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Direct Editing in SOLIDWORKS


Direct Editing in SOLIDWORKS

When modeling in SOLIDWORKS, much attention is paid to the structure and order that sketches and features that are created in, which make up the “design intent” of the model. This order and structure should allow for easy design changes and automatic updates of downstream features on a well put-together CAD model.

But what if a model has no features? Such is the case for imported models (such as .STEP and .IGES) which can benefit from Direct Editing techniques. The Direct Editing toolbar, visible in Figure 1 below, can be enabled by right clicking an existing tab of the SOLIDWORKS command manager (such as the Features tab) and choosing “Direct Editing.”

Figure 1. Direct Editing Command Manager toolbar.

Another great use case for direct edits is at the end of a feature tree to apply clearances to otherwise “nominal” dimensions.

In a pinch, direct edits can also be used to modify native SOLIDWORKS parts that suffer from poor structure or design intent. However, it should be noted that using direct edits in this way will only make the model structure more fragile and difficult to understand for other users. If you feel like you are relying on direct edits as a crutch, then it is likely that the proper solution is to put in the time to restructure the model with better design intent.

For users coming from traditional sketch-based features, direct editing can be a bit puzzling at first. The aim of this article is to demystify the time and place for each major feature. It is also worth noting that despite directly modifying faces of the geometry, these direct editing commands are still history-based, producing features in the feature tree that can be suppressed, rolled back or parametrically edited—they just pay no mind to existing sketch dimensions and constraints in the model.

Move Face

The Move Face feature enables “pushing” and “pulling” existing faces of the model—the first thing that often jumps to mind when thinking of direct edits. It features three options: Offset, Translate and Rotate.

In Figure 2 below, the Move Face feature with Translate can be seen being used to adjust the position of a slot on an imported model. Note that all faces of the slot must be selected.

Figure 2. Move Face: Translate.

In this case, a blind end condition is being used to move the slot a specific distance, but there are also other end conditions, such as “Up to Surface” and “Up to Vertex” to allow extending features up to another geometry reference.  

Note also that the Move Face command produces a feature in the feature tree. This means that features created by direct editing commands can still be suppressed, rolled back / reordered or have its dimensions accessed for editing or configuration.

It is only possible to perform one type of movement at a time, so if it is necessary to both translate and rotate geometry, this must be done with two consecutive Move Face features.

Rotation using the Move Face command is visible in Figure 3 below to change the bend angle of a flange on an imported sheet metal part. It may be necessary to define a rotation axis to perform the rotation about, which in this case was as simple as creating an axis referencing the bend arc.

Figure 3. Move Face: Rotate.

The offset option in Move Face allows shrinking and growing the size of existing features, in a direction normal to the existing faces, as visible in Figure 4 below.

Figure 4. Move Face: Offset.

The offset mode of Move Face can also be used to increase or decrease the thickness of models, such as the imported sheet metal file below in Figure 5.

Figure 5. Offsetting imported sheet metal.

Delete Face

The Delete Face command, particularly when used with the “Delete and Patch” option, is indispensable for removing features from imported geometry and simplifying models. As visible in Figure 6 below, selecting a group of chamfers with delete and patch will extend the surrounding faces and form the sharp corners that would have been present there before the chamfers were applied. The same can be done to remove fillets back to sharp corners.

Figure 6. Delete and Patch: Deleting fillets or chamfers.

Aside from removing fillets and chamfers, delete and patch can be used as an alternative to manual extrudes and extrude cuts to remove holes and unnecessary details such as engraved text and other small features.

Figure 7. Delete and Patch: Holes or slots.

For troublesome parts, delete and patch may be used as an intermediary step to simplify the geometry enough to allow a move face feature to execute.

Patterning Faces

For features of an imported part that needs to be arrayed or repeated, the face selection options inside the pattern types in SOLIDWORKS can be useful. Figure 8 below shows a linear pattern of an existing slot in a featureless file by selecting the slot faces.

Figure 8. Patterning faces.

Face-based patterns such as this are also useful in traditional modeling workflows if the intent is to pattern only some subsection of a feature.

Split & Move/Copy Body

The Split Feature and Move/Copy Bodies feature can be used together to accomplish complex model changes through a multistep process.

Figure 9. Split Feature.

Split requires selection of a cutting tool, which can be a plane, surface or sketch. Clicking the “Cut Part” button and checking the checkboxes under the scissor icon will produce separate solid bodies.

Figure 10. Splitting the model.

Once the bodies are separated, the Move/Copy bodies command allows for separating the two bodies. Similar to the Move Face command, translation and rotation can be performed in separate steps as separate features.

Figure 11. Bridging material.

Finally, traditional sketches and extrudes can be used to “bridge” the material back together into a single solid body part.

While the end result of the model change in Figure 11 above could have been accomplished by a Move Face command, the splitting and bridging technique opens up other possibilities such as rotating the separated body and Lofting or Sweeping the bridge between them.

For a more in-depth look at the Move Face, Delete Face and Split techniques consider the video guide Direct Editing for Imported Models.

Troubleshooting Direct Edits

When using the move face feature, it is crucial to select all the faces that need to move. This may sound obvious, but in practice is easy to overlook. Observe Figure 12 below, comparing two alternate selections in a move face translation.

In the image on the left, the chamfers are not included in the selection. In the resulting preview, a hint at how the move face command works can be seen: the surrounding chamfer faces are extended using the existing face data that is present in them. In this case, this is not the intended design change, and the image on the right shows that with the chamfers included in the selection the size of the entire ledge can be extended.

Figure 12. Move Face Troubleshooting: Incomplete selections.

More practically, missing a face or two in a direct edit selection can cause the feature to fail outright and give a puzzling rebuild error. There are a few things that may cause a direct edit feature to fail, but incomplete selections are one of the most common.

Thankfully, there are selection tools that help automate selection of faces, using the Select Connected Faces popup toolbar when initially making a selection in the move or delete face commands, visible in Figure 13 below.

Figure 13. Select Connected Faces toolbar.

Aside from incomplete selections, faulty faces in the model can prevent direct edits or any other type of modeling feature from successfully generating.

As faulty faces are more common on imported files, Import Diagnostics is a valuable tool to identify and repair them, as visible in Figure 14.

Figure 14. Import Diagnostics.

Note that if an import was performed with 3D Interconnect enabled, it will be necessary to “Dissolve Feature” on the imported model to break the external file reference before Import Diagnostics can be performed.

If no faulty faces are present or the model is SOLIDWORKS native, and all the proper selections are present, then it’s possible that there isn’t enough information in the surrounding faces for SOLIDWORKS to perform the move.

This is a common failure for situations such as offsetting a fillet inward, once the offset is great enough it exceeds the radius the offset will fail. These types of issues can be identified at least by testing smaller offsets and trying to identify the problem area.

Problem areas (such as fillets) may be removed with the Delete and Patch command and then added back on after the move is performed.

For complex surfaces and organic shape geometry, it is possible to run into outright limitations with the Move Face command. The performance will be related to how cleanly, and the manner in which, the surfaces were constructed and how much underlying data they contain. But if a failure occurs trying to move or delete and patch a complex surface, the only reliable fallback is to resort to manual surface modeling tools.

Direct Edits and Drawings

One reason direct edits may not be suitable for a production CAD file is their effect on drawings. When using Imported Annotations or the Model Items tool to import dimensions onto the drawing sheet, any dimensions in the base sketches will not represent the final state of the geometry.

If the drawing is detailed using manually created Smart Dimensions, then this is not of much concern.

Geometry Comparison

There are a couple of geometry comparison tools available in SOLIDWORKS, but the new Body Compare functionality added in all versions of SOLIDWORKS 2020 and newer has the most utility for comparing imported files.

Notably, it is capable of comparing solid bodies against surfaces and even mesh file types such as STL, making it a valuable tool for comparing revisions of imported bodies.

Figure 15. Body Comparison in SOLIDWORKS 2020.


Direct editing features such as the Move Face and Delete Face command can be useful to modify and simplify imported models or to perform final adjustments such as adding clearances to SOLIDWORKS native CAD files. The features themselves still produce a model history that can be edited, configured or suppressed.

Failing direct edits can be troubleshooted by ensuring proper face selection, testing a smaller offset and inspecting the base geometry for faults.  Understanding how and when to use each direct editing feature opens up a variety of possibilities not available in conventional modeling workflows. 

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