SOLIDWORKS Trim Entities Command Capabilities

When removing sketch entities in SOLIDWORKS, deleting a specific portion can require extensive cleanup and adding additional sketch entities. However, the Trim Entities command will automate a lot of the busy work and allow you to trim or extend entities in your sketch in one single operation. This article explains, in-depth, uses of the SOLIDWORKS Trim Entities command and provides an overview of all the different selection options. 

Power Trim

The first and most versatile option within the Trim Entities command is Power Trim. Power Trim allows users to delete and extend individual segments of their sketches. What makes the Power Trim command unique from the standard deleting process is its ability to dynamically create new sketch entities. 

As you can see below, if you delete the line going through the center, the entire line will be deleted, including the overhangs on the side. 

However, if you instead Power Trim the center, the original line will be automatically segmented, and the lines on the side will be given a new relation to locate them in the sketch. 

To use the Power Trim command, launch the Trim Entities Command from the CommandManager and ensure Power Trim is selected in the PropertyManager. 

Left-click in the graphics area and drag your cursor to begin trimming any entity the dotted path touches. A red square will appear wherever the last entity was trimmed. Releasing your left click will allow you to start a new selection. 

The Power Trim option allows for efficient edits to sketches without having to redraw the horizontal, vertical, and construction lines.

Power Trim Extension

If you wish to extend a sketch entity, it may seem easiest to draw another sketch entity at the end to lengthen it. However, that new extension will also need its own dimension to be fully defined, and this can both complicate dimensioning work and make further design changes more difficult. 

Thankfully, the Power Trim command can also be used to extend sketch entities. With the Trim Entities command open and with Power Trim selected, left-click the sketch entity to extend, and move your mouse to either side of the entity to preview how the extension will look. 

Once the direction and magnitude match your design intent, left-clicking again will add the extension and create a new sketch entity combining both.

Corner

The Corner option within the Trim Entities tool allows you to extend two sketch entities until the point they would naturally meet in a corner. 

From within the Trim Entities Command, select Corner in the PropertyManager and choose the entities you wish to connect. After left-clicking one of the entities and hovering over the second, a preview will display the expected new geometry. 

Note: The Corner tool will both trim and extend entities to make the corner, so any overhang will be removed. 

Trim Away Inside/Outside

Power Trim is a very powerful tool for deleting or extending sketch entities, however, it can often be too broad a brush for more detailed sketches. The Trim Away Inside/Outside option allows you to select a region to trim entities from, reducing the chance of accidentally deleting elements you wish to keep. 

To use the Trim Away tool, select the Trim away inside or Trim away outside option in the PropertyManager. 

For the Inside option, select two sketch entities to be the outside boundaries of the region; left-clicking on any elements contained within these boundaries will be deleted similarly to the Power Trim. 

In a similar manner, selecting the Outside option will only allow you to trim entities outside of the selected region. 

The images above show the difference between Trim away inside and Trim away outside options using the two vertical lines as the boundary region. 

Trim to Closest

The final trim option in the Trim Entities command is Trim to Closest. Trim to Closest is a simplified version of Power Trim, but instead of drawing a path to delete sketch entities, you can instead left-click specific sections to delete them while preserving the other sketch geometries. 

The main advantage this gives over the regular Power Trim is that it allows you to precisely click entities instead of dragging, reducing the chance of accidentally deleting other entities in complex sketches. 

Options

Two option boxes at the bottom of the PropertyManager change the behavior of the Trim Entities command: Keep trimmed entities as construction geometry and Ignore trimming of construction geometry.

If you want to keep a reminder of which entities have been trimmed or wish to have another sketch entity attached to the same point, selecting the first box will convert all trimmed entities into construction geometry instead of deleting them.

Also, if you have already converted some entities into construction geometry or if you have existing centerlines or other construction geometry, you can ignore trimming of construction geometry so you do not accidentally remove them with the Power Trim. 

Conclusion

The Trim Entities command is incredibly versatile and provides varied options to remove or extend sketch entities in a sketch. Use the Power Trim to quickly clean up a rough drawing and remove a line in the center, or get more specific with the Trim to Closest if the sketch is too complex to drag your mouse. 

The ability to delete these entities while preserving design intent and definition states makes this tool incredibly adaptive and useful for large sketch changes. If you have any questions regarding the Trim Entities tool or SOLIDWORKS in general, please reach out to GoEngineer.

Want to Learn more?

Take your SOLIDWORKS skills to the next level. In our SOLIDWORKS Essentials training course learn how to use SOLIDWORKS to build 3D parametric models of parts and assemblies and prepare drawings of those parts and assemblies.

I hope you found this article showcasing the capabilities of the SOLIDWORKS Trim Entities command helpful. Check out more tips and tricks listed below. Additionally, join the GoEngineer Community to participate in the conversation, create forum posts, and answer questions from other SOLIDWORKS users. 

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