 In this tutorial, we will show you how to manage design intent and how to apply face-related commands and solve it. In synchronous modeling in SOLIDGE, you have so much control over the 3D model itself that there is no need to go back to the sketch. In SOLIDGE, you can make changes to a 3D model face rather than a sketch. Let's just start by opening a new isometric part. Draw an 80x40mm rectangle on the XY plane and use the steering wheel to extrude the sketch 20mm. Let's add 4 6mm rounds to the 4 corners of the rectangle. Finally, let's draw 2 7mm circles somewhere on the top face of the model and make 2 holes using the extruded cut command. The placements of the holes do not matter at this time as we will use the face-related commands to move them to the right position later on. Now, let's see the design intent relationships in action. If you select the right side of the model, we can extend it using the steering wheel. SOLIDGE recognized that we made the original rectangle symmetric with respect to the origin, therefore it's keeping the symmetric design intent for us. You can decide if you want to modify the model this way or turn off the symmetric design intent from the design intent panel. There are many other design intents that SOLIDGE can recognize including coplanar, concentric, or even tangent. You can learn more about the design intent panel by pressing the question mark. We did not align the holes to the right place when we placed them. From a history-based modeling perspective, we need to go back to the sketch and modify the original sketch we used to make the holes to put them in the right place. However, what if I delete the original sketch? In history-based modeling, that would be a big no-no. In SOLIDGE, using synchronous technology, you can use the face relay commands to position the holes concentric to the center of the rounded 8. From the face relay section, choose concentric, then simply click on the hole, right-click to accept, and then select the round. We can repeat the same process for the second hole. These relationships can easily be deleted from the Pathfinder. Finally, let's make two rectangles on the top face of the part. Use the rectangle by two point commands and hold left-click and drag to make these two rectangles. You can select the reasons and press down on the arrow to make a cut, but we need the cuts to be coplanar. Using the coplanar face relay relationship, the faces can be made coplanar. Just select coplanar relationship, click on one face, right-click, or press enter, then click on the other face. Now the faces are coplanar. Now, if you click on a face-to-extent, not only SOLIDGE recognizes symmetry, it also keeps the rounds intact and recognizes the newly added concentric relationship. In this video, you'll learn about design intent in SOLIDGE and face relay commands.