SOLIDWORKS - MBD

Model Based Definition (MBD) is an add-in tool that helps us to create 3D drafting with all PMI, this tool produces the output in eDrawings®, 3D-PDF & STEP 242 for clear 3D communication which bypasses time-consuming 2D processes and eliminates potential problems.  

MBD tool supports the establishment of document digitalization and control hardcopy utilization.

Creating MBD document for an assembly:

For creating the MBD with the necessary Product Manufacturing Information for the assembly mentioned in the image MBD tool must be activated.

Where to find,

Now the tool is available with plenty of options to work with the assembly.

Activating MBD also adds a 3D Views tab at the bottom with the Capture 3D view option. The capture 3D view option helps to capture the views of the assembly similar to the performance of sheets in the 2D drawing.

Creating Annotation view:

An Annotation view must be inserted with necessary view orientation for capturing each 3D view of the assembly in selected orientation. For this instance isometric is chosen as a view orientation for the newly created annotation view.

After creating the annotation view select activate and orient option from the right-click menu.

Note: It is advisable to create individual annotation view for each view captured via the Capture 3D view option

Creating BOM:

For creating notes & BOM separate notes area must be created for saving it. Now, for this instance a new notes area is inserted with the name of BOM Table and is activated from the right-click menu.

Now the BOM is generated for the assembly and it is positioned near to assembly view area without affecting the visibility of the assembly.

Now select *Isometric from the Annotations then click activate and orient option from the right-click menu.

Capturing 3D view:

After positioning the assembly orientation the current 3D view is captured with the help of the Capture 3D view option and it is saved with the name of Assembled.

Now the 3D view is created with BOM, similarly, we can add notes, balloons, dimensions, GD&T, etc. following the same procedure based on the needs.

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Essential SOLIDWORKS Tips and Tricks to Boost Your Productivity

SolidWorks Tips and Tricks

Tip 1: Auto-dimensions in Sketch Mode

In the above image, we can see that a rectangle is being sketched in a SOLIDWORKS sketch and as the rectangle is being created, dimensions are displaying on the screen. This is a function of “auto-dimensions” in sketch mode and it’s one of the most powerful time savers found in SOLIDWORKS.
To enable this functionality, start by launching Tools > Options.

Next, head into System Options > Sketch.
From the Sketch settings, the following two options must be checked:

Auto-dimensions in sketch mode are now enabled. To begin using this functionality, create a new sketch. Then begin creating sketch geometry.

Let’s use a circle as an example:
1.Single left-click the Circle command.
2.Single left-click the center point of the circle.
3.Begin moving your mouse away from the center point of the circle (without clicking anything).
4.Let go of your mouse (without clicking anything) and move your hand to the keyboard.
5.Enter the diameter (55mm) of the circle and press Enter.

You now have a circle with a parametric (driving) dimension.

Auto-dimensions can be used for a variety of sketch entity types including lines, arcs, circles and rectangles. Learning how to properly use auto-dimensions is one of the best ways to save time in SOLIDWORKS sketch mode.

Tip 2: Basic Arithmetic When Adding Dimensions to Sketches

When working on engineering related projects, we regularly need to perform basic arithmetic to calculate things such as offset distances and half distances. SOLIDWORKS allows us to do basic arithmetic directly in the dimension input boxes.

In this example, I’m using auto-dimensions to create the sketch for this part:

I begin sketching my first line at 135mm and then sketch a vertical line

at 12mm. Now I need to create a horizontal line but I don’t know what this dimension is supposed to be.

Since we can do basic arithmetic in SOLIDWORKS, I can simply type “135-25” and allow SOLIDWORKS to do the math for me.

After pressing Enter, I see that the line has been created to the correct distance and I can now move on to the vertical line for which I will use the same technique.

Although these are simple examples, this is a technique that I frequently use to save time and one which allows me to quickly define my sketches.

Tip 3: Reassign Dimensions using Dimension Grips

In the previous tip we saw that we can use basic arithmetic to quickly create driving dimensions at the correct locations. However, one could argue that although the geometry is correct, the design intent from the customer is not being maintained.

