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How to Offset a Surface in SolidWorks?

In SolidWorks, the Offset Surface tool is used to create a new Surface body that is at a distance from the selected set of faces/surfaces. This tool is frequently used for advanced surface modeling. It can also be used to create a shelled body or any form of wrap.

Not to be confused with the Offset on Surface tool which is a 3D sketch tool used to offset model edges and faces on a surface.

1. Click Offset Surface tool present in the Surfaces toolbar or go to Insert Surface Offset.

2. In the PropertyManager, in the Surface or Faces to Offset input box, select all the surfaces or faces in the graphics area that you want to offset.

Tip: You can also select an entire solid/surface body or the entire model by using the Box or Lasso Selection. Left-click and drag to highlight the area and all the faces will be selected.

3. In the Offset Distance input box, enter the value of offset that you want. Use the Flip Offset Direction button if you want to offset the surface in the reverse direction.

Tip: You can also create an offset surface with a distance of zero. You may notice that the tool will change its name from Offset Surface to Copy Surface but that does not affect any functionality of the tool itself. An Offset Surface command of zero is used more frequently than you think.

4. Click Ok and offset surface(s) will be created. Hide your solid body if the surfaces are not visible. To hide a Solid body all you have to do is right-click on the solid body in the graphics area and click on the Hide icon or you can expand the Solid Bodies folder present in the FeatureManger Design Tree and then right-click on the body that you want to hide and select the Hide icon.

Where can I use this tool?

The Offset Surface tool has a lot of use cases. Listing them all is beyond the scope of this article but we will list a few.

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1. To find the volume of an open body such as vases, pots, etc or to find the internal volume of a hollow solid body.

For example, consider this solid body that is shelled internally.

Now, in order to find out what is the volume of air present inside this body, you can do the following:

  • First, use the Offset Surface tool to create an offset of all the internal faces at an offset distance of zero. Use Section View to select internal faces easily. Make sure that you select all the internal faces so that the surface body encloses a closed volume. Otherwise, you have to use Surface tools to manually close the holes in the surface body to make it airtight.

  • Next, hide the original solid body.

  • Then, convert the surface body you created using the Offset Surface tool into a solid body. You can use any of the methods listed in this article to convert the surface body to a solid body. For this example, we will use the Thicken command. Ensure that the Create solid from the enclosed volume option is checked. And we need this body as a separate solid body so make sure that the Merge result option is unchecked.

  • Go to Tools-> Evaluate ->Mass Properties or click on the Mass Properties feature present in the Evaluate toolbar.

  • In the Mass Properties dialog box, right-click in the input box and select Clear Selection to remove the already selected entire part.

  • Now select the solid body that you made by converting the offset surfaces either from the graphics area or from the Solid Bodies folder present in the FeatureManager Design tree. And there you will find the volume of the solid body which is equal to the internal volume of the original shell body along with much other useful information.

2. To shell a body.

Many a time the Shell feature may fail because of many reasons. You can use the Offset Surface tool to create the shell.

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3. As an alternative to the wrap feature.

Sometimes, when using the wrap feature you may find that the shape of the wrap is different than your sketch or the placement/position of the wrap is not what it should be ideally. In this case, you may use this particular set of tools to obtain a better end result:

  • First, use the Split Line tool to use your sketch to split the surface into multiple faces.

  • Then use the Offset Surface tool to offset these faces with an offset value of 0.

  • Then use the Thicken or Thickened Cut tool to either create an emboss or deboss as per your requirement.

  • And your end result will be similar if you have used a wrap feature instead.

4. To remove interferences between parts in assemblies.

For example, take a look at the below assembly where we modeled a hook in a different part file and positioned and oriented it on the main body.

But if we run the Interference detection tool, we see that the hook is overlapping with the main body by a lot.

And since the main body has an organic shape, there is no easy way to remove this material. So you can follow these steps to eliminate the overlapping in these cases:

  1. While in the Assembly, select the body from which you want to remove the overlapping martial and click on the Edit Component icon. You can also access Edit Component from the Assembly toolbar. In our case, we will remove material from the hook.

2. Next, use the Offset Surface tool to create an offset of zero of the surface that you will be using as the cutting surface.

3. Next, use the Cut with Surface tool to cut your solid body with the offset surface you just created. If required, use the Flip Cut icon to flip the direction of material removal.

4. And voila, the parts are no longer overlapping. You can now hide or delete the previously created surface body.

What to do if the Offset Surface tool throws an error?

Offset Surface tool may fail because of the following reasons:

  • One of the faces/surfaces you selected to offset has an area with a radius of curvature that is less than the offset distance. To find the minimum radius of curvature, use the Check tool present in the Evaluate toolbar or go to Tools -> Evaluate -> Check
  • The surfaces/faces, if offset will self-intersect or interfere with nearby faces.
  • The offset surfaces are not connected.

When the Offset Surface fails, you will get an error message like shown below. The good thing is SolidWorks will automatically identify which faces failed to offset.

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Tip: Sometimes, using a smaller or larger offset distance may remove the error.

Once the identification process completes, all the failing faces will be highlighted in yellow. You can select them individually and remove them or use the Remove All Failing Faces to remove all of them in a single click.

Click OK. You will notice that there are some gaps that are caused by the faces that you removed because they were causing the offset to fail. You can repair these gaps by manually adjusting the offsets of the failed faces or using the Surface tools such as Delete Hole, Filled Surface, Lofted Surface, or Boundary Surface to recreate them.

How do I offset a surface without creating a new surface body?

If you want to create an offset of a face/surface but do not want that offset surface to become a new Surface Body, then you may want to use the Move Face tool. Click on the Move Face command present in the Direct Editing toolbar or go to Insert -> Face -> Move to use the tool. Then use the Offset mode to offset all the surfaces/faces you want. Note that this command also moves all the other faces that are connected with the selected faces so as to maintain the design integrity.

And that’s it. We hope that this article helped you learn how to use the Offset Surface tool in SolidWorks. If you have any questions or suggestions, feel free to leave a comment down below.