For an old feature, vary sketch still gets a lot of praise from those that use it. It can be very useful when wanting to use a linear pattern but need to have some adjustment happen on some of the instances. The picture to the left shows what happens when you take a seed (thru cut on the far left) and propagate it without the vary sketch option using a linear pattern along the bottom edge. Vary sketch can adjust the cut but it requires some design intent in the sketch geometry to work properly.

When you create the sketch for the feature you are going to pattern, you need to make sure that the sketch has a feature that will adjust as it patterns. For example, the top part seed feature is an offset of the spline shape of the top of the part. This allows the top of the part to adjust as the feature’s horizontal locating dimension is changed.

The trick to using the vary skech option is that instead of selecting the bottom edge of the part as the direction vector, you would select the locating dimension of the seed feature. In the example picture, the locating dimension to use would be the dimension that locates the leftmost side of the seed feature to the left most edge of the part. Once you select this you will see the preview of the linear pattern as you would if you selected the bottom edge. Now check the vary sketch option. You will notice that the preview will dissappear and I believe this is a bug, which I have submitted but has never been fixed! Anyway, when you click on OK you will notice the following result (picture to the right). This option tells SolidWorks to pattern using the locating dimension as a driver to change the sketch as it would by changing the dimension. If you haven’t seen this feature before it can be an eye opener! ~Lou

This is a followup post to episode 92 when I discussed 3D sketches in SolidWorks. As I mentioned, many people don’t realize that you can extrude or cut with a 3D sketch as long as it is closed and it has a vector direction to extrude along. As you can see, selecting the 3D sketch will be a contour that creates a fill surface and your direction can use a linear edge or sketch. It will essentially perform a directional sweep but this direction option can be useful for 2D sketches as well, in the event you don’t want to extrude or cut normal to the sketch plane.

I also mentioned that you could use this to cut a free form directional cut into a complex surface using the spline on surface command. This command can be found under Tools, Sketch Entities, Spline on Surface. Once launched, the command will begin a 3D sketch and allow sketching on a complex surface, which will automatically reference the spline points coincident with that surface. Once finished, sketch a straight line in the vector direction of the cut, which could be within the same 3D sketch, or select a linear edge of the part. Now launch the Cut Extrude tool and select the straight line as the direction component and select the spline on surface as the cut contour.

This is one of those features that may come in handy for those obscure applications so I thought I would add a visual aid to follow the podcast. By the way, in case you were curious, this was added back in SolidWorks 2004. ~Lou

Obviously you can create a 2D sketch on a face or a plane, but did you know you can also select an edge? When you pre-select an edge and insert a sketch, SolidWorks will create a plane perpendicular to edge at the endpoint closest to where you select and open a sketch on it automatically. Read the rest of this entry »