Hi. I’m Mike Dady, Application Engineer for Alignex. A few months ago, I was having dinner at a friends’ house when I was given a wine glass that piqued my SOLIDWORKS interest. The glass had a set of spiral grooves machined on it’s exterior. My engineering brain immediately began wondering how I would go about recreating this exact design within SOLIDWORKS & SOLIDWORKS CAM. Let’s take a look at how it works.
After some review, it turns out we can do it all using the SOLIDWORKS CAM Standard package that comes with every license of SOLIDWORKS on subscription support. The first step on our journey is establishing the path needed to cut the groove in our Part. The varying diameter of the glass is the complicating factor to this process. There are multiple solutions that can create the path needed, but the most versatile is using Solid-Surface Hybrid Modeling. This creates an Intersection Curve that will update as the glass geometry changes. To learn more on this process, check out ‘Mastering Parts and Features’ in the Training Section of the Alignex web site.
Now that the modeling has been completed, it’s time to machine the groove using SOLIDWORKS CAM. Our first step will be to create a Configuration that has the grooves Suppressed. This new configuration will be used for the machining stock by using a Part File in the Stock Manager. Pick the current Part Model, and then choose our stock configuration to complete the process.
To machine our groove we’ll use a Curve Machining Feature. Right away we see another reason the Intersection Curve is the best solution for our groove path. We’ll re-use it in SOLIDWORKS CAM to create our machining feature. Once the curve is selected, move on to set the depth of the feature. With the machining feature complete, we’ll create an equally spaced Pattern to machine the second groove, and then create the Operation.
Our next step is to change the Operation setup to properly machine the grooves. Currently the Operation is using a Flat End Mill and that will not work. Normally, we would customize the Technology Database ahead of time to add the tool for machining the grooves. Today, we’ll create a custom tool on the fly. Everything starts by adding a keyway tool into the Tool Crib from the Library, and then the Tool is selected for use in the Operation. It doesn’t matter what size keyway tool is added since it will be customized to match our groove diameter. We have to make sure our Tool Diameter and Overall Length are large enough for cutting the lower section of the glass. The Tool Protrusion also needs to be adjusted in the Holder definition. It’s a good practice to use the Tool preview in the graphics window to check for interferences.
Next up is adjusting the Contour Side Parameter Allowance. The current value will have the tool only trace the outside of the glass. We need to adjust the allowance to match the groove depth using a negative value to cut into the glass.
The last Operation change will be modifying the Lead-In and Leadout to match our model. The overlap will need to be removed or our groove will be too long. Make sure the Leadout length is large enough to prevent the tool from crashing while retracting due to the undercut. Now that all our modifications are complete, we can create the Toolpath.
To verify everything is setup correctly, we’ll Simulate the Toolpath to review everything. This will let us know if there are any interferences with the Tool or Holder, and let us review our final machined geometry.