I have a project I need to cut a 1/8th" by 9/32" slot in a piece of .230" plexiglass along a line. I'm using a 1/8th" bit. The path should be centered on this line. Trying the center cut tool I could not find a way to set the slot width. Is there any? Can the depth of cut be set directly and not have to try to figure out what percent of .230 is 1/8th" deep? Thanks Bruce
When I need a specific depth I do a two stage drawing On one copy I do the lines that need a specific depth. On another copy is all the general depth stuff. On drawing one, set the cuts to be 100% depth. Then for each depth you need, set the material thivkness and generate gcode. Note that you can select a single line and only that line be be generated. So you can do many different depths if you need to. Once you have all the files you need, use the gcode joiner to join them into one cut file. This video shows the process in more detail
There is no way to set the width on a line cut, it always uses the current bit. There are 2 ways to cut your slot: 1 - add a parallel line each side of your centerline, 0.078" way. This will result in a 9/32 slot. make sure all three lines are set to 100% depth, then use the method outlined in my previous reply to set the material thickness to the depth you want. You can add the parallel lines with the measure tool. 2 - instead of a centerline, draw the entire slot as a rectangle (centered on the line you have), then use the pocket tool to create the cutlines. You may want to extend the ends or add dogbones if you want something rectangular to plug into the slot. If your line is more complicated than just a straight line as I have used above, then drawing the parallel lines can be done with a simple trick. Sketchup has an offset tool, but it will only work on faces. So connect the ends of the line with a temporary line/lines to create a face, then use the offset tool to add an outside and an inside offset 9/64" away from the existing edge. Now you can delete the temporary lines and clean up the ends, then pocket the resulting shape.
Craig, thanks for your answer. When faced with a percent of depth rather than a direct entry, sometimes you just can't think of the mathematical formula to arrive at the percentage. Not really hard. I'm learning you have to keep a calculator open working in Sketchup. David, remind me again when the material thickness is applied? When the cut is created in a drawing? Or when the G \code is generated the material thickness is applied to all cut depths? I had figured out the width work around of using two path cuts. I'd hoped there was a easier way. Thanks for the help and the work on the software. Bruce
Material thickness is applied when the Gcode is generated. That is why all other depths are percentages! This way you can cut 'half way through' any size material just by changing 1 number.
David, I get the genius in the percentage working no matter the thickness and I suppose there is application for that. However wouldn't it be more genious to be able to enter either? A percentage would be followed by a % otherwise its an absolute depth cut for example. Here is the circular slot I was trying to cut. The slot was to hold a brush. This is a router dust boot. Here is my solutions for this situation based on what I learned. On the top example the slot is 9/64" wide requiring two cuts of the 1/8" bit. The inside face was created with the offset tool to 9/64". Then an inside cut of 100% was applied to the outside or larger face and an outside cut of 100% applied to the inside or smaller face. On the lower example the slot is 1/4" wide. In this case the pocket tool will not work. Instead I again used the offset tool to create the inside most face. Since the slot is wider than twice the bit I also created a face between the inside and outside. I then applied an inside cut to the outside face, a center cut of 100% to the center middle face and last an outside cut to the inside face. Using Davids technique I'd have to cut either of these in a different G-code file with the material depth set at what ever depth I'd want the slot. I've not tested this but believe it would work. Do you agree David? Thanks for all the help Bruce
It will work fine Bruce, but you are wrong when you say the pocket tool will not work. As of version 1.4c, it will work. The top cut is 9/64" wide and is just a process of select pocket tool press HOME to select FLOOD mode (read the help!) hold CTRL and clic That insert the 2 offset lines you see in my drawing. Since they are less than 1/8" apart there is no need to insert a zigzag. The bottom slot is 1/4" wide and is a CTRL-click as above then a 'click' to insert the zigzag. Of course you can either set a precise percentage depth, or set it to 100% and use material thickness to get the depth you want.
