How to Choose Between a Feature Pattern and a Sketch Pattern
When creating models with patterns in SOLIDWORKS, I am often asked, “Is it better to make this feature using a sketch pattern or using a feature pattern?” My answer is almost always the same: “Use a feature pattern.” In this article, we will examine the differences between the two types of patterns and look for the direct impact of performance and rebuild time when using one technique over the other.
Keep in mind that while I almost always say to use a feature pattern, there are exceptions. By the end of this article, you should have some good tools to determine whether a sketch pattern or a feature pattern is better, depending on the circumstance.
Our model will begin with the following geometry.
The starting geometry
We will be adding a pattern of rectangular holes with small corner fillets to the plate. Feel free to create this geometry and follow along with the steps.
When we are examining the rebuild times for our model, the screenshots will reflect the following option being enabled.
Figure 1. “Verification on rebuild” is enabled.
In Figure 1, we can see that “Verification on rebuild” is enabled. This rebuild mode typically takes a little longer but results in a more elaborate and accurate rebuild. We will leave this option on for the remainder of the tutorial.
When we finish our model, we will see results similar to the following.
Figure 2. Results using a sketch pattern and a feature pattern.
In Figure 2, we can see the results of the final model using the Performance Evaluation tool. We can also see that using a sketch pattern requires a much longer rebuild time than a feature pattern and that the majority of the rebuild time is derived from the complex sketch and cut extrude feature for the holes.
Now that we have taken a look at the final results, let’s take a look at how we got there.
The Sketch Pattern
We will begin today’s example by creating the holes in the plate using a sketch pattern. A sketch pattern is created by selecting all the desired entities within the sketch mode and then specifying a distance to pattern these entities in Direction 1 and Direction 2. Since we are using the sketch pattern command, we must create all the entities for the rectangular hole (including the corner fillets) in one single sketch. The starting sketch for the sketch pattern feature will look like this.
Figure 3. Sketch geometry for the sketch pattern.
As we can see in Figure 3, the sketch has a lot of relationships. I always recommend to my students that they keep their sketches simple. One of the downsides of creating a pattern using the sketch pattern is that the sketch must contain all the desired pattern geometry, which often requires a fairly complex sketch. Later in the article, we will see that using a feature pattern will allow us to create a much simpler sketch of a rectangle and then add fillets at the feature level.
Next we will create the pattern of the sketch geometry. We will begin by clicking the sketch icon for Linear Sketch Pattern.
The Linear Sketch Pattern command can be found on the sketch toolbar.
After clicking the Linear Sketch Pattern command, we are prompted to define a direction for the X and Y of our pattern. In a sketch pattern, we are not required to choose edges to define the direction of our sketch pattern.
Figure 4. The direction of the sketch pattern can be defined as X axis and Y axis.
In Figure 4, we can see that the red sketch origin is showing a longer red arrow pointing up and a shorter red arrow pointing to the right. The shorter red arrow represents the direction of the X axis, and the longer red arrow represents the direction of the Y axis.
In our example, we wish to pattern the rectangular hole along the X axis and Y axis of the sketch, so we can leave the Direction 1 and Direction 2 boxes as shown (X axis and Y axis). However, if we wanted the pattern direction to be different, we could choose edges from the model to define the X axis and Y axis of the pattern.
Now that we have defined the two directions of the pattern, we can click in the box labeled “Entities to Pattern” and select all of the entities representing the rectangle with rounded corners.
Figure 5. Selecting entities to be included in the pattern.
After selecting the entities to be included in pattern as shown in Figure 5, we can finish the pattern by specifying the pattern distance and number of instances in the Direction 1 and Direction 2 boxes. For our pattern, we will use a spacing of 13 mm and 10 instances for Direction 1. We will use a spacing of 11 mm and 8 instances for Direction 2.
Figure 6. Setting the spacing and number of instances for Direction 1 and Direction 2.
In Figure 6, we set the spacing for our pattern in Direction 1 and Direction 2. If we were working in a feature pattern, we would be ready to finish the command, but in a sketch pattern, we have a few additional settings to examine. In the sketch pattern property manager, we can see that there are settings for “Dimension X spacing,” “Display instance count,” “Dimension Y spacing” and “Dimension angle between axes.” These options should all be checked.
Figure 7. All five of these options should be enabled for most sketch patterns.
In Figure 7, we can see the options for the sketch pattern. In most sketch patterns, all five of these options should be enabled. We are now ready to hit the green checkmark and examine our results.
The sketch pattern is complete, but the sketch is still under-defined.
After clicking the green checkmark to complete the sketch pattern, we examine the results. The pattern looks correct, but the sketch is still under-defined. The Sketch Pattern tool creates a centerline between the first two instances of the pattern in Direction 1.
Figure 8. The sketch pattern generates a centerline between instance 1 and instance 2.
As we can see in Figure 8, the sketch pattern generated a centerline between instance 1 and instance 2 of the pattern, but this centerline does not have a horizontal sketch relationship. If we add the horizontal relationship to this sketch centerline, the entire sketch will become fully defined.
Figure 9. After adding the horizontal relationship, the sketch becomes fully defined.
In Figure 9, we can see that the sketch has been fully defined, and we are now ready to perform a cut extrude. We will use the “Through All” end condition for our cut extrude.
Adding a “Through All” extruded cut for all holes.
After adding this extruded cut, we can choose the Performance Evaluation tool from the Evaluate toolbar.
The Performance Evaluation tool can be found in the Evaluate toolbar.
The Performance Evaluation tool will give us a breakdown of the total rebuild time required for each feature in a part file.
The Performance Evaluation results for our part created with a sketch-driven pattern.
As we can see from the results above, the majority of the rebuild time is dedicated to the sketch and feature used to create the holes. This is the result of trying to use an overly complicated sketch to create a cut extrude.
Next let’s take a look at the process of creating the same geometry using a feature pattern.
The Feature Pattern
We will start by deleting the cut extrude and sketch we created in the previous steps.
Delete the sketch and the cut extrude of the holes that were used in the sketch pattern.
One of the benefits of using a feature pattern is the ability to keep our sketches simple. Since we will be creating a feature pattern that includes the rectangular hole and the four corner fillets, we can keep our rectangular hole cut very simple. The sketch for the rectangular hole will look like this.
Figure 10. The sketch of the single rectangular hole can be kept very simple.
After completing the sketch shown in Figure 10, we will cut extrude this sketch through all.
Next we will create a simple fillet of 1 mm in each of the four corners of this rectangular hole.
Figure 11. Add a fillet feature of 1 mm to each of the four corners of the rectangular hole.
In Figure 11, we can see the addition of the corner fillets as a feature. Since we are separating this fillet from the sketch (by creating the fillet as a separate feature), we are creating a situation where, in the future, we can create a simplified configuration of the model by suppressing this fillet feature. In the sketch pattern example, we would not have been able to do this, since the fillet was included in the sketch itself. This ability to suppress/unsuppress the fillet feature is another benefit of creating the pattern at the feather level rather than creating a sketch pattern.
We are now ready to create the feature pattern by choosing the Linear Pattern command from the Features toolbar.
The Linear Pattern command can be found on the Features toolbar.
After launching the Linear Pattern command, we are prompted to select an edge of the model to define Direction 1 and Direction 2 for the pattern. We will choose the edges as shown.
Figure 12. Selecting edges to define the pattern Direction 1 and pattern Direction 2.
As we can see in Figure 12, the linear feature pattern is asking for an edge to define Direction 1 for the pattern. We can also (optionally) select a second edge to define the pattern Direction 2. We will select the two edges as shown above.
Next we will specify the spacing and number of instances for our pattern. We will match the numbers we used for the sketch pattern and will set Direction 1 to have a spacing of 13 mm and 10 instances. We will set Direction 2 to have a spacing of 11 mm and 8 instances.
Lastly, we will choose the feature or features to pattern. We will select the simple rectangular hole and the hole corner fillet feature.
Select the two features to be patterned.
After selecting these features and examining the preview, we are satisfied that the preview looks good, and we are ready to hit the green checkmark to finish the command. The finished patterned part should look like this.
Finished part after pattern is complete.
We will now use the Performance Evaluation tool to examine the rebuild time of our model after using a feature pattern for the holes.
Performance Evaluation showing rebuild time after using the feature pattern.
Now let’s compare the feature evaluation of the sketch pattern next to the feature pattern.
Figure 13. Performance Evaluation showing rebuild time of a geometrically identical part built using different pattern methods.
As we can see in Figure 13, the sketch pattern model has less features than the feature pattern model, yet the sketch pattern model has a rebuild time that is almost 10 times greater than the feature pattern model. Creating the model using a feature pattern, we were able to keep the sketch of the rectangular hole simple and tidy. We were also able to separate features for the rectangular hole and the corner hole fillets. This will give us the flexibility to create a simplified version of the model where the hole fillets are suppressed. For these reasons, the feature pattern would be a much better choice for the model we created.
So Which is Better for My Model?
Every model you create will be different, and you may find yourself in a situation where a feature can be created a number of different ways. By creating two different versions of the model, you can utilize the Performance Evaluation tool to determine which technique yields a faster rebuild time. You should also be looking for ways to keep your sketches simple, even if it means creating more features in the tree.
Generally speaking though, a feature pattern is better.
About the Author
Tobias Richard is a SOLIDWORKS elite applications engineer from Philadelphia. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support and tips and tricks since 2001.