I’ll be adding a weekly version of Freebie files. Enjoy
{post has been updated with correct files and corrected spelling}
https://drive.google.com/file/d/1KfvkGrlymFxijmgD2_VaS8eX2mN_HbB9/view?usp=sharing
This is for the tons of people asking how to make a stacked text sign, or a text over text vcarve.
This is the first of the 2, with a vcarve over text sign. This is the easier of the 2 signs to make and gives you a sense of accomplishment.
This is a file that uses 3/4 thick stock, but i use a flat depth of .125, so 1/2 inch thick stock would work just fine.
This starts with a 10″ x 2.5″ thick piece of 3/4 thick wood. this also translates will to larger signs, such as over the door with width of 28-30 inches. These can make good desk signs and office decor.
This is the part you need to pay attention to. The wood needs to be flat. Not kind of flat, but flat. The spoil board needs to be flattened, and your machine needs to be trammed. If these are not done, please youtube how to and start there. Nothing is more frustrating than getting 1/2 way done or more and starting to vcarve the top letters and some are too deep and the others are too shallow. you can fix it to a degree if you have not removed your work, but there are limits to how well this will work.
if you are looking for a good video, Winston Moy has one that deals with Shapeoko 3 tuning: squareing, spindle tramming and more. As usual, his videos are good and they give you a lot of extras due to his engineering experience.
https://www.youtube.com/watch?v=P4VverLXpCI&t=1s
If you have material not flat, either plane it down, or get a friend with a planer to flatten it. if you don’t, it will be trouble. you can do this with your cnc, but remember, if it is a solid board, you may cause it to warp. Induced stress, cutting on one side, can cause it to pull towards one corner. For this reason, i’m a fan of hardwoods that are dry(use a moisture meter) and that are cut and glued up in strips, with alternating grain.
This will give you the best chance of not warping. And then when project is being finished(paint or clear poly), do both sides. Don’t allow moisture to affect one side more than the other.
Now, back to the project.
This work is done in aspire, but is the same in vcarve. This file starts with 2 sets of text. The first is a Text “FAMILY” in a layer called edit bottom txt. I use this to store the bottom text as text and provide a place to edit this, so that this file becomes a template file. This text is in Times New Roman, 1.6 inches tall, and stretched to 9 inches long, using set size. This is centered in the workspace.
The next text is “Family is a gift that lasts forever” in a layer called edit top text. This font is 1/2″ tall, using the font Monotype Corsiva. I’ll include this font in the zip file. This text is also centered in the workspace.
I now copy a the text from edit top text to a temp layer called temp. All layers should be off except temp, and it should be active. I will convert this to text to curves. Right click and select convert to curves. Now All layers should be off except temp, and it should be active. CTRL A to select all vectors, as we converted this from text we can edit to vectors. will the text selected, click on offset. make sure create shart offset corners is not selected, and delete original is selected. offset .1 inches outwards.
you should look like this (i turn my temp layers red, to remind me to move after)
turn on edit bottom layer txt and right click on and copy to layer temp. Turn off layer edit bottom layer txt.
Right click on text FAMILY and convert to curves.
With SHIFT pressed, select all letters, except the inside of the leter A and any of the inside of the clouds around the letters. (inside and outside).
Now click on weld. You should be something like this.
Do a CNTL A and select all. right click and copy to new layer, temp 2. On layer temp(temp 2 off, layer temp active), delete the inside of the letter A. Now select all and weld this together
now turn off temp, activate temp 2 and turn temp 2 on. temp 2 layer should be the only layer on.
We still need to take care of the letter A. Select the inside small part of the letter A, then with shift key down, select the cloud around it, and click on subract(next to weld). Holding down Shift, select the 2 pieces (or more) on the inside of the letter A. Right click and copy to layer temp.
Turn on only layer temp. CTRL A and select all. Right click and copy to new layer, Bottom Toolpath. Activate Bottom toolpath and turn everything else off. Draw a box 9.5 wide by 2.5 tall. Center this on your page.
Turn off all layers and turn on edit top text. CTRL A and select all Text. Right click and copy to new layer top toolpath. Turn off edit top text and turn on top toolpath. Make Top toolpath active.
CTRL A and select all Text. Right click and convert to curves.
Turn on top toolpath and bottom toolpath and all other layer off.
You are now ready to make toolpaths. Switch to toolpaths.
without selecting any vectors, click on vcarve toolpath.
set start depth 0, flat depth 0.125, vbit as tool, 60 deg. .25 inch. Use flat area clearance tool, .125 or .0625 em. raster, climb, ramp pluge moves 1 inch.
Now for selection of vectors. click Selector near bottom of page. Closed, associate with toolpath, layer bottom toolpath. If you use a bit setter on a Shapeoko, make sure and set tool numbers. I use the number order they run in. I named my toolpath, vcarve 60deg .25 .0625 em. It creates a pocket for the .0625 and a vcarve for the 60 deg .25 vbit.
Now select vcarve toolpath again. 0 start depth, no flat depth, tool vbit 60 deg .25, then selector for vectors.
Closed, associate with toolpath, top toolpath. I’ve named this toolpath vcarve top 60 .25 vbit.
time on mine shows 35 min. most of that is the .0625 bit, but it is my favorite small bit and it will cut with the best of them. likes to go fast, not slow. slow and it shows it getting very hot. speed it up in inches per min and it sounds better and cuts like butter.
Now you have a template file to do this later by deleting everything in the layers except edit bottom text and edit top text. Then change text and away you go. If the toolpaths are still there and you don’t delete the layers, you can calculate and away you go with out all the drama of setting this up. quick to do when doing production work.
PRO TIP. When running toolpaths, use the bit setter or if you don’t, use the same location on your board and do a paper method on your z axis zero. It will give better