Reduce, Reuse, Recycle Your Sketches

Reduce, Reuse, Recycle Your SketchesBy CAPINC Applications Engineer, Laura Weismantel

One of the ways you can save time while building a model in SolidWorks is to never model the same feature twice. There are many tools that can be used to achieve this objective, such as the patterning and mirror commands. Something else that can help you with the same objective is to reuse your sketch geometry instead of re-drawing same or similar geometry as you build your part.

Popular techniques used to recycle sketch geometry are the Convert Entities and Offset sketching tools. The Contour Select tool can also be very helpful when you want to use the same sketch for multiple features. But these tools, however convenient, are only useful when the geometry you want to reuse lives with the same location and orientation to the rest of your model and the only difference is planar depth. What if the sketch entities you need to recreate should be at a different orientation to the part or even another part altogether? You may be thinking “Impossible!” but you couldn’t be more wrong.

There are three tools that can be used to accomplish this objective, two of which will be discussed here. Depending on your needs in reusing the sketch, you may decide to either create a derived sketch or perform a simple Copy/Paste operation. The key difference is a derived sketch will remain linked to the original sketch geometry so if you change the original sketch, the derived sketch will update, as well. This link can be broken, but it cannot be repaired. Using the Copy/Paste function, you can capture the old sketch geometry (copy) and then paste it on whatever face or plane you want. You are then free to make whatever changes you want to the sketch because it is no longer associated with the originating geometry. Also, sketches can be copy/pasted from one part to another and they do not have to have any real relationship to each other. Derived sketches can be used on different parts, as well, but only if they both live in the same assembly.

Copy/Paste Sketches


  1. Select the originating sketch by clicking on it in the feature manager.
  2. Copy the originating sketch by going to the Edit menu in the Menu Bar and selecting Copy. You can also use the Ctrl+C Windows command.
  3. Select the target face or plane for your new sketch.
  4. Paste the sketch by going to the Edit menu and selecting Paste. Like in step 2, you can also use the Ctrl+V Windows command. The sketch will be pasted in the approximate location you clicked on the plane or face.
  5. Edit the new sketch to fully define it.

When you use Copy/Paste to reuse a sketch one thing you need to pay attention to is the way the original sketch is constrained. If the original sketch is defined using horizontal and vertical constraints, keep in mind that those relationships may be different in the sketches new location. Horizontal constraints may need to be changed to vertical constraints, and vice versa. Switching these relationships in a complicated sketch may prove to be rather time consuming. In anticipation of pasting a sketch onto a new face or plane, you should eliminate as many horizontal and vertical constraints as possible in the original sketch. This can be done by replacing all horizontal and vertical constraints with perpendicular and parallel relationships. You may wish to keep one piece of geometry defined as horizontal or vertical in order to fully define the sketch. Know where this relationship is and be prepared to replace or redefine it in the new sketch.

In the first sketch of the lightning bolt, notice how many horizontal relationships there are. In the second image, I’ve replaced all of these relationships by making the lines perpendicular to the single construction line, which is defined as being vertical. When I paste this sketch later I know that if I want to change the angular orientation of the sketch, the only constraint I may need to remove is the vertical constraint on the construction line.

Reduce, Reuse, Recycle Your Sketches

You should also be aware that any dimensions or relationships to outside geometry (ie: model edges, reference geometry, other sketches, etc.) in the originating sketch will be omitted from the new sketch when it is pasted. This will result in under-defined sketch geometry that you can then choose to define any way you want. This includes any relationship made to the original sketch origin and will result in the user needing to define the exact location of the sketch in the new sketch plane.

Derived Sketches


  1. Select the originating sketch by clicking on it in the feature manager.
  2. Hold the Ctrl button to multi-select the plane or face for the derived sketch to be created. If done correctly, the sketch and the plane or face should both be selected at the same time. This is the only way to access the Derived Sketch command.
  3. With both items selected, go to the Insert menu in the menu bar and choose Derived Sketch. If this command is not available for selection, it means you do not have the proper items selected from steps 1 and 2.
  4. You are automatically placed in the sketching environment so that you can give the derived sketch proper location and orientation.

Unlike with the Copy/Paste procedure, it does not matter whether or not you use horizontal and vertical constraints in the originating sketch. None of the dimensions or relationships in the original sketch will be visible or accessible in the derived sketch. If you try to create a dimension that would define the shape of the derived sketch you will receive an error message stating “Only dimensioning between a model entity and a sketch entity is allowed in derived sketches”. This is because the only dimensioning allowed is for the purpose of defining the sketches location within the new sketch plane.

Derived sketches do give you some freedom to rotate, translate and even scale the original sketch geometry. Go to Tools > Sketch Tools > Modify… to open the Modify Sketch dialogue box:

Reduce, Reuse, Recycle Your Sketches


To perform an operation using this dialogue, enter the desired value for change into the appropriate field and press enter. This makes the change to the sketch and keeps the dialogue box open until you are finished. For example, if you wanted to rotate the model by 90 degrees you would enter “90” in the Rotate field and press enter. Pressing enter a second time will rotate the model another 90 degrees. While the Modify Sketch dialogue is open you can also mirror the sketch by hovering the mouse over the black origin temporarily created on the sketch. Right clicking on the x-axis of the origin will mirror the sketch over the y-axis. Alternatively, right-clicking on the y-axis will mirror the sketch over the x-axis.

Reduce, Reuse, Recycle Your Sketches

Once the location of the sketch has been determined by either constraining or dimensioning sketch geometry, it will turn black, indicating that it is fully defined. If at some point you wish to break the relationship between the original sketch and the derived sketch, you can right click on the derived sketch in the feature tree and choose the “Underive” option. As stated previously, once a sketch is underived, it cannot be reconnected with the original sketch.

You can create a derived sketch in a separate part from the original as long as they live in the same assembly. This can be convenient for creating male/female geometry in coupled parts. Keep in mind that this will result in external references from one part to another, but as long as those parts maintain that relationship, the features created from the derived sketches will always match.

In conclusion, SolidWorks gives us many ways to reuse geometry, whether that be on the feature level or the sketch level. Depending on what you want to do with the geometry, you may choose to Copy and Paste a sketch or create a derived sketch. If you find you are doing either of these operations using the same sketch over and over again, you may consider taking advantage of the third method for recycling a sketch by creating a sketch block. A sketch block is like a sketch you keep stored in a your design library and reuse anywhere you’d like. You can choose for the inserted block to be linked to the original so that it updates when the original is changed or you can break the link so that you can edit the block on a case-by-case basis. The discussion of sketch blocks would be an extensive one, so we will save that for future Tech Tips. Stay tuned!

Categories: SOLIDWORKS, SOLIDWORKS 2013, Tips & Tricks, Web/Tech
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