The power of Move Face in SOLIDWORKS!

Editing geometry created in the SOLIDWORKS model is usually easy, but what if the geometry belongs to an imported model from some neutral file format?  Even if the model were created in SOLIDWORKS, sometimes modifying the geometry gets tricky, such as when adding draft.  For situations like this, there is SOLIDWORKS Move Face, one of the most convenient and underrated commands in the software…to reference the work of George R. R. Martin, Move Face might be worth more than all the gold in Casterly Rock!  😀

Where to find the Move Face command

Found on the Direct Editing tab of the Command Manager, this simple command is in my opinion one of the most underrated tools in SOLIDWORKS.  The Direct Editing tab may not be shown by default, so right-click any other tab to show it.  Or, use Command Search to initiate a Move Face command.

Where to find the Move Face feature

Offset Face

Let’s resize this hole in an imported sheet metal part, using SOLIDWORKS Move Face > Offset.  The preview is in yellow:

Resizing a hole using the Offset option in Move Face. Note that the Parameter value is actually the radial change, so multiplied by two will be the diametric change.

Translate Face

What if we want to move that edge flange?  We’ll need to pick up all the faces that are to be moved in that particular direction (right-click one of the outer faces > Select Tangency is great for the outer shape), and use Move Face > Translate:

Moving an Edge Flange using the Translate setting.  Can use the Copy checkbox if we want to create a second tab from the first.

Adjusting Draft Angles

Now let’s use the SOLIDWORKS Move Face to solve a draft challenge:  how to modify the draft angle of the two faces shown below to make them steeper?  The Draft command is limited in the range of draft angles it can produce, so we’ll look to Move Face for a solution.

Our objective is to increase the draft angle of these to faces. Move Face is ideal for that.

We’ll start by chopping the model in half, and finish by mirroring the half-body back onto itself, to take advantage of part symmetry.  After all, doing the work twice is not efficient.  Using Command Search, we press the “S” key and started typing the first few characters of Cut with Surface.  Selecting a suitable plane to bisect the model, we end up with half of the original solid body as shown below.

Rotate Face

To adjust the draft of that face, we’ll use the Rotate setting of Move Face, but this requires an axis of rotation, and there are no useful straight edges bounding that face.  We can pre-select these two vertices below, and add a Features > Reference Geometry > Axis:

In half of the original body, added a reference Axis through these two vertices

…and then run Move Face > Rotate:

With the Rotate function of Move Face, will need to select an axis of rotation

Lastly, we’ll mirror the body back onto itself, to take advantage of part symmetry:

The finished part, with modified draft at the bottom of the pockets

Learn more with SOLIDWORKS Training

Learn more tips and tricks in our SOLIDWORKS Sheet Metal training course, and our SOLIDWORKS Advanced Part Modeling training course.