Getting Closer to Losing the Drawing
Most engineering ideas start off as a sketch or drawing of some sort. Then the drawing becomes more refined and eventually ends up as a 3D CAD model, which can then be used for manufacturing or rendering or a whole bunch of other uses. CAD models are incredibly useful.
Then why is so much money spent on updating the original drawing when changes are made to the product? Surely, it’s better to just create a good 3D model in the first place that can be reused and updated at will, rather than spend thousands of dollars and hundreds of work hours going back, issuing a change request, waiting for approval, making changes to the drawing, and then waiting for the quality assurance loop to give it the OK. And after all that rigmarole, you still have to update the CAD model so that it fits the new drawing.
In addition to the headaches of updating redundant drawings, many engineering companies still insist on sending 2D drawings with TDG information to manufacturers, where the factory CAD technicians must then convert that 2D information into 3D data so that toolpaths can be generated for manufacturing.
Did you know that as a result of constantly transforming data between 2D drawings and 3D models, 60 percent of 2D drawings don’t match the original intended design? And according to the U.S. Department of Defense(DoD), up to 50 percent of a design team’s time is spent messing around with drawings. That’s insane!
And that is why model-based definition (MBD) is such a great thing. With MBD, it is possible to just jump straight to the 3D modeling phase, add the geometric dimensioning and tolerancing (GD&T) and product manufacturing information (PMI) data to the model, and then go about your day without worrying about the drawing. No more extra sheets of paper with tolerance and surface finish information. No more redline markups on printed PDFs. No more invoices to be paid for drawing updates. And, of course, the environment benefits, too.
As you are about to see in more detail, SOLIDWORKS 2018 MBD enables you do all this and more.
So let’s go ahead and take a look at how we can utilize these features in SOLIDWORKS 2018.
Opening the Tutorial
I initially created a bracket to use as an example for this article, but while searching through the SOLIDWORKS 2018 tutorials within the software, I found a much cooler model to work with for this example. And because the model is located in the SOLIDWORKS MBD tutorial section, it means you can give it a try for yourselves.
To get started, go to the menu at the very top of the screen, select HELP, and click SOLIDWORKS Tutorials in the drop-down menu. This will bring up the tutorials pane, and you can select All SOLIDWORKS Tutorials from the headings. This will show a list of all the tutorials available. I show a shortened version of this list in Figure 1. Take a look at the list and click SOLIDWORKS MBD Overview.
This will open the SOLIDWORKS MBD Overview Tutorial introduction screen in the tutorial panel. Click NEXT TOPIC at the bottom right of the panel. The next screen will provide you with a link to the location of the assembly model that is stored on your hard drive. Click that link, and you will see the drum pedal assembly open in your main design window (Figure 2).
Once the assembly model has loaded, click NEXT TOPIC (Creating a BOM table) at the bottom right of the tutorial pane.
Creating a BOM Table
The bill of materials (BOM) table is a staple of engineering documentation. The need to constantly update the BOM is a real pain in the neck and is also a resource-intensive task for many companies.
Thankfully, updating the BOM tables becomes easier with MBD.
Go to the FeatureManager design tree panel on the left, open the Annotations folder, right-click on Notes Area and click Activate, as shown in Figure 3.
Next, go up to the ribbon at the top of the screen, click the Assembly tab if it isn’t already selected, and click the Bill of Materials icon. This will open the BOM PropertyManager in the FeatureManager design tree area on the left of the screen.
In the PropertyManager, under:
-BOM Type, select Parts only
-Configurations, select Default
-Part Configuration Grouping, select Display as one item number and Display all configurations of the same part as one item
Then click the green check mark icon. You can now position the BOM in the main display area, and resize it as you see fit (just drag the outer borders or columns/rows to resize it), as shown in Figure 4.
When you have finished making your adjustments, go to the bottom of the tutorial pane on the right, and click NEXT TOPIC (Adding a Display State).
Adding a Display State
Now we need to add the various display states. Display states show the orientation of the assembly and how the parts are located with respect to each other. These display states can be in the form of orthographic, isometric or any other kind of view that you want to appear in your document. We can rotate parts or make them disappear from view, and once a display state has been assigned to that situation, we can recall it at a later time without needing to manipulate the parts again.
For the first view, we want to orient the annotations so they are in plane with the footboard (the actual pedal).To do this, go into the FeatureManager design tree and expand the annotations folder. Locate the Footboard component, right-click Footboard, and select Activate and Reorient from the menu. This will show the assembly from a top-down view.
Now, we only want to see the actual footboard in this view (not the rest of the assembly), so we need to hide the rest of the assembly. To do this, go to the FeatureManager design tree, locate the PART named foot_board (see Figure 5), right-click the part, and select Isolate. You should see all of the other parts of the assembly disappear.
Next up, we want to save this display state. Click the ConfigurationManager tab in the left-hand pane (see Figure 6), then right-click on the empty space in the ConfigurationManager area. In the menu, select Add Display State. You will notice at the bottom of the ConfigurationManager that this new view has been saved as Display State-3.
Now, go back to the bottom of the tutorial pane and click NEXT TOPIC (Capturing the 3D View).
Capturing the 3D View
The next step is to capture the 3D view. Go to the ribbon at the top of the screen, select the SOLIDWORKS MBD tab, and click the Capture 3D View icon, as shown below.
The PropertyManager options will open up in the left-hand pane. Here, you can rename the 3D View Name. In this case, we will keep the name as “Footboard”.
In the Configuration section, select Default.
In Display State, select Display State-3.
In Annotation Views, select Footboard.
And then click the green check mark when you are finished.
Now, go back to the tutorial pane, and click NEXT TOPIC (Copying a Tolerance Scheme) at the bottom.
Copying a Tolerance Scheme
Now we want to copy the tolerance scheme from the full assembly display state (Display State-1) to the isolated footboard display state (Display State-3).
At the bottom of the left-hand pane (ConfigurationManager) under Display States (linked), double-click Display State-1 and the full assembly will appear in the main window. Now,in the ConfigurationManager, double-click Grey. The assembly will turn grey.
Now, go to the ribbon menu at the top, select the SOLIDWORKS MBD tab, and click the Copy Scheme icon. This will open the SchemeProperties panel in the PropertyManager in the left-hand pane. We can change the scheme name here, but in this case, we will leave it as Dimension Schema 1.
In the Source Configuration section, select Default (see Figure 7). Click the green check mark, and then move to the NEXT TOPIC (Adding a Display State) in the tutorial pane.
Adding Display State (again)
Now that the tolerance scheme has been copied, we can add the new display state. This is the same procedure that we used before, except we want to ensure that all of the other annotation views (except for Footboard) are hidden. We can do this by going to the FeatureManager, opening the Annotations folder in the design tree, and right-clicking each component annotation and selecting Hide. Make sure that the Footboard annotation is not hidden. If it is, then right-click on it, and select Show.
Again, go down the FeatureManager design tree to the actual part icons, right-click on Foot_Board part, and press Isolate. All of the other components will again disappear. As before, now we click on the ConfigurationManager tab in the left-hand pane, right-click in an empty space, and click Add Display State. This will create Display State-4.
Now that we have added the display state to the grey component, we can move to the next step. Click Next Topic (Capturing the 3D View) in the tutorial pane.
Capturing the 3D View
Return to the ribbon at the top of the screen, select the SOLIDWORKS MBD tab, and click the Capture 3D View icon as before.
In the PropertyManager area, we will rename the 3D View Name as “Grey Footboard”.
In the Configuration section, select Grey.
In Display State, select Display State-4.
In Annotation Views, select Footboard.
Then click the green check mark and go to the NEXT TOPIC.
Adding Balloons to the Assembly
In the ConfigurationManager, double-click Default and select Display State-1 at the bottom of the pane. This will recall the full assembly.
In the FeatureManager design tree, expand the Annotations folder, right-click Front and click Activate and Reorient. The view in the main area will change to the front plane, and you will see the full drum pedal assembly from the side, complete with the DimXpert annotations. We don’t want these, because we are creating a new 3D view with bubbles.
To hide the DimXpert annotations, right-click Annotations and clear Show DimXpert Annotations.
Now, go to the SOLIDWORKS MBD toolbar at the top of the screen and click the Balloon icon.
In the PropertyManager, under Settings, in Balloon text source, select Bill of Materials1. This will link the balloon text to our BOM.
Now, if you click on a part in the main view, the balloon tool will know which part you are trying to identify and will create a balloon connected to that part via a leader line. Click to place balloons as shown in Figure 8. The balloons will automatically be numbered based on the BOM you created.
Click the green check mark and move on to the NEXT TOPIC.
Now we need to Capture the 3D View again.
Click Capture 3D View (in the SOLIDWORKS MBD toolbar).
In the PropertyManager:
In 3D View Name, type Balloons.
In Configuration, select Grey.
In Display State, select Display State-2.
In Annotation Views, select Front1.
Click the green check mark to finish, and click NEXT TOPIC.
Now that we have aligned our orthographic views with the corresponding planes for the annotations, we can do an exploded view.
In the FeatureManager design tree, expand Annotations folder, right-click Isometric and click Activate and Reorient. On the SOLIDWORKS MBD ribbon at the top, click Exploded View.
Now we can click on various parts in the design window and explode them as we see fit. Alternatively, we can expand the Hardware folder in the FeatureManager design tree and select the components from there. This is particularly useful for selecting hard-to-see items, such as screws. In this exploded view, I have exploded the base, two of the screws and the beater shaft (see Figure 9).
Now that the model has been exploded, we can go to the NEXT TOPIC and capture the 3D view again.
Click Capture 3D View in SOLIDWORKS MBD ribbon.
In the PropertyManager, in 3D View Name, type “Exploded View”.
In Configuration, select ExplView1.
In Display State, select Display State-2.
In Annotation Views, select Isometric.
Publishing the Document
We are done! We can finally publish the model as a document. Click NEXT TOPIC to continue.
If you take a look in the SOLIDWORKS MBD ribbon, you will see several options related to document publishing (see Figure 10). Here, we can click on the Publish to 3D PDF icon. If you wish to change the template to 3D PDFs, you can do so by clicking the Template Editor icon. We can also publish to eDrawing format, but for this tutorial, let’s look at 3D PDF publishing.
Now we can view our published 3D PDF document, with the BOM list, the various views (see Figure 11) and any other PMI data that we chose to include in it (see Figure 12).
Using SOLIDWORKS MBD removes the need for going back and changing drawings, because the main source of our data is in the form of a 3D model. This model can contain data for manufacturing, such as for CNC toolpaths, or even 3D printing. That same model can be used for creating a BOM, or for rendering to create marketing materials. In MBD, the 3D asset is central to everything.
In principle, one could create the model in 3D from scratch, assign the dimensions and PMI data, and produce an electronic drawing—then have that item manufactured without ever having to touch a piece of paper. Moreover, if we wish to update the final drawing information, we need only go back and alter the model.
As you have seen, the procedure for creating the document is fairly repetitive. It involves selecting the best angle for presentation, saving the display state, ensuring the annotations are available to that specific view, and then repeating the process until we have the views we require.
The good news is that we can make use of templates when it comes to creating the final document. So, while the process may seem a little tedious at first, I can promise you from experience that it’s a lot less time consuming than going from 2D to 3D and back again to 2D.
Give it a try for yourself.
About the Author
Phillip Keane is currently studying his PhD at the School of Mechanical and Aerospace Engineering at Nanyang Technological University, Singapore. His background is in aerospace engineering, and his current studies are focused on the use of 3D-printed components in spaceflight. He previously worked at Rolls-Royce and Airbus Military and served as an intern for Made In Space and the European Southern Observatory.