As we can see in the image above, the customer wanted the max height to be 65 and the customer wants this max height to be independent from the thickness of the plate. In our current sketch the total height is dependent on the 12mm plate thickness plus the 53mm vertical dimension. In a scenario like this, we can simply reassign the height dimension to the base of the model, using the dimension grip.

To do this, start by pressing escape, then single left-click on the 53mm dimension.

Next, move your mouse down to the lower arrow of the dimension, until you see this icon:

This is the dimension reassign grip icon. Once this icon appears, drag and drop from this point onto the desired location from the dimension.

The 53mm dimension has now been reassigned to the base of the model and has been recalculated to 65mm. We are now matching the design intent provided by our customer.

We can repeat this process with the 110mm dimension. Note that this time we will see the reassign dimension grip icon at the end of the dimension extension line rather than on the dimension arrow.

After reassigning this dimension grip, our sketch now matches the design intent of the customer.

Learning how to reassign dimensions in sketch mode is a powerful skill, and one which every SOLIDWORKS user should master. While it’s true that you could simply delete the dimension and recreate it, that dimension might be referenced somewhere else in the model and deleting it could cause negative effects downstream.  By learning how to reassign the dimension, you can prevent these types of model failures.

Tip 4: Create Angular Dimensions to an Imaginary Line

We have one final dimension to create in our sketch and that dimension is an angle dimension of 15 degrees. Unfortunately, we don’t have a vertical line to reference for this dimension.

SOLIDWORKS sketch mode offers a great solution for these types of scenarios: The “imaginary line” for angle dimensions. To access this functionality, begin the smart dimension command and single click the angled line in our sketch.

Next, single left-click an endpoint of this angled line. In this case I will click the bottom end point of this line:

After single clicking on the endpoint, the “imaginary line” crosshair for angle dimensions appears. We will then single click on the vertical arrow of this crosshair.

After clicking on this vertical arrow, SOLIDWORKS allows us to create the desired 15 degree angle dimension, relative to an imaginary vertical line.

Using the “imaginary line” for angled dimensions saves us the process of creating a vertical centerline and allows us to quickly create the desired driving angle dimension per the customer’s design intent. And, as a bonus, we can also use this functionality in SOLIDWORKS Drawings.

Tip 5: Add Mirror to the SOLIDWORKS Context Menu

Our fifth and final tip is one of my favorites and can be a HUGE time saver in SOLIDWORKS: add the “Mirror Entities” command to the context menu for sketch mode.

Whenever working in sketch mode, we can create geometry that represents one half of the desired sketch geometry and then mirror the sketch. Let’s say, for example, we wanted to create a handle shape, so we create a sketch that looks like this:

We have sketched half of the handle and we we’ve sketched a centerline. We are now ready to mirror the sketch. Since this is a function that I regularly use, I’d like to have a more intuitive workflow to access the sketch mirror command. This is a great spot to modify the context menu.
The context menu in SOLIDWORKS appears automatically after we select one or more entities.  If I select all the entities in this sketch, the default (out of the box) context menu looks like 

There are some excellent tools on the default context menu, but I’m not seeing the Mirror Entities command. So, I’ll right mouse button on this menu and choose Customize.

Next I’ll find the sketch command for mirror entities and drag and drop this icon onto the context toolbar.

After adding this icon, I can choose OK and then return to the sketch. Now when I window select all the entities in my sketch, the context toolbar displays and includes the Mirror Entities command.

And this allows me to quickly create the desired geometry.

Editing the SOLIDWORKS Context toolbar to include the mirror entities command can be a great way to save time in SOLIDWORKS sketch mode, especially for users who frequently create centered and symmetric parts.

Tip 6: Auto Arrange Dimensions

Creating Dimensions is a more important task for the designers so that communication takes place among the manufacturers. Placement of Dimensions must be neat, precise and eye-catching to ensure error less manufacturing.

In SOLIDWORKS Drawing, we have a fantastic tool called AUTO ARRANGE DIMENSIONS that enables the user to place the dimensions spaced, aligned, centered, adjusted and staggered if necessary.

This can be done by Window select the required dimensions-> Pause the mouse for a few seconds-> Icon will appear-> Select the first one “Auto Space”-> Dimensions selected will be equally spaced. Further needed, we can adjust and stagger.

 

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