* This is one of a series of modeling challenges you can use to test your SOLIDWORKS skills. First, read the challenge and try to figure out a solution on your own. Then, compare your solution with my good, better, and best recommendations. As always, feel free to share even more tips and tricks in the comments below.
Modeling, measuring, and modifying native SOLIDWORKS files is easy. Most of the really fun modeling challenges arise when working with imported geometry. All you’re typically given to start off with is what we call a “dumb solid” – just a hunk of digital mass with no intelligence (i.e. parametric feature history). Sometimes you’re even left at the mercy of another CAD system’s inferior export quality. This can be troublesome, because what one CAD system may consider cylindrical, SOLIDWORKS may not.
For example, imagine importing what looks like a simple sheet metal part file, using the Convert to Sheet Metal tool to flatten it, and then realizing it won’t work because the bent faces aren’t perfectly cylindrical. The only workaround is to replace the filleted faces with true cylindrical faces. Here’s how to do it:
- Use Copy Surface (Offset Surface with an offset value of 0) to copy the flat faces
- Use Delete Body to delete the original imported solid
Expand the solid body folder, select the body, and click the delete key to quickly activate this tool
- Use Extend Surface to fill the gaps of the removed filleted faces
- Use Face Fillet to bridge between the surface bodies with a perfectly tangent transition
- Use Convert to Sheet Metal to convert the surface body to a sheet metal solid body
- Now you can use the Flatten command to display the flat pattern
So that’s a pretty cool tip, but that’s not the modeling challenge for this post. I skipped a step between #3 and #4. First you need to know the size of the fillet before you can model it. Since imported models don’t have feature dimensions, the challenge is – how do we measure imported fillets?
Most of us know you can use the Status Bar (the informational text shown in the bottom right hand corner of the SOLIDWORKS interface) to display measurements of select edges and faces. Most of us also know if you select a circular edge, the Status Bar will report a radius. This can help in situations as shown on the left end of the model below. The problem is that when selecting an edge that isn’t perfectly normal to the direction of the circular profile, all the Status Bar will report is an Arc Length – no help when trying to measure a fillet. So what do we do when neither edge of a cylindrical face is normal to the profile of the fillet? SOLIDWORKS solved this problem in 2015 when we added the ability to display a radius value when selecting a cylindrical face. It’s a pretty simple solution that you definitely want to be aware of!
Normal Profile Sketch
The last solution works for cylindrical faces, but what about fillets that are applied to a curved edge (i.e. fillets that aren’t cylindrical)? In these cases, we’ll need to create a circular profile to measure. Here’s an easy way to do so:
- Select the vertex and the edge of the fillet and then create a sketch
By preselecting a vertex and an edge before creating a sketch, SOLIDWORKS automatically generates a plane coincident to the vertex and normal to the edge and activates a new sketch on that plane all in a single step
- Select the filleted face and then create an Intersection Curve
And Intersection Curve will generate a sketch entity at the intersection of the selected face and the active sketch plane which will create a circular arc normal to the profile of the fillet
- Select the resultant arc to display the measured radius in the Status Bar
Even with those nifty shortcuts, that last tip still took too many steps for me. It also wouldn’t have helped us with our original imported sheet metal example that didn’t contain fillets with exact radii. That leads us to our final solution. It’s actually way too easy, but it’s also commonly overlooked and neglected, which is why I felt compelled to write this post. To measure any fillet in any condition, all you have to do it fire up the Curvature Evaluation tool and hover over the filleted face. SOLIDWORKS will display a live measurement of the curvature directly under your mouse. That’s all there is to it!
If you create models with a ton of different sized fillets, this is also a great way to make a quick final inspection to make sure all of your fillets were applied correctly. Enjoy!