Part Configurations

Often customers will want to view multiple configurations of the same part to see which they like best. Instead of creating four or five new part files to show the customer, it is much easier to create each version of the same part with the configurations manager tab.

Configurations

Within the configurations tab on the feature manager tree, right click on the Part and select Add Configuration.

Figure 1: Configuration tab location

Organize Configurations

Each configuration should have its own unique name to quickly distinguish between each configuration. This will help distinguish each configuration within assemblies and drawings to ensure the correct model is chosen.

Figure 2: Configuration Name

The saved configurations will appear in a pop-down menu within assemblies and drawings as seen below. Simply click on the part and the option to choose between each configuration will appear. Keeping simple and descriptive names will be the best option for configuration models.

Figure 3: Pop-down Menu

Modifications to Configurations

The feature tree model gives the option to suppress and unsuppressed features. Each configuration will be slightly different which means some features will need to be suppressed and others unsuppressed depending on the design intent. The default configuration should be the original design before modifications are incorporated.

Default:

Figure 4: Default Bracket

Large Mount:

Figure 5: Large Bracket

Small Mount:

Figure 6: Small Bracket

The reason each configuration has its own hole wizard feature is to ensure it has no relation to any other configurations. If bracket were to have only one clearance hole, then all three configurations will be identical; hence the need for three separate hole clearances.

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Pattern commands are a designer’s best friend in terms of replication and improving overall efficiency. Linear, Circular, and Curve driven patterns are all common commands used by the everyday CAD user. This blog will guide you through using these three pattern features in SolidWorks and provide context as to when they can be used to simplify the modeling process.

Linear Driven Pattern

The Linear Pattern Command is used to drive features, faces, or bodies in a linear direction.  This feature helps save time by cutting down the repetitive movements of adding a bunch of holes or other forms of geometry. In Figure 1, the location of the linear pattern command in addition to the curve and circular driven pattern commands are shown.

Figure 1: Command Locations

Using an existing hole wizard feature, the linear pattern will systematically generate identical holes across the model. The first step in executing a linear pattern is to select a desired feature in the Features and Faces selection box or by preselecting prior to hitting the Linear Pattern Command (Figure 2).

Figure 2: Selecting the Feature

After selecting “3/4-10 Tapped Hole1” feature in this case, the dimensions defined in the feature appear and can be used to aid in the patterning process (Figure 3). The next step in the command manager is selecting up to two linear pattern directions. For this example, the two 4.00 dimensions were used to define two pattern directions, as they are in the desired linear direction to make an equally spaced square hole pattern. Additionally, there is also the option to select edges, faces, planes, and other geometry in the preferred linear direction.

Figure 3: Setting Direction

Now that the directions are set, the next step is to fill out the necessary parameters for each direction required to make the pattern. The first parameter is the number of instances. As seen in Figure 4, the desired “3/4-10 Tapped Hole1” hole feature pattern will add 2 instances in both directions creating a 2×2 square. The distance in both the vertical and horizontal direction was set to 12 inches in order to keep the pattern centered to the square piece.

Figure 4: Hole Instances

If the desired pattern direction is oriented incorrectly, the opposing arrows button (highlighted) next to the selection box flips the direction relative to the reference selected. Figure 4 also shows a pattern preview on the part (enabled from the checkbox on the bottom of the command manager), which will help verify the orientation and intended pattern direction.

Lastly, as seen in Figure 5 the green check mark in the top left corner of the manager will execute the command and reveal the pattern on the model.

Figure 5: Final Check

Curve Driven Pattern

In the next example, the Curved Pattern Command is used to execute a hole pattern consistently about the outer curvature of a cam (see Figure 6). The setup and command manager layout are nearly identical to the linear pattern and the steps are listed below as follows:

– Select the feature/face/body to pattern

– Select a curved reference (this can be an open or closed curved geometry)

-Adjust the direction, spacing, and number of instances in the desired pattern

-Preview the pattern and then execute.

In this curve driven pattern example (see Figure 6), I selected a hole feature, the edge of the cam as the Direction 1 reference and adjusted my instances and spacing to 4 and 0.425 correspondingly. As with the linear pattern, up to two different directions can be added.

Figure 6: Curved Pattern About an Edge  

Circular Driven Pattern

The Circular Pattern Command is an excellent tool used to replicate features, faces, or bodies in a rotational manner about an axis. In this example (see Figure 7), I show how to replicate an extruded cut with filleted corners about a round piece of tubing.

Figure 7: Circular Pattern Overview

Similar to the linear and curve driven pattern, the first step is selecting a feature (or features in this case) to replicate in the Features and Faces selection box or by preselecting prior to hitting the pattern command.

Figure 8: Selecting Features and Faces

After the cut-extrude and fillet are both selected, the intended rotation axis is selected in the top selection box under Direction 1 in the command manager (see Figure 9). The rotation direction can be toggled using the arrow button to the left of the selection box. The next step is to select the degree of spacing and number of instances.

Figure 9: Circular Pattern Parameters & Preview

In this example, since the original extruded cut through both sides of the pipe, the pattern only needed to rotate the feature 180 degrees instead of 360 to complete the cut all the way around, so I chose a 45-degree spacing and 4 instances to complete the pattern across the tube. As with other pattern features discussed, up to two directions can be selected.

That’s all for now! You now know the basics in Linear, Curved, and Circular Patterns. If you like the content or have questions, signup for our email list to stay in the loop for solutions or weekly content.

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Feature Mirroring

While creating parts in SolidWorks, efficiency and accuracy are essential when working on a project for a client! For projects that are repeatable, Perception Engineering saves time by applying the mirror feature command if models are symmetrical. SolidWorks is equipped with a few different types of mirroring commands: sketch mirroring, part mirroring, and feature mirroring. For this blog the focus will be on feature mirroring utilizing the given top, right, and front planes to create feature mirrors!

Getting started

The mirror icon is located on the feature command bar as seen in Figure 1.

Figure 1: Mirror Icon

To ensure proper use of this feature, be sure an extrusion is modeled. This feature will mirror the extrusion over a desired plane. A simple exercise to do is to create a feature on the front plane and have it share one edge with the right plane as shown in Figure 2. This feature works the same no matter how complex the model, as long as it has one shared edge with a plane.

Figure 2: Highlighted shared the edge with a plane

Plane and Feature Selection

Now that you have a feature ready to be mirrored, such as an extrusion. Select the mirror icon on the features toolbar. The first selection box asks you to pick a mirror face/plane. Select the right plane as the mirror plane, then the right plane will appear in the selection box, as seen in Figure 3. Now, all that needs to be done is select the feature that is to be mirrored. The second selection box asks for a selection of a feature to be mirrored. It is possible to click directly on the feature itself to select it, or it can be selected on the feature manager tree. Once the feature that is desired to be mirrored is selected it will appear in the selection box.

Figure 3: Property manager

There is also an option to choose a 2D face to mirror instead of a 3D feature. By using this option, you cannot mirror bodies but only surface face features such as holes, surface cuts, and other features that are placed on an already created 3D body. To do this correctly, the face must be mirrored onto an already created feature, the face cannot be mirrored into blank space to become its own feature.

Figure 4: Faces to Mirror

The ability to mirror faces can be very helpful. If there are multiple complicated features on an extrusion body, rather than draw out every one they can simply be mirrored to the desired locations.                                                                                                       

Preview Selection

There is an option to preview the mirror at the bottom of the property manager, as seen in Figure 5. If the partial preview is selected a 2D highlighted copy of the newly mirrored feature will show across the right plane from the original feature. If the full preview is selected it will highlight both features showing that the outcome will be one combined body with an extrusion depth shown in 3D. All there is left to do now is click the green check at the top of the property manager and mirror the feature!

Figure 5: Preview modes

Reasons to Mirror

Mirroring is a simple and easy way to save time when modeling parts. Mirroring is used primarily to create perfect symmetry for a part, this way you only need to make half of the part in only half the time! Mirroring can also be used on more than just part bodies, it can be used on smaller extruded features, cuts, and various shapes that appear symmetrically throughout the part.

Figure 6: Fully Mirrored

The team here at Perception Engineering use the mirror command to save time when the part model is similar in geometry. Both features and sketches are used in the modeling phase regularly so having the models orientated symmetric along the top, right, and the front plane will save some time.  

Thanks for tuning in our weekly blog! Please subscribe to our weekly postings and feel free to ask us any questions or concerns and our team will get back to you. 

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Exploding an assembly view in SolidWorks can make all the difference when trying to show every component involved in the making. Instead of showing multiple views and angles, one view can be used to show all components. A well done exploded view will also help in the understanding of how the entire assembly fits together. Exploded views are used in almost every industry when it comes to explaining a product and how it works. Knowing how to use the exploded view feature is a crucial key feature and will be finishing touch needed when showing an assembly.  

Feature/Icon Location

Exploded views are only able to be performed on an assembly, not a single part. Therefore, the exploded view icon is only located inside of an assembly file. To reach the icon it can either be found on the assembly tab toolbar or can be created by going under the configurations tab and right clicking on the assembly icon and creating a new exploded view. Both locations are shown below in Figure 1.

Figure 1: Feature/Icon locations

Exploded View Feature Manager

There are two types of exploded view step types to choose from, as seen in Figure 2. There is a regular step and radial step. By choosing regular step, objects selected, being one or multiple, will all move in the same direction with each other. The radial step type is mostly used on parts that are in a circular type pattern. When using a radial step, all parts chosen will move away from each other from a common center point when dragged. Almost as if they are lying on a circle that’s radius is expanding. The focus of this blog will stay on regular step exploding since this is the most common type to be used.

Figure 2: Explode step types

Exploded part selection

Exploding an assembly using regular step type is quite simple. After choosing the step type the components that are desired to be moved are selected and dragged, this can be one part or multiple. If multiple parts are highlighted at the same time they will all move in the same direction when pulled. The direction is chosen by the user. After clicking on a part to be moved an origin point is shown on the selected part showing the possible direction and rotation options. Simply click and hold on the arrow in the direction that is desired and drag the mouse. After the components are moved an “exploded step 1” will appear in the exploded steps view box inside the feature manager. From here previous steps can be edited by right-clicking on them. An example of these steps is shown in Figure 3 below.

Figure 3: Explode step 1

Under the part selection box in the feature manager, there is the option to input set values for how far the part will move and what rotation angle can be put on the selected part. These can be used for exact spacing of exploded parts if it is needed. There is also an explode direction selection box located below the part selection box, as shown in Figure 4. In this selection box, the direction of the exploded step can be changed to match a face or axial direction of another part located inside of the assembly. This can help in the overall flow of the exploded view, giving it a cleanly spaced look when the exploded view is finished.  

Figure 4: Set value locations & Explode direction change

Other Exploded Options

Located at the bottom of the exploded view feature manager are a few other options to choose from when exploding an assembly. A very helpful one is the option to turn off and on select subassembly parts. This allows you to move a subassembly as one whole part or one part of the subassembly at a time. This option can only be applied if there is a subassembly inside the assembly that is being exploded. There is also a button that gives the option to reuse a subassembly explosion. If a subassembly being used has already previously been exploded, by clicking this button that exploded state will be shown and it will not have to be redone! These options are shown in Figure 5.

Figure 5: Subassembly explode options

After Exploding The Assembly

Once the assembly has been fully exploded it can be quite hard to tell just exactly where everything has come from and where everything goes back to. Especially in an assembly with a large number of parts. There is an option to add smart explode lines to help with this. These lines, when added in, follow the path that every part was dragged from all the way back to its origin. This helps greatly in showing how an assembly is put together. However, if there are a large number of parts the lines can become cluttered and overwhelming, this option can be left up to personal preference. In Figure 6 below a final exploded assembly is shown with smart lines as well as the location of where to add in the smart lines. 

Figure 6: Full exploded view with smart lines

Things to look out for

When exploding an assembly, make sure all components can be seen from one view. Typically for exploded assemblies, the viewpoint is from an isometric view. Also, when exploding an assembly, after clicking off a part, the assembly may collapse and go back to its original state. You do not have to redo the entire exploded assembly. Simply go back to the configurations tab and under the exploded view configuration, right click and hit edit feature, the assembly will re-explode.

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