Using Sketches to Rip Sheet Metal Parts

The ability to use sketches to rip sheet metal parts may be one of the most important features, especially when importing solids. The rip feature used to only be able to rip linear edges on the part. However, as you can see in the example to the left, this would not work since the bottom is missing gaps to rip by. Instead of going through the effort of using a complex cut feature to add the gaps you can simply use sketches. This technique will only work if the sketches terminate at verticies on the part. Notice in the example how each of the sketch entities start and end at verticies on the part. The sketches do not need to be separate for each entity either. In this case the four entities are all within one 2D sketch on that bottom face. Now you are ready to insert your bends! First, you select the fixed face and then scroll down to reveal the Rip Parameters. and select on the edges and sketches that rips can be added to. It is good practice to make sure the rip edges are sharing verticies so in the example to the right notice how the sketch entity and the model edge are setup. Selecting the inside edge may cause issues when trying to perform a rip like this. Now you can flatten your part properly without having to perform a ton of preprocessing procedures. ~Lou

Changing The SolidWorks Toolbox Flag

I have talked about this tool before in the podcast but I thought I would take the opportunity to show the interface of this little data utility in order to bring a level of clairity to the table. This tool is located in the installation directory under Toolbox/data utilities. Once inside of the data utilities folder you can launch the sldsetdocprop.exe by double clicking on it. This will popup the Set Document Property dialog box.

This tool was made to alter the toolbox flag that is recognized by both SolidWorks and PDMWorks Workgroup. Many times users want to take files from the toolbox and modify them and check them into the PDMWorks vault. If your vault settings are set to exclude the check in of these documents, even if you moved your modified Toolbox part to another location, PDMWorks will not allow check in of this document because of this internal flag. In order to remove this flag, selection of the Property state from "Yes" to "No" will now allow this file to be seen as any old SolidWorks file. On the flip side, you can take your standard SolidWorks files and change them so they are considered to be a Toolbox part when in an assembly or inside of PDMWorks. The tool also allows a nice bulk update interface by adding files and/or directories as well as a filter for file types. Once you have added all the files to modify in the update window, click on the "Update Status" button and the flag has been changed! ~Lou

Auto Align And Mate Hole Patterns

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

Automatically Vary A Pattern

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