By Cory Holden
When using 3D sketching tools it can often be very difficult to get the exact curvature that you want for your sketch. One way to make this process much easier for the designer is to use the intersection curve sketch tool. This tool is very powerful in helping you generate a complex 3D sketch in the sense that it allows you to visualize what will happen ahead of time. For instance, you can visualize the intersection points and predetermine the 3D sketch that will be created.
To start off, this tool can be found in the SOLIDWORKS menus under Tools > Sketch Tools> Intersection Curve. This feature requires you to have intersecting solid or surface geometries to be used. Personally, I find it most effective to use two surfaces in the example demonstrated in this article, and this was determined after testing both methods. The second method that could be used instead of intersecting surfaces is intersecting solid bodies. This particular case limits what you can do with the Intersection Curve feature because you do not have as many visible faces to select to get a more specific sketch geometry. By using the surfaces approach it leaves a lot more visibility during creation of your 3D sketch. Also the solid bodies approach will require you to have two close profiles that can be extruded into solid bodies, whereas using the two surfaces you would not need to have a closed profile. Therefore, the possibilities with the intersecting surfaces approach would be limitless. If you ever do decide to use the intersecting solid bodies approach keep in mind that they do have to be separate bodies that intersect and the easiest way to achieve this goal is to turn off the merge results option in the extrude feature.
This picture represents the two intersecting surfaces approach, and as can be seen from the picture there was one profile drawn in a front view and then extruded using the extrude surface feature, and the same process was followed with the sketched profile in the right view. The surface extrudes were both over extended just to ensure that they fully intersected at all desired points.
In the picture above, upon choosing the intersection curve feature, it asked me to select the faces of which I desired for the intersection 3D sketch to be drawn from. Since I only want to two top complex rails of my frame drawn from these profiles I only chose the top faces that were involved (highlighted in blue in the picture). This also allows me to quite easily limit the scope of my 3D sketch and really focus in on the specific areas I need a 3D sketch to be created. Also, this step of the process is very helpful allowing me to visualize what will happen next, as you will see in the picture below the planes give you a visual representation in the current state of what your 3D sketch will look like.
Next, once my faces were all selected I hit the green check to accept the feature. Upon doing this SOLIDWORKS places a 3D sketch right where all of the blue selected faces from above intersect. I left the extruded surfaces unhidden in the picture above so you can really visualize what the intersection curve feature is doing and how it is placing the 3D sketch.
The result is this sketch for the upper part of my car frame which would have been very complex 3D sketch geometry to create manually with 3D splines and other 3D sketch tools. Both the front sketch profile that I used to do the surface extrude as well as the right sketch profile were both under defined. Even though those early steps were just rough profile drawings and under defined the intersection curve feature has created a fully defined 3D sketch.
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