of course things are easier with no time constraints and spread out over a few days. In the real test those two problems should take approx. 30 min to complete so practice is worth while. The exam will cover much more than just these basic but being able to quickly check off a few questions can be a huge boost to a tester's score and will allow for more breathing room and time to check more complex models.

Sketching: The basis of Solidworks

Despite the recent addition of Instant 3D and a number of free form deforming tools most Solidworks models begin with a well laid out sketch. This is true too for the CSWP exam. Laying out a sketch in the wrong fashion is the easiest way to make a costly mistake.

The first step is understanding the basic tools. The built in solidworks tutorials (30 Min lesson, 3D sketching) cover most of the basic. Starting a sketch, creating circles, offset, construction geometry, dimensions, hole wizard, fillets, 3D sketching, patterns and more. Most other sketch tools can easily be learned by selecting it and clicking the ? in the resultant feature manager.

There are also a few tricks that can help with the workflow of things.

Grid: Solidworks is good at having features automatically snap to relations. Horizontal and vertical lines, edges and points snap to coincident. This can be both misleading and wrong given the inaccuracy of the pictures in the CSWP. Sides that look to be co-planar in the exam question figure may be just that, but they may change in future questions. I find that having a grid available helps lay things out with proper relations while still making sure the realtions do not overdefine or improperly define certain edges.

To turn on the grid check the box at(Tools>Options>Document Properties> Grid/Snap> Display Grid)
To enable snap to grid check the box at (Tools>Options>Syctem options>Sketch Relations/Snaps> Grid)

S key and RMB in-context menus: The single biggest time saver in newer version of Solidworks is the addition of in context menus. The RMB (right mouse button) brings up an in context menu that can be customized from a limited list. This is very helpful in flying through a quick sketch and eliminates the need to get the mouse back up to the tool bars. Even more powerful is the S key which brings up a shortcut menu of actions typically used in the current state and it can be customized with anything. Not only can the S key access all the sketch features needed it can also be customized to add such items as Extrude and Cut, the two most commonly used features following the sketch tool. Although the movement of the mouse to the top of the screen might seem like a small thing to eliminate over time this ligtning quick access to any needed feature can significantly reduce the time spent looking for items.


Full defined sketches: Making sure a sketch is fully defined is simply good practice. Under defined sketches cause major problems when changes must be made, arcs over extend, lines cross, dimensions loose defining vertices, and features fail. It is much easier to go back and remove definition that it is to painstakingly correct each error caused by an under defined sketch. For visual purposes a fully defined sketch or sketch entity will appear black while under defined entities will appear blue. Once your sketch is complete click the RMB and get the in context menu. This will include an option for "Fully define sketch". A property manager appears and allows the user to select the entities and relations to be defined.

Variables: Because of the nature of the CSWP where a single model with only a few changes can make up 3-4 questions it's important to allow read ahead and plan for future questions. Typically an exam model will have a few variables labeled A,B,C, D. Each question will ask for the center of Mass given different values of A,B,C,D so being able to quickly switch the values can save valuable time. One easy way to setup these variables is to simply use equations. This way the sketch dimensions can be set to equal "A", "B", "C", and "D" even if D applies to 4 values only one value, "D", must be changed. Making a single change is easier than fixing every instance of the value and again eliminates issues.

To set a variable using equation is a two step process. First the variable must be defined. To do this select Tools>Equations. This brings up the equation manager. Select "Add" and then simply type

"D"= X

X should represent the value of A.

Next "D" must be linked to a dimension. Again select add then select the dimension, the default format should be similar to "D3@Sketch2". This is the "Primary Value" of the dimension and can be changed in the feature manager of the dimension tool if necessary. Then simply tell SW what you want this value to be. In this case "A" the resultant equation is a rather simple

"D3@Sketch2"="D"

Now to change the values for questions 2-4 simply change the equation for "D" and all instances will be changed.


As is usually the case in 3D cad there is more than one way to handle organizing a design and layout and each is user. If anyone has a better workflow for laying out these variables input is always welcome.

For now the tutorials and these tips will be all that I'm overviewing for sketches. Of course, as mentioned earlier, sketches are the corner stone of the Solidworks package so further review will be a part of all other studies.

Beginning prep for the CSWP exam

To a regular user of sketching tools it's easy to look down the list of items to know for the CSWP test and think "Mirror, Filet, Dimension ... I know a majority of theses things well, I should be fine". But the CSWP test is setup such that a small mistake at the beginning can be very costly. Because many of the questions are based around the changing of only a few dimensions. This is designed to test the design intent and completness of a model. Making sure to properly name and label key features can save a lot of precious time.

That's when looking further down the list and saying "Max von Mises stress location, Max Displacement location... this is an engineering test". The problems asked on the CSWP exam tend to ask for the center of mass. Change measurements A, B, C and you've got half the test. This is why a simple mistake can be so costly, and it seems pertinent to fully prepare. So where to begin...

How about right at the top of the CSWP Prep List.


Sketching

Learning to model in 3D

One of the more popular questions among designers and engineers in the 3D world is "What CAD package do you use". There are a number out on the market, all with various features and niches, and choosing the right ones to learn and master can be a difficult tasks. It is common for professionals to utilize a number of programs for various tasks but for the most part settling on a single CAD for a majority of projects is the way to go.

So which to pick, and what to consider. Do you go for the market leader? The low cost option? The free open source package? Do you need special features for electronic layouts? A good 2D>3D option? What do most customers use? Will my files be compatible? Will I have to upgrade hardware?

All of the above are good to consider before signing up, but even better is managing to get a free license to test things out. Many products offer trials for 30 or 60 days. Earlier in 2009 one of the big players in the industry, Solidworks, began offering the "Engineering Stimulus Package". This gave a free student version of Solidworks standard to any out of work engineer as a way to allow for continued learning. Along with the trial license comes access to the built in tutorials, forum access and a free voucher to take the CSWA (Certified Solidworks Associate) test.

In my past job I was fortunate enough to attend Solidworks World in San Diego where I got to take the CSWA so for my own personal Engineering Stimulus Package the end game will be the CSWP (Certified Solidworks Professional) exam.

The CSWP covers a variety of materials from basic modeling to Simulations and stress testing. There are a few copies of sample tests floating around.

CSWP 2008 Sample Test

Solidworks Training Files

There are a number of training programs available through private companies and through Solidworks VARs. Opinions vary on the worth of each of these as most of them are rather costly. My suggestion ,having seen the test once before and understanding mostly what it is about, is to forgo the CSWP specifics and to focus more on learning the program than learning for the test. A robust knowledge of design principles and an understanding of the given tutorials should be sufficient to allow a motivated user to gain certification.

The next few posts will be primarily about learning and training for the CSWP. In addition to the listed resources I also have access to the MyIGetIt library of training courses. With any luck, in a few short weeks this blog will contain more information of 3D design as well as a snazzy CSWP logo to announce my passing.

If you've taken or plan to take the CSWP exam please share your plan of attack or any tips/tricks/things to remember for others.
 
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