Slightly Advanced SOLIDWORKS Surface Tools
Most of us are creatures of habit. This can be especially true for those of us who work with 3D CAD programs on a daily basis. We tend to use the same features and modeling techniques the vast majority of the time. This may be because we are working on similar designs or simply because we know those tools and what they can do.
It also reveals a little about how we learned the program. Regardless of whether you are self-taught or have been through formal training, when you are learning SOLIDWORKS you start with sketches, with tools from the Sketch toolbar and with tools from the Feature toolbar, and you produce solid models.
This is how the process continues for many. You never need to look for different tools, and you certainly never need to look at the Surfaces toolbar. You only have to Google “SOLIDWORKS surfacing” to be told that it is there to produce models that are not possible with solid modeling tools. All the examples shown are made of organic shapes and smooth curves.
However, hiding in plain sight are a range of surface features which can greatly assist with your day-to-day solid modeling. To use these surface features when solid modelling, let’s reflect back on the original intent that SOLIDWORKS first had for surfaces, and that is reference geometry.
We’ll run through a few of these surface features and see how they can be incorporated within our daily solid modeling.
Cut with Surface
There is a little bit of irony that the Cut with Surface feature is to be found on the Surface toolbar. If you customize your toolbars and look for Cut with Surface, you will find that it is listed under Features and not Surfaces. Either way, it is a simple and efficient tool. It does exactly as the name indicates, and uses a surface to cut the solid.
SOLIDWORKS also uses planes to cut away a solid. It is often easier to select a plane when the plane is parallel to the side you want to remove material from.
However, there is more often a need to use the Cut with Surface tool in conjunction with the Offset Surface feature.
The Offset Surface tool is used to recreate a surface with a zero distant offset or to create another surface at a distance away from the selected surface.
That surface can be used in numerous different ways. A common use is when you need to scribe a part with the shape of another part. In this case, we have an oval shaped sink which sits on a countertop. We will cut the shape out of the countertop.
As it is in an assembly, we can use Edit Part on the countertop and use Offset Surface, to recreate the selected surface of the sink the required distance from it. That distance could be a zero offset. If you do change to a zero dimension, you will see the command change from Offset Surface to Copy Surface.
We can now use Cut with Surface to create the cut.
What do we do with the Surface now that we no longer have a need for it? We could simply hide it but it will be better to delete it. When using this combination of solid and surface bodies, SOLIDWORKS will assist by creating different folders in the feature tree for both the surface and solid bodies.
There is a Delete/Keep Bodies tool which is another feature that hides by default on another toolbar – in this case, the Direct Edit toolbar. This too can be used to remove the surface. However, you may prefer to access this tool by selecting the body from inside the Surface Bodies folder and using the Delete key on the keyboard. This will automatically launch the Delete/Keep Bodies command with the body shown selected. Hit the Enter key to confirm.
The use of Offset Surface is only limited by your unfamiliarity with it. Once you start using it, it becomes one of those go-to commands. If you work regularly in large assemblies and need to reference parts from different sub-assemblies, you will appreciate working within the part. As shown above, the ability to recreate a surface from one part in an assembly to form another part allows you to work within the part. The surface might be used as a reference to create a sketch or to create a new part from the surface.
Delete Face is a versatile tool because of the options it has, which change what the tool can be used to achieve.
Delete Face with the option to Delete is a way to change a solid body into a surface body. By deleting a face of a solid body, you lose the solid body and are left with surface body, and you will enter the realm of surface modeling. But that is for another article. Let’s concentrate on how we can use this tool with a solid body.
The Delete Face with the option of Patch is one of those miracle commands. With a single command, you replace the need to use three or four other commands to achieve the same result. It is especially useful if you are working with imported data or bodies that don’t have features.
For example, a drawer slide provided by the component supplier is not the correct part. You wanted a simple drawer slide, not a self-closing version. You could chase the supplier for the correct part—or have the part you need in a minute.
Using Delete Face > Delete and Patch, you can select all of the faces that are not required and it will delete those faces and patch the surfaces to retain the part as a solid body.
How about a sheet metal part with the wrong radius, or with holes that are not required?
The Delete Face using the Delete and Patch option is a timesaving feature with its ability to remove multiple faces and replace them with a single feature
Looking at the final option of Delete Face > Delete and Fill, it is similar to Delete and Patch but is used to replace multiple faces with a single face. Many models have tangential faces of the same radius which will display an edge. This might be common where you have mirrored a part to be symmetrical. While this might not be an issue in the model, it is normally not how you would like the faces to be displayed. With Delete and Fill, you can replace those faces with a single face.
Surface tools can be used to assist with solid modeling. However, Delete Face > Delete and Fill has a hidden trick useful for imported models, which often suffer from translation issues. It’s not unusual for a model to have surface issues when it is created in one program, saved to a neutral format and then brought into SOLIDWORKS. It is also not unusual to have what looks like a solid model be a surface model. Plenty of models do not show any gaps and appear to be a solid body.
Use Delete Face > Delete and Fill to remedy the situation. Selecting any face to fill not only replaces the face but in the background, the model is checked to make sure it is sealed and automatically made into a solid model.
How you model in SOLIDWORKS should constantly evolve. This can take place over many years as new commands or options appear and the SOLIDWORKS interface evolves with each year’s release. And one of the greatest changes in modeling techniques in the last few years has been the surface features used with solid modeling, as mentioned in this article.
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About the Author
Michael Lord has spent his working life in Product Development & Engineering at TRAKKA Pty Limited, an Australian manufacturer of Motorhomes (RV) & Special Purpose Vehicles. He is also a Group Leader – Sydney SOLIDWORKS User & representative on the SWUGN Committee (Pacific Region). Further thoughts on the use of SOLIDWORKS can be found at michaellord.me.