If you are working with a Multi-Body part file, you may find yourself in a situation where you no longer need a solid/surface body. So to keep the geometry clean you can either hide that Solid/Surface body or you can delete it.
To hide a Solid/Surface body all you have to do is right-click on the solid/surface body in the graphics area and click on the Hide icon.
Another way to hide a body in SolidWorks is that you can expand the Solid Bodies or Surface 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.
Hiding the body is, most of the time, a good idea because if you further need that body downstream you can just unhide it. However, it is extremely recommended that you do not do that if you don’t know how to use Feature Scope. Also, there may be times when hiding the non-required body is not always a good idea. For example, let’s say you imported a file with hundreds of Solid and Surface bodies but you only need a few bodies. In this case, you would be wise to delete the unwanted bodies as not only it will make the file size smaller but it will have a huge impact on the performance of SolidWorks. Also if you want to send the file to someone else, it’s a good practice to delete the unwanted bodies so that the person receiving them doesn’t get confused with all the extra bodies.
Well, technically speaking, while it may seem that you can delete a body, what actually happens is that the body is not deleted, it just becomes inaccessible to you. The reason behind that is that SolidWorks is history-based CAD software. This means that you can always use the Rollback bar to go before the feature that you used to delete the body and voila, you will find that the body is still there.
There are multiple ways to delete a body in SolidWorks. In this article, we are going to show you all the methods that you can use to delete your body whether it’s a Solid body or a Surface Body. For example purposes, we are going to use a Headlight combination of an Armoured Vehicle which is made up of 5 Solid Bodies as you can see in the Solid Bodies folder in the Feature Manger Design Tree.
1. Using the Delete/Keep Body Tool:
The Delete/Keep Body tool is solely used to delete or keep one or more surface or solid bodies.
1. Select the Delete/Keep Body tool present in the Direct Editing toolbar or go to Insert -> Features -> Delete/Keep Body.
2. Next under the Type menu, select what kind of operation you want the Delete/Keep Body tool to perform:
- Delete Bodies: Select this option if you want to specify the bodies that you want to delete. In the Bodies to delete input box, select all the solid or surface bodies that you want to be removed.
- Keep Bodies: Select this option if you want to specify which bodies you don’t want to delete. In the Bodies to keep input box, select all the solid or surface bodies that you don’t want to be removed. All the bodies that are not selected will be deleted.
Tip: This command is useful when there are a lot of bodies that need to be deleted and only some need to be kept.
3. Click OK and a Body-Delete/Keep feature will appear in the Feature Manager Design Tree. You can edit this feature if and when needed.
2. Using CUT commands:
Note: This method cannot be used to delete Surface Bodies.
1. First, we created a Sketch for Extrude Cut feature that fully encloses the frame.
2. Next, we used Through-All in Both Directions to make sure that the Extrude-Cut will cut through everything.
3. The most important step in this method is to select the right body in the Feature Scope. In Feature scope, you have to choose Selected Bodies and then ensure that the Auto-select option is not checked. If it is checked you will not be able to specify which body you want to cut. Next, in the Solid Bodies to Affect input box select the body that you want to delete from the graphics area.
4. Click Ok and your solid body will now be removed.
3. Using Save Bodies:
The Save Bodies tool is commonly used to save any solid body in a different file from a Multi-Body part. But you can also use this tool to delete a body. Again this method also can’t be used to delete a Surface Body.
1. To access the Save Bodies PropertyManager, right-click on the Solid Bodies folder present in the FeatureManager Design Tree and select Save Bodies. Or go to Insert -> Features -> Save Bodies.
2. You will find all of your solid bodies listed in the Resulting Parts table. Select the bodies that you want to delete. You can select them either in the graphics area or from the table itself.
3. Make sure that the Consume Cut Bodies option is checked as it will allow the Save Bodies command to remove the selected bodies from the current file while moving them to their new files.
4. If you want that all the bodies that you are saving, to be automatically included in a new assembly file with the same position as they are in this part file, then click on the Browse button provided under the Create Assembly menu, and a Save As dialog box will open and then enter the name of the assembly and the assembly will be created and opened automatically.
4. Click OK and all the bodies you selected will now be opened in a new window as separate part files and the original part file will no longer have those bodies.
Note: The separate part files saved by the Save Bodies command are linked to the original part. This means that if you use the rollback bar to roll above the Save Bodies feature and then change anything in the solid bodies that were saved, these changes will be reflected in those separate part files.
And that’s it. We hope that this article helped you learn different ways to delete a body in SolidWorks. If you have any questions or suggestions, feel free to leave a comment down below.