The HRS Blog – SolidWorks and CAMWorks

When designing in SolidWorks, at times it may be beneficial to create parts that have more than one solid body, in applications like weldments, sheet metal, or mold tools. It may also be necessary to show how those parts go together using an exploded view. While it is possible to save the individual bodies as separate part files in an assembly and perform an exploded view there, it may be easier and quicker to perform the exploded view in the multi-body part. This functionality was introduced in SolidWorks 2012.

This process, outlined in the steps below, is similar to creating exploded views with assemblies.

1. Create a New Configuration

Manage exploded views by putting them in their own configuration. Click on the Configuration tab > Right click below > Click “Add Configuration” > Add Name “Exploded View”

2. Create Exploded View

Go to the Insert menu and click on “Exploded View”. You may also locate the exploded view using the command search in the top right corner of the SolidWorks window.

3. Explode Steps

This will bring up the Exploded View Property Manager. Select the bodies to explode then drag the manipulation handle in the desired direction. You may select single or multiple bodies to explode in a given step. These steps are added on the left side titled “Explode steps”. Under “Settings” it lists the bodies selected, the direction, and the distance. To add additional steps, just select different bodies and drag.

4. Auto-Space Components

Clicking the “Auto-space solid bodies after drag” option will take all of the components selected and space them equally apart from each other.

5. Edit Explode Steps

Right-clicking on the intended step and selecting Edit Step allows you make adjustments to the selected components, their direction, and distance. Components may be added or deleted. The direction can be edited by selecting an arrow and toggling the reverse button. You can align the drag handle to a specific entity by right-clicking the drag handle and selecting: Align to, Align to Component Origin, or Move to Selection. After aligning the drag handles, select an arrow for the direction. You may specify a different distance next to the “D1” field. When finished, click “apply” and then “Done”. You may continue to edit existing steps or add new ones. Click the green check-mark when finished.

6. Finished Exploded View

To go back and forth between the collapsed and exploded state, go to the Configuration Manager tab and expand the “Exploded View” configuration; inside is a derived configuration that holds the exploded view with its explode steps. Right click on the derived configuration to collapse or explode the part. Edit Feature takes you to the Explode Property Manager. The “Collapse Items” option just collapses the configuration tree.

Limitations:

There are a few limits to this command. You may not re-use a multi-body explode in an assembly exploded view, like you can re-use a sub-assembly exploded view. Also, you cannot animate explode or collapse or save it as an .avi file. Lastly, cannot hold down alt to move and align the drag arrows like assembly explodes.

Everything is always a matter of cost. How many times have you been deprived of something because it’s just too expensive?  On the design side, you always have to keep in mind how much your product is going to cost to make, going from computer screen to an actual tangible product. If you are on the side that’s going to be manufacturing that design, you probably don’t want to spend your entire day quoting  out your clients’ projects, but actually spend the time manufacturing it too!

Have you ever wanted to do a linear pattern that varies from instance to instance? With SolidWorks 2013, now you can. New in 2013 is the ability to vary the dimensions of a patterned feature, as well as the spacing in between each instance to increase design flexibility and ease of use. Let’s take a look.

Here is a part with a slot that needs to be patterned. However, the design intent is that each slot should be a different length, width, and distance apart. Those dimensions need to vary. In SolidWorks 2013, you can do exactly that.

First create a linear pattern with the existing slot as the seed.

Then, after initiating the linear pattern feature, choose an option in the PropertyManager, labeled “Instances to Vary”. When you enable this option, you are given the ability to constantly increase the distance between increments. For example, you can set the increment distance to 10 mm, which means that the distance between instances will increase by 10 mm each time (e.g.  30, 40, 50 mm, etc.).

Selecting the blue box under Instances to Vary and then selecting a dimension allows you to choose dimensions that you would like to vary along the pattern. For example, you could increase the slot length by 25 mm and the slot width by 5 mm for every instance.                  

So there you are. With SolidWorks 2013, you can create a linear pattern that can vary dimensions and distances between increments. The possibilities for making customized patterns are endless.

For more information on what’s new in SolidWorks 2013, visit the Hawk Ridge Systems website – www.hawkridgesys.com or download the What’s New in 2013 datasheet.

That being said, there are plenty of situations in SolidWorks when things aren’t quite so crystal clear; one in particular that comes to mind is with section views. Lucky for us, SolidWorks has two abilities that should help out.

One of these tools is the checkbox called “Keep cap color” which allows the user to paint all sectioned faces on a model with a specified color. This comes in especially handy for those certain section views that you may not immediately notice, such as this lens assembly from the National Optical Astronomy Observatory, NOAO.

You can even do a multi-plane section view and paint each group of sectioned faces with different colors, which proves especially useful for transparent parts! Just check the box for Section 2 to add another section plane, and click the button for “Edit Color.”

Finally, SolidWorks also gives us the ability to remove the section cap entirely, revealing the details of your model underneath. To do this, simply uncheck the box named “Show section cap,” which is on by default. This is a great way to examine the innards of an assembly, such as these socket head cap screws, without going through your feature tree and hiding a bunch of parts first.

So, if you have updated to SolidWorks 2012 or beyond, save yourself the potential embarrassment! Use these new section view options and always be in the know.