When I used to give SolidPlant demonstration, there is a feature "3DGrid" which is used to create a grid for weldment structure in plant design. I wondered that there has to be similar functionality in Solidworks too. That's when I came across "Grid System" feature. No it is not "View Grid"!
This feature is available at Part as well as Assembly level. In assembly when you invoke grid system, Solidworks will automatically create a new part by "New part" (under insert components). This will be a virtual part and then automatically enters into "sketch mode".
Let's explore its functionality and I must Solidworks can do more justice by adding much more functionality to this feature.
I would press "S" shortcut key as I hate to remember command's location and search "grid" and click on "grid system" feature. Its icon differs with "grid view" by replacing "eye" with "3D".
2. As soon as you click on the feature, by default it will start sketching on Top Plane. If you want to start sketching on different plane, then you need to preselect the plane and then select the feature.
3. I am drawing certain geometry and exit the sketch. In the property manager, you can find option to assign number of levels and subsequent distance from the levels.
3. I have entered 4 level at 250 distance. Now the interesting thing to note is that when you expand grid system feature, you will realize how multiple operations were bundled under one to save your time!
4. At any time you can go back and edit the feature for distance and add or remove levels. Now, you might wonder that this are disconnected and to connect all the sketches I will need to create a line one by one? Yes if you use traditional weldment feature but don't need to create sketch. Here is the catch.
5. Expand the surface bodies folder, you might notice that surface bodies are hidden. Unhide the surfaces and now it looks as shown in image below. All you need to do is select all edges of surface extrude and use convert entities under "3dSketch" feature. Hide sketches from the heads up toolbar to save from unnecessary selections.
6. Now, when I said "yes" while using traditional weldments then when I don't need to create the sketch? Use "structure system". It allows you to use edges, planes, sketches, points, intersection of planes in order to create the weldments! 🙂
So that is something "Solidworks help" wouldn't have helped you with.
Happy learning!
