How did you create the stencilized version? Do you have to manually edit each character individually, or is there a trick that I’m not aware of? (Actually I am certain that there are many tricks that I am not aware of, but let’s limit ourselves to this particular topic…)
(Sigh) - I was hoping that wasn’t the answer, but kind of knew that it was. Oh well, another learning opportunity!
I’m trying to make new struts for my larger build with the words “Big Red LowRider 3” in the D3 Roadsterism font. I am figuring out (slowly) how to get rid of the trailing extensions after the “g”, “d” and “3”, and how to remove the islands from the “B”, “g”, “R”, “e”, “d”, and “o”.
Since I struggled a bit to figure out how to do the stencilizing (is that a word?) of the font, I figured that I might leave behind a brief tutorial for the next hapless soul that wants to attempt it.
To create the editable text items
Download the D3 Roadsterisnm Long Italic .ttf file from here (or myriad other web sites).
Add the font to WIndows (Settings - Font Settings - Add Fonts - drag and drop downloaded .ttf file)
In Fusion go to Solid - Create menu, select Create Sketch (select the XY plane)
In the Sketch - Create menu, select Text
Create a “bounding box” by clicking on two diagonal corners (Make sure it is large enough to contain your text - too small and it will create multiple lines of text)
In the Text sub-window, select the D3 Roadsterism Long Italic font. You don’t need to select the Bold or Italic icons (unless you want to, I guess)
Select the desired text size (I started with 40mm, but you can scale it later)
Enter your desired text in the “Sample Text” section of the Text sub-window (don’t try to type the text on the sketch itself, certain letters will act as function keys)
Use the Align Center and Middle buttons to center the text in the bounding box
Click OK
Important - before finishing the sketch, right click on the text and select Explode Text. This converts the text to shapes that can be extruded (it will not extrude unless exploded). Note that the letters are now converted to a series of lines, arcs and faces.
Finish the sketch, select all of the newly created text shapes. You will have to de-select all of the islands in the O, R, D, e, etc. using the CTRL key
Extrude the selected text items (I used 2mm, thicker might be easier to edit later). Note that each word will be a separate body, and items like the dots on lower case i’s will also be separate bodies.
To remove the trailing section on the last letters of each word (if desired):
Rotate the view to show the back (extruded) face of the text on an angle.
Highlight the back face of the trailing section and delete.
Rotate the view to see and select the lower right edge of the character that you just edited.
Use the Fillet tool to round off the lower right edge of the character (3 mm radius)
To create the stencil section for islands:
Create a Construction Plane on the top face of the extruded text
Create a sketch on that construction plane
Create closed shapes using Lines in the desired location for each stencil bar. I drew a line starting on the top line of each island as a reference point, continued the line straight (no angle) to the left until it was clear of the character, continued a second line down about 3mm (staying clear of the character), then a third line to the right until it is inside the island (staying parallel with the first line), then lastly a fourth line going back to the starting point.
Use the Dimension tool to set the distance between the top and bottom horizontal lines to 3mm (or different based on your text height).
Finish the sketch
Use the Extrude tool to Cut the newly created box(es) and create the stencil supports.
Use the Fillet tool to round off the corners where you cut the characters (1.5mm radius). You may have to select and fillet more than one edge on some corners.
Ahh sorry, due to bandwidth issues I’m late to this party too, I can’t check but I’m pretty sure I uploaded a dxf to Printables on the logo model download - if I get back to it I’ll link it here.
that should save a few steps - I’d just extrude it in 'Fusion then do as you did more or less.
