Nouvelles méthodes de conversion d'une surface en solide avec SOLIDWORKS

Article by Rod Mackay updated December 16, 2015

Article

When working with surfaces in SOLIDWORKS you would typically be converting Surface into Solid using the Knit Surface or Thicken Surface feature. But with the latest versions of SOLIDWORKS you now have the ability to create a solid using the Boundary Surface or the Trim Surface features, provided the surface features can create a closed volume from the inputs.

The ‘Create Solid’ option now included with these features was formerly called ‘Try to form solid’, and in previous releases, you often had to use the Knit Surface tool to combine the surface manually before you could convert the surface into a solid.

Converting Surface into Solid using Trim Surface

Let’s have a look at a simple example of creating a solid using the Trim Surface feature. Here we have a cell phone button design comprised of two surface bodies (shown in the surfaces folder in the tree). I want to generate a solid model from the two surfaces.

Converting Surface into Solid

Two Surfaces

I should be able to create a solid using the Trim Surface tool because where the surfaces intersect is a closed volume – you can see the volume space clearly from the section view shown below:

Surface Section View

Surface Section View

  1. First I’ll activate the Trim Surface tool from Insert > Surface > Trim Surface
  2. For the Create Solid option to become available you will typically use the Mutual Trim option as you’ll trim the existing surfaces removing the excess to create the closed volume.
  3. With Mutual Trim selected I’ll pick the surfaces I want to mutually trim, in this case the two surfaces.
Mutual Trim surfaces selected

Mutual Trim surfaces selected

  1. Next use either the keep or remove surface selection option depending on how you want to select the surfaces for the enclosed volume. For this example I’ll use keep surfaces, so I’ll have less selections to make.
  2. Pick in the selection box below the option before picking surfaces in the model otherwise you’ll deselect the trimming surfaces!
  3. In the graphics area I’ll select the surfaces I want to keep, note the three preview options in the PropertyManager for showing and hiding your selection[s]. In this example the top and bottom of the button are selected.
Surfaces Selected

Surfaces Selected

  1. Having selected the surfaces AND an enclosed volume is present from the selections you should be able to pick the Create solid option at the foot of the PropertyManager (if the option is disabled then you’ll likely not have an enclosed volume and additional surfaces may be required to create the enclosed space).
Create Solid from Surface

Create solid from Surface

  1. Pick OK and you should now have a Surface Trim feature at the foot of your FeatureManager design tree that has generated a solid model
Surface Trim Solid

Surface Trim Solid

I’ll apply the section view again so you can see in the figure below the enclosed volume space is now filled as a solid (blue colour). As you can see converting Surface into Solid takes less steps in SOLIDWORKS.

Section Solid

Section Solid

Using SOLIDWORKS Boundary Surface

The Boundary surface feature works in the same manner. When you are applying a boundary surface and it creates an enclosed volume like the one shown in the example below, the create solid option will be available and the feature will combine the group of surfaces into a solid, essentially removing the Knit surface step you would have taken in a previous release:

Surface de délimitation

Surface de délimitation

En savoir plus sur le surfaçage

To gain a better understanding of converting Surface into Solid with SOLIDWORKS you should take our SOLIDWORKS Surfacing training course either online or in a classroom near you.

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Rod Mackay

Rod utilise des logiciels de CAO 3D depuis plus de 25 ans et a formé des milliers de concepteurs à une utilisation plus efficace de leurs systèmes de CAO. Rod est le webmestre de Javelin et est basé à Ottawa, ON, Canada.