Advanced Breakdown of the SOLIDWORKS Boss Extrude Tool
One of the oldest commands in the SOLIDWORKS software is the boss/base extrude command. An Extruded Boss/Base feature will allow you to take a 2D sketch and add thickness to it in the third dimension. Every few releases, this feature gets some terrific functionality added to it. In today’s blog, we will review and break down some of the great tools available in each section of the extrude command.
The “Blind” End Condition
One of the first things to learn about the extrude command is the concept of the end condition. The end condition can be thought of as the parameter or rule that causes the extrusion to stop.
In Figure 1, we can see that the sketch has been created as a rectangle with the dimensions 40mm x 100mm. We then begin the extrude command and choose an end condition from the pull-down menu. The default end condition is “blind,” which means we will take our sketch and extrude it a set distance from the sketch plane. After that distance is met, extrusion will stop. So the condition for ending the extrusion is that it will proceed a set distance and then stop. Again, this is known as a “blind” end condition.
The “Direction 2” Option
Another common option for an extrusion is to extrude the sketch in two different directions.
Figure 2 shows the same extrusion as Figure 1, but with the checkmark for Direction 2 selected. Oftentimes when creating solid models, we need an extrusion to go a certain distance in one direction and a different distance in the other direction. In this case, we chose to go 20mm in Direction 1, which is up, and 7.5mm in Direction 2, which is down.
Each of the end conditions and options that are available in Direction 1 will be available in Direction 2 (with the exception of “Mid-Plane”), so as you read through this blog, remember that each of the options I describe for Direction 1 will be available to you if you choose to use Direction 2.
The “Reverse Direction” Option
Another important tool in the extrude command is the ability to reverse the direction of the extrusion.
Sometimes when we enter the extrude command, we discover that the extrusion is going the wrong direction. This icon (which looks like two angled arrows facing opposite directions) may be selected to reverse the direction of the extrusion as it originates from the sketch. In Figure 3, we can see that the upper half of the image shows the blind extrusion going in the default direction (up) and the lower half of the image shows the same blind extrusion going in the reverse direction (down).
The “Mid-Plane” End Condition
When working with the SOLIDWORKS software we often design parts starting from the origin and working our way outward. If you want to create an extrusion with your sketch plane dead center, consider using the “Mid Plane” end condition.
Figure 4 shows an example of a mid plane extrusion with a depth of 20mm. An important element of the “Mid Plane” end condition is that it will always take the total depth and apply half of the value to one side of the extrusion and half of the value to the other side of the extrusion. Thus, in this example, the extrusion is going up 10mm and down 10mm.
Additional End Conditions
When creating certain features, there will be a significant benefit to incorporating a more dynamic relationship to the condition that ends the extrusion. For example, rather than creating a blind extrusion, you may want to create an extrusion that always goes up to a certain face on the model. This way, if the model changes in size, the end face of the extrusion will always move with the new location of the selected face. To create this type of relationship, you would change the end condition to “Up to Surface.”
In Figure 5, we see an example of a more dynamic end condition. If the underlying rectangular base was to grow or shrink, the depth of the new extrusion would change so that it always terminates at the selected face (shown in pink above).
Some other examples of these types of dynamic end conditions in the extrude command are “Through All,” “Up to Next,” “Up to Vertex,” “Up to Next,” “Offset from Surface” and “Up to Body.”
When creating certain features, there may be the requirement for draft or taper to be applied to the faces of the feature. This is particularly important when design parts are to be cast or injection molded. In the case of the extrude command, this may be accomplished by choosing the icon for “Draft” while creating the extrusion.
Selecting the “Draft” icon will allow you to specify the amount of draft you would like to add to the extrusion. It is important to recognize that this draft will be applied to every face of the extrusion, aside from the top and bottom faces. If you wish to apply draft to just certain faces, or you wish for the draft value to vary, you should leave this option unselected and create a draft feature or features after the extrusion is complete.
You may also choose to apply the draft in the opposite direction by selecting the checkmark for “Draft outward.”This option is beneath the draft angle, as shown in Figure 4.
Creating a “Thin Feature” Extrusion
So far we have discussed the ability to take a closed rectangle and extrude it into a rectangular prism. Often when working with plastic parts or sheet metal, we want to create a simple sketch of lines and extrude this into a feature, applying thickness during the extrusion.
To create a new extrusion using the thin-walled option, start by creating a sketch and then choosing the extrude command. After beginning the extrude command, choose the checkmark for “Thin Feature.”
Please note that if your sketch is an “open sketch,” such as the sketch shown in Figure 6, the option for “Thin Feature” will be automatically selected. Once you choose to create a thin-walled feature, you will be prompted to input the wall thickness of this thin-walled feature. In Figure 6 above, the wall thickness has been set to 2mm.
One of the greatest enhancements to the SOLIDWORKS software came in the 2003 release when SOLIDWORKS added the ability to work in multibody solids. In simplest terms, a multibody solid is a single part file with two or more bodies that are not merged together.
In advanced part design, there are occasions when an extrusion that would normally be merged to the existing solid might function better if the extrusion was not merged. In these advanced scenarios, you may choose to uncheck the option for “Merge result” within the extrude command.
In Figure 7, we see an example of a co-planar circle being extruded from the planar surface of the top of the rectangular base. You have unchecked the option for “Merge result,” therefore the new extrusion will not be merged to the rectangular base and will become its own body. This technique is used in advanced modeling to control which features affect which bodies. It could also be used to design an entire assembly within a single part file.
When working in the SOLIDWORKS software, users are encouraged to create neatly trimmed and cropped sketches. An example of this would be a simple rectangle used in Figure 1.When creating a layout of multiple features that are intended to work together, it is often easier to include all the details in a single sketch. This often creates a complex sketch that cannot be extruded with the default options for extrude. In these scenarios, users may take advantage of the “Selected Contours” option.
When creating a sketch that has multiple nested contours or non-trimmed overlapping lines, the extrude command will not yield a preview right away. You must first add the desired regions to extrude to the “Selected Contours” box.
After clicking on the extrusion command, the user will see that the “Selected Contours” area of the extrude command is available. You can mouse over different regions of the complex sketch and left-click to add these regions to the “Selected Contours” area of the extrude command. Once the desired regions are selected, you may click the green checkmark to finish the extrude command.
After creating the first extrusion, you can select the sketch again from the feature tree and choose to extrude the same sketch over and over again. Each time, you can choose different regions in the “Selected Contours” box and assign a different height to each region.
As you can see in Figure 9, the complex sketch from Figure 8 is named “Sketch1.”This single sketch can be used over and over again to create the three different boss-extrude features. For each of the three boss-extrude features, you would choose a different area of the sketch use in the “Selected Contours” box.
Direction of Extrusion (Non-Standard)
Occasionally when working in SOLIDWORKS, we want to create an extrusion that goes in a nonstandard angle. Let’s consider the following example:
In Figure 10, we see a circular sketch being extruded with an end condition of “Up To Surface.”What we really want is for the direction of this extrusion to match the angle of the wall. To accomplish this, we can click in the box for extrusion direction and we can select the edge of the extruded wall.
In Figure 11, we can see that the “Selected Direction” box has been activated and an angled edge has been selected from the model. The extrusion of the circle will now run parallel to this edge, rather than perpendicular to the sketch plane. This can be a real time-saver, and this will also be a dynamic relationship, meaning that if the angle of the edge changes, the angle of the extrusion will automatically update.
One of the more recent additions to the extrude command is the ability to extrude from a location other than the sketch plane. Most features you create in SOLIDWORKS will be extruded from the sketch plane, but occasionally, you will wish to extrude from a location offset from the sketch plane by a set distance or at a set location based on other geometry in the part file, such as a vertex or another face. To do this, you may choose the desired setting from the “Extrude From” pull-down menu.
In Figure 12, we can see that the “Extrude From” pull-down menu has been selected, and we have chosen to extrude from a selected vertex. The vertex has been circled in red, and the preview shows that the extrusion will now begin from the location(height) of the vertex, rather than extruding from the original sketch location.
Most of the time, I leave this option set to the default value of “Sketch Plane,” but I find it to be very useful when my goal is to extrude geometry onto a non-planar surface that has a thin wall.
In Figure 13, we see an example of a thin-walled part in which the sketch to be extruded was created on the front plane, but the extrusion was generated from the front wall of the part.To do this, we started the extrude command and then selected the “Extrude From” option and selected “Surface/Face/Plane” from the pull-down menu. We finished by selecting the front non-planar face of the model to declare where we wanted the extrude feature to begin.
When SOLIDWORKS was first released back in 1995, the extrude feature was included in the software, but we only had a few of the options we see today. Over the years, some great enhancements have been added to the extrude command. Depending on what type of geometry you are creating, you may find that utilizing some of the great enhancements can be a real time-saver and will help you get your products to market faster.
About the Author
Tobias Richard is a SOLIDWORKS elite applications engineer from Philadelphia, Pa. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support and tips and tricks since 2001.