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It is common place to stamp or etch machined parts, so they can be identified easily on the shop floor. As many users know, SOLIDWORKS has a sketch tool that can be used as the basis of modeling a feature like this: Sketch Text. Sketch Text is a fairly simple tool that can lead to a wide variety of results! It can support practically any TrueType font, and more can be installed. The tool even has a selection box to accept curves!
I’ve put together this small example of some text going along a spline. Let’s try to extrude this text to see what happens. When we hit the check to accept, we get this message:
This message is pretty clear. There are intersections somewhere in our soon-to-be extrusion. When we inspect the sketch text further we see the issue. The word “spline” is on the inside bend of a curve, so all the letters are bunching up and causing intersections, shown in red in the figure below.
So normally when we encounter this message, we have 2 options: either pick a contour from the intersecting regions or fix the sketch so that it doesn’t have intersections. Let’s try the first option!
If you click into the “selected contours” box on the property manager then try to click the sketch text, you find that nothing happens. That’s because Sketch Text is a little bit different than your regular sketch entities. Due to the nature of TrueType fonts and how they are rendered, SOLIDWORKS is not directly able to calculate the intersections of each of the letters.
Let’s go for the second option: fixing the sketch. As many of us know, a good way to take care of intersecting contours is to use our trusty trim tool. But you may have noticed, if you try to directly hack away at it with the trim tool, the text seems to be immune to that too. The reason is the same as above: we can’t directly calculate the intersections. What are we to do?
Notice my wording from before: While we can’t directly work with it, that doesn’t mean we are out of options! TrueType fonts work by storing an outline of each character in a font file as Bezier curves. Wouldn’t it be nice to extract these Bezier curves? As it turns out, there is a specific command to do that: Dissolve Sketch Text.
To access the command, right click on the sketch text itself (wait for the font “A” to appear next to your cursor), and the Dissolve Sketch Text command will be in that menu:
At this point, you will notice that all the contours became shaded (if you’re running 2017+, that is). The curve data was converted to SOLIDWORKS Geometry! Most of the time, it uses splines to approximate the shape of the letters, but we can see that this blocky font turned into a bunch of lines. SOLIDWORKS considers these as just regular old contours and so they are subject to practically all the sketch tools available to us, including Trim!
Let’s do just that! Grab your Trim tool, and you will find that you can finally slice through the parts of the letters! Make it such that the intersections are no more! A good way to check if this was done correctly is see if the contours are shaded. If you have the option enabled, and the contour is still not shading, something is wrong with the intersections of the sketch. Otherwise, Repair Sketch is your best friend! You can see how mine came out below.
Once you are certain that the intersections are removed, head back to the extrusion tool (or whatever tool you were trying to use sketch text for).
You should now find that your text extrudes with no problems! Keep in mind that once you dissolve sketch text, you will not be able to resize the font, or change the font itself for that matter. It is as if you had sketched it; the command just makes a handy shortcut. Hopefully, that helps with your texting woes!
Thank you for following along!