A Kanban is part of a system used to control logistics of inventory in a production environment and is commonly used to achieve JIT (Just In Time) manufacturing goals. In addition to the powerful capabilities of SOLIDWORKS to design products, it can also be used to streamline manufacturing environments. This example is going to take a look at designing a simple Kanban rack system that is parametrically controlled by just a few key dimensions. The model employs the use of Top-Down assembly modeling techniques.
The model is controlled by a 3D sketch in an assembly that represents the centerlines of the tubes and is governed by 4 key dimensions – the height of front and back legs, and the depth and width of the rack system. The 3D-Sketch is coincident to the top plane and is oriented such that the origin is in the center so the front and right default planes pass through the center of the rack. This particular system has the back legs longer than the front, however, you can set this up in any configuration you want.
I modeled up a variety of connectors and placed them in a folder which I then created a link to in the Design Library of the Task Pane. The few connectors I modeled up in SOLIDWORKS provide me with a good variety of connection possibilities and are based on readily available products used for this purpose. Having the connectors in a file linked in my Design Library keeps them at my fingertips for dragging into my assembly.
The general workflow for this model is a simple, 3-step process:
- Create the 3D-Sketch in an Assembly File.
- Place connectors in the assembly and mate them to the 3D-Sketch as appropriate.
- Insert as a New Part and create the tubes in the context of the assembly based on and related to the connectors.
The first connector is placed in the assembly and mated to a leg of the 3D-Sketch with a concentric mate. A second connector is then added to the opposite leg and aligned to its opposing connector. The cylindrical faces highlighted in the image are selected and a concentric mate is chosen to align them. These connectors will then be used to control the size and placement of the tube that will join them together.
Once two connectors are mated to the 3D-Sketch and oriented facing each other, it is time to insert the tube that will join them. It is important to note that when designing using Top-Down modeling technique, the designer must choose New Part from the drop-down menu below Insert Components on the Assembly Command Manager. When a New Part is created in the context of the assembly, the first step is to select a plane in the assembly that will hold the in-place mate to the new part. In this example, the Right plane in the Assembly is selected (this action results in a sketch being created on the Front plane of the new part and the environment changes to editing sketch in edit part mode which is indicated by the blue highlighted component in the assembly feature manager tree). To create the profile of the tube, select the inner diameter of one of the connectors and click Convert Entities and offset that circle to the desired thickness of the tube.
The connectors are designed so that the tube will be inserted into the connector to a depth of 30mm. Once the profile is created, the tube will be extruded in both directions with end conditions that are offset from surface a distance of 30mm inside the connector. Reverse Offset will need to be selected so the end condition resides inside the connector. Notice in the image below, the end face of the connectors is chosen as the offset surface. Once this is complete, the tube will grow with changes made to the 3D-Sketch.
The legs are added into the model, again by Inserting a New Part, but this time the Top plane in the assembly is selected to place the new component. The tube profile is then created on this sketch and extruded with an end condition Up To Vertex, with the top corner of the 3DSketch selected as the defining vertex.
This process is continued throughout the model:
- Place the connectors in the assembly mating them to the 3D-Sketch.
- Orientate them facing each other.
- Create the tubes in context of the assembly related to the connectors they join.
In order to create the shelf, connectors are simply mated to the existing cross tubes. Due to the placement of the 3D-Sketch in the assembly, it is easy to use the Front and Right planes for mirroring shelf components. In my assembly, I created the bottom shelf with all of its connectors and tubes and grouped them in the feature manager tree in a folder. I then patterned the contents of the folder to create more shelves. As I change any of the four dimensions, the entire model updates accordingly. Ahhh the joys and satisfaction one gains from a clean parametric model! Happy Kanban!
A video that demonstrates the techniques in this blog can be found here.