With SolidWorks being a muilt-window application, there are a few tricks you can do with multiple windows tiled using drag and drop. As you may already know, selecting features from one part and dragging and dropping them into another part to copy them is a feature that has been around for some time now. This is where the technology for the current Design Library and the old Feature Pallette originates. This works for mating parts to an assemby that are open simultaniously within SolidWorks by selecting the edges or faces, holding control and drag and droping till your index finger falls off.

Circular edges, on the other hand, have a uniqueness when it comes to drag and drop mating. Grabbing a circular edge, with a drag and drop, mates the circular part coincident and concentric (2 mates) in one shot. But it goes one mate further when a circular pattern resides on both the mating part and the target assembly, assuming the patterns match. As illistrated to the left, selecting the upper part’s circular edge and dragging it into the lower assembly containing the base and dropping it on the edge will mate the lid to the base coincident and concentric. In addition, it will automaticaly align the seed holes of the patterns and allow you to clock the alignment by tapping the TAB key. So in this case, 3 mates are added in one drag and drop action!

This can be further automated by adding a mate reference to the outer circular edge. Mate references can add this automatic mating technology to parts without having to open them to select the edge on a drag and drop. It will tell SolidWorks to do this automatically so you can drag and drop your parts directly from Windows Explorer with the same result! ~Lou

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

Do you remember the old auto explode from the earlier versions of SolidWorks? It was rare when it worked but might be an asset with simple assemblies. Well, there is a great embeded command in eDrawings that can help you when you need to explode an eAssembly. The best part is that this tip works even when it was published without an exploded view. To do this all you need to do is a CTRL E and your assembly will auto explode similar to the old Auto explode in SolidWorks. Learned this tip a few years ago at SolidWorks World Conference.

When it comes to FEA analysis there are 6 steps that will be followed regardless of the package you use. These are:
1. Geometry creation - Many of us will be using SolidWorks for this but can be imported geometry.
2. Materials - Specify this in SolidWorks or within COSMOSWorks. Another great resource is matweb.com.
3. Boundary Conditions - Applies the restraints and forces that are being applied to the part. This tells the solver what exactly the geometry is experiencing.
4. Mesh - Breaks the geometry into small pieces (best analogy is LEGOS)
5. Run - Run the solver. This takes the above 4 steps into consideration in order to calculate stress, strain and displacement, etc.
6. Results - The entire goal of the analysis. Quantative part of the procedure which begins the design verification process.

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