You have only 3 hours—these tips and tricks will save you time.
Are you good at SOLIDWORKS? Think about it. It’s one thing to think you’re good at SOLIDWORKS; it’s another thing to be able to prove it. With the Certified SOLIDWORKS Professional (CSWP) exam, you can say you’re good at SOLIDWORKS and hold up the CSWP certificate as proof.
But getting a CSWP is no easy task. The CSWP is a challenging 3-hour exam that is more a test of speed than skill. The questions may not trip up veteran SOLIDWORKS users, but the time limit might. The 3-hour time limit has emerged as the biggest challenge in passing the CSWP.
Let’s take a look at some tips and tricks to help you with this challenge.
Part 1—Game Plan for Passing the CSWP
1. Understand the Question Being Asked
The first thing to understand is that you’re modeling a part based on a given drawing. The question asks, “What is the mass of the part?” Here’s an example of the first question on the CSWP exam, which can be downloaded here.
2. Getting Started
The first three things you should do on the CSWP exam are shown below:
- Set your units
- Define your variables
- Set your material
3. Design Intent
The part you create for question 1 will be reused and edited for questions 2 and 3. So when you are creating the part, think about how it could change. The challenge is that you don’t know how it will change, so here’s my recommendation—define the dimensions exactly as they are shown in the drawing. This goes for both the sketch dimensions and the feature parameters.
This is an educated guess about how the part might change based on observations and is consistent with all the certification exams as well as the Model Mania competition at 3DEXPERIENCE World.
4. Variables and Changes
The second step when getting started (shown above) is to create variables. This will create more up-front work but will make the upcoming changes a breeze and therefore overall save a ton of time. You only have 75 minutes for the first segment (part modeling). The only way to effectively get it done in sufficient time is to leverage variables. The exam suggests that you use variables. Notice that a significant number of dimensions are called out as variables, which are all defined as part of the question.
You can reuse the part modeled for question 1 for question 2 with just a few changes. All the changes are made obvious, so you don’t have to worry that you missed any. It’s mostly just the variables that will change. If any dimension changes, it’s called out in an obvious way, like being circled on the drawing. Although question 1 took 15 minutes to model, questions 2 and 3 combined should take less than 5 minutes thanks to variables.
Part 2—Tips & Tricks for Passing the Exam
For this part, we will use the official example exam that can be downloaded from this link here. I recommend following along at home for the first part and then trying the second part on your own.
Tip 1: Getting Started
To get started, you’ll want to begin setting up the part. Do these same three steps every time:
1. Units
Match the document units to the units used in the question. It’s easy to use the status bar in the lower right corner of the screen to switch unit systems. Just pick the correct one from the list to quickly change the document properties.
2. Variables
Add the variables and equations listed in the question. SOLIDWORKS lists all the variables in the equations folder in the Feature Tree, which is hidden by default. You can either set the system option to have this folder always visible or you can right-click at the top of the tree to click “manage equations,” which is in the hidden tree items option. All you need to do is add this in the Global Variables section. Even though some of the variables are given in the form of an equation, it’s still defined in the Global Variables section. This is such an important section that it’s worth spending a minute to double-check your work.
3. Material
Define the material of your part as it is given in the question. For this example, the material is alloy steel.
Tip 2: Using Variables
When it comes to variables, the hard part is setting them up. Once they’re all defined, you can easily use them. For example, the base is B wide by A high, so I will use those as the dimensions instead of typing in values. Just hit the “=” sign to switch to “variable mode” so that you can use the variables. Because my hand is already on the keyboard, I like to use arrow keys to save time and navigate through the list to get to the correct variable.
Tip 3: Model Exactly Like the Drawing
You’ll notice that when I create any features, I define the dimensions exactly as they are defined in the drawing. This is a technique that works well for doing any SOLIDWORKS certification or competition. There are a few tricks, however, that you need to know.
Tip 4: Use the S Key to Minimize Mouse Movement
Model the base as it is shown in the drawing and add dimensions using the variables. The main trick here is to minimize mouse movement. I like to leverage the S key shortcut bar instead of using more customizations because I prefer to keep my system as close to out of the box as possible. But that is because I’m a SOLIDWORKS instructor and students will have various customizations or no customizations at all.
Tip 5: Auto Transition from Line to Arc
With the next section, I’ll save time using a thin feature extrude. Instead of 8 lines, I can draw the shape with just 3 and use the extrude feature to fill in the thickness.
Pro Tip: The arc section can be created by leveraging the trick of auto transition to arc. This is done within the line tool. After you place a point, don’t click again and just leave the endpoint for a moment, then come back to the point to switch from line to arc. For this process, you’re just moving your mouse, not clicking it.
Tip 6: Thin Extrude
Use the thin extrude to save time and fill in the rest of the shape. Watch out for the prompts from SOLIDWORKS to fill in the open contour. This could be helpful in other instances—though not for this process. To keep with the strategy of modeling exactly as shown in the drawing, you’ll need to leverage the combination of modeling with sketch geometry and feature parameters.
Tip 7: Waking Up References
Leverage all the existing geometry you can to help you model quickly. You don’t have to add additional reference planes or midpoints if existing geometry can get the job done. To wake up any reference points from existing geometry, just hover your mouse over them. For example, here we hover over the edge to wake up its midpoint so that we can place the circle on it.
Tip 8: Change Extrusion Start—Extrude from Offset
By default, extrusions begin on the sketch plane. But here, it’s helpful to begin at an offset. You can change the “start from” property of an extrusion by expanding the drop-down menu to reveal the options. Seeing this for the first time was a real eye-opener. Imagine all the planes you don’t have to create because of this. Just in this example, we didn’t have to create an extra offset plane, nor did we have to add the dreaded two-direction extrusion.
For the next tip, we will move ahead to adding some of the fillets, but for those of you following along, I’ll fast forward through the next steps, which are a repeat of adding the cylinder and another extrusion in the corner. Just remember to minimize your mouse movement to save time.
Tip 9: FilletXpert
To help speed up the process of adding fillets, you can leverage the FilletXpert’s suggestions. The trick to using this is to hover your mouse over the suggestions to see if any of them will help get the job done. You’re looking for edges highlighted in a magenta color. FilletXpert has a pretty good track record of suggesting what works for the design and can be a huge time saver on the CSWP.
Tip 10: Offset Entities
After adding the additional 15mm fillet on the base, you can see that the next cut-out is just a 9mm offset of the outline. This is a perfect time to use the offset entities command, which copies the shape at an offset.
Next, we will create a basic extruded cut.
Tip 11: Copy and Paste Features
Once the extruded cut is created, you can reuse it by copying and pasting it. Just like you’re accustomed to doing, this is a control C and control V operation. Click on the feature and copy it. Click on the face and paste it. You’ll, of course, have to do some cleanup, but the end result is time savings.
Be sure to add the final details—hole wizard holes, fillets and chamfers. Then you’re ready for your answer.
To find the answer, click on the Evaluate tab and use the mass properties tool to find the mass of the part. Remember the part is made of alloy steel as defined in the problem statement. This is their way of checking the part volume but with an additional step just to make it a little bit harder.
So that’s the first question, which should have taken around 20 minutes. Now here are questions 2 and 3 in live time:
You can see how the model instantly updates after adjusting the variables. At 20 minutes into the exam, we have one question completed. Then, in only 2 more minutes, we will be well on our way with three questions completed.
Those are the tips and tricks I think you need to know to pass the first part of the CSWP exam. But this is just one of the three segments of the CSWP. It’s a challenging exam that brings credibility to your claim of SOLIDWORKS mastery. You will have proven that you’re a certified pro at SOLIDWORKS because you didn’t just make your models right; you made them quickly